Top Solid'Design [PDF]

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Welcome to TopSolid'Design Help Version 7

We thank you for choosing TopSolid 7 ! TopSolid 7 is the ideal application to answer your computer-aided-design needs. Thanks to its intuitive and impressive interface, you will be able to model your parts, assemble them and create any type of draft. You will also find specific tools to create sheet metal parts and their unfolding, core cavity blocks and injection mold design. You can access the online help for the current command at any time by pressing the F1 key on your keyboard or by clicking on the icon displayed in the upper right corner of the commands dialog box.

Screen presentation

The TopSolid 7 screen consists of different zones allowing you to manage projects and documents:

1 2 3 4 5 6 7 8 9 10 11 12

TopSolid button System toolbar Context and Menu Tabs Dialog Window Document Tabs Context Commands (Work Bar) Banner Context States Entity Window Options Window Operations Window Dialog Area

1 - TopSolid Button

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Search, change and request/approval tabs Compass Workspace Visualization and Rendering Bar Scale Bar Project Management Window Project Tabs Preview Area Visualization tolerances Tools bar of tree Measurement Parts window

This button, also called the Application Icon, allows you to access commands for file management, editing, display, document visualization windows, PDM management and exiting the software.

2 - System Bar This icon bar groups frequently used TopSolid commands: Open Current Document, Save All Documents, Print, Undo, Redo, Stage Change and Refresh. Contrary to the context icon bar, it is not customizable.

3 - Context Tabs and Menus This area displays the entire set of available commands. The contents of this menu depends on the type of document being edited, as well as installed add-in modules. Right-click the text of a context tab to display context icons on the Work Bar found just below. This bar contains the most frequently used commands of the menu (you can also change the toolbar by placing the mouse cursor in this area and turning the wheel, if the mouse has one). Left-click the button (or right-click the tab text) to scroll the menu. Commands are split into sub-menus that can be accessed by clicking the arrow found at the right of the text (you can also click the text with the right mouse button).

The icon on the right of the Home tab or the F11 function key allows to display the document without the icons bars and trees .This mode allows to work using the contextual menus, and the keyboard shortcuts. The menus are displayed when the cursor hovers the document tabs. This menu bar can be pinned to be always visible.

4 - Dialog Window This area displays when the name of a command ends in "..." (such as, for example, the Sketch > Line... command). It allows you to enter different information that performs the selected command. By default, the dialog window displays in the upper-left area of the workspace, but it can also be displayed in the form of an anchored tool window with the TopSolid > Display > Dialog command (click it to turn on the mode). The top of the dialog window consists of an icon bar allowing you to perform basic commands: OK

Cancel Help

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Validates the dialog and executes the current command when all necessary data is entere is missing, this button is grayed out. You can also run the validation by right-clicking and s icon from the popup menu or pressing the Enter key on the keyboard. Closes the dialog without running the current command. You can also close the document clicking and selecting the icon from the popup menu or pressing the Esc key on the key Launches the online help of the current command. You can also launch the help by pressi on the keyboard. Activate or not the preview of the command result. This option is only available for some co (surfacic commands, hollow, thicken, trim, ...) which needs a lot of system resource. Perform increased by deactivating the preview. Allows you to select the operation mode of the command. If the thumbtack is in, the comm automatically restart after use, which allows you to concatenate, for example, multiple fille relaunching the command. However, if the thumbtack is not it, the command only works on When certain commands function like wizards, the Next and Back icons allow you to go fo in the stages.

In dialog, the size of the displayed lists can be set with the contextual menu. Automatic size: The list changes from 4 to 8 lines according to its contents. If the number of lines is higher than 8, a scroll bar appears. Possibility to fix the number of lines. This dialog is done dialog by dialog, it is saved and proposed when opening again this dialog. If the number of lines is higher than the entered value, a scroll bar appears.

Example: Set of the number of lines in the Shape > Repetition command. The dialog can be displaced in the graphic area by dragging the title. The different sections of the dialog can be temporary closed by clicking the icon in the circle.

5 - Document Tabs This area contains the list of open documents; each document is open in a window with a tab containing the name and icon of the type of document. It can also be followed by symbols that describe the status of the document: Symbol *

Document Name: Window #

Example

Document Status Modified Document. Document containing an invalid operation or item. Left-click edit the 1st invalid operation. Document for which the operations tree cursor was lowered see the part or assembly in a previous state. Left-click this ic the cursor to the top of the tree. Document open in several windows.

When multiple documents are open, the tab of the current document has an orange background. Furthermore, in the right part of the window, the icons allow you to respectively display the list of open documents in order to select the new current document and close the current document.

The popup menu of tabs allows you to access document (Save, Vault, Close) and window (Tile, New Window, etc.) management commands. You can quickly close a document by clicking on the document tab with the middle mouse button (wheel). Tabs can be reclassified by dragging them horizontally. You can slide a tab to the workspace to create a new window.

6 - Context Commands (Work Bar) The command bar contains the most frequently used commands of the chosen context. Selecting a command generally triggers the display of command options in the Dialog Panel. Commands are displayed in the left part of the context, whereas states (or modes) are displayed in the right part.

You can change the toolbar by placing the mouse cursor in this area and scrolling the wheel, if the mouse has one.

7 - Banner The banner displays the name of the current document, as well as information related to the type of PDM used. In Local Mode, the Local PDM information displays, in Client/Server Mode, the name of the connection as well as the user name between brackets displays.

8 - Context states States (or modes) allow you to set the options of the current context, select the mode when the icon is on an orange background (orange is the default active color and can be configured in the Window feature of the Tools > Options... command). For example, in the Sketch context, Construction mode allows you to define the construction type for the items created next.

9 - Entities window

10 - Options window

11 - Operations window

12 - Dialog Area The dialog area displays messages that guide you through each command. The right part contains the coordinates of the cursor in relation to the absolute frame, as well a progression cursor for the current command, when necessary.

13 - Search, change, request and approval tabs. This area automatically opens when you slide your cursor over one of the tabs, in the same way that it automatically closes when your cursor remains outside the tab for a few seconds. The Search tab allows you to search the document based on different criteria (see the Search command for details). The Change tab allows you to quickly view documents currently open by different users connected to the same PDM server (see the Change command for details). The Requests tab allows to visualize sent approval requests and requests to approve (workflow). (see the Requests command for details).

Search and Changes tabs can be displayed/hidden with the Search, Changes and Requests commands of the TopSolid7 button > View.

14 - Compass The default position (lower left) displays the orientation of the absolute frame with different sensitive areas that turn green when the cursor hovers over them, this allows you to control the orientation of each view: Displacement of View (Panoramic): To move the view based on an axis, clicking one of the axes (represented in green in the opposite image) with the left mouse button, then move the cursor while holding down the left mouse button. Spherical Rotation: To rotate the view spherically, click the end of an axis (represented in green in the opposite image) with the left mouse button and move the cursor while holding down the left mouse button. For a perpendicular orientation to the selected axis, double-click the axis or the end of an axis. Rotation Around an Axis: To rotate around an axis, click a circle arc joining two axes (represented in green in the opposite image) with the left mouse button and move the cursor while holding down the left mouse button. For a 90° rotation, double-click a circle arc joining two axes. Displacement of Compass:

You can move the compass by clicking the origin of the compass (represented in green in the opposite image) and moving the mouse to an item while holding down the left mouse button, then releasing the button to anchor the compass to the desired item. The compass is positioned on a peak, a planar face or in the middle of a cylindrical, conical or spherical face and the original sphere will be replaced by a cube. When the compass is anchored on an item, the orientation of the absolute frame is materialized by a trihedral positioned in the lower left corner of the screen. You can move the compass back to its initial position by selecting the original cube with the left mouse button, holding down the button and moving it to the void. Negative Axes: You can display the X-, Y- and Z- axes by positioning the cursor next to the assumed location of these axes, they will then appear in green and you will have the same options as for positive axes.

The size of the compass is set by modifying the value of the Scale Factor of Screen Size Objects in the Display feature of the Tools > Options command. When the compass is not visible (while it is positioned on an element which is outside the graphic area), it is possible to dynamically rotate this the wire frame on the bottom left of the graphic area. A double click on this frame allows to position again the compass on this frame.

15 - Workspace The workspace allows you to view the document being modified. The management commands of this area (Zoom, Orientation, Multiple Windows, Rendering, etc.) are found in the Visualization menu, the most frequently used commands are grouped in an icon bar called Visualization and Rendering Bar found to the right of this area. The mouse buttons also allow you to quickly access certain commands: Zoom: Turn the wheel of the mouse to zoom in or out of the view. Global zoom: Double-click on the middle button (wheel) allows you to resize all elements in the graphic area (global zoom). Rotation: Click and hold down the middle button to turn the view contents. Furthermore, you can indicate a rotation axis by positioning the cursor on an item (edge, segment, etc.), and pressing the Alt key on your keyboard. Translation (Panoramic): Click and hold down the right mouse button to move the view contents. Furthermore, you can indicate a translation axis by positioning the cursor on an item (edge, segment, etc.), and pressing the Alt key on your keyboard.

When the workspace is divided into multiple views, the active view is identified by a black edge, the view also

contains the compass and the visualization and rendering bar.

16 - Visualization and Rendering Bar The visualization and rendering bar groups the most frequently used commands of the Visualization menu, these commands allow you to quickly act on the document being modified. Icon

Command Displacement of View (Panoramic). View rotation and access to Rotate View and Lock View commands. Face view and access to other views (above, right, etc.). Perspective View. Split workspace into 4 views and access other split commands (1 view, 2 views, etc.). Best Zoom Window Zoom Shadowed rendering with edges and access to rendering commands (see the different rendering mode commands for more details). The icon changes according to the selected render. Attributes by default. The icon changes according to the selected color. When setting the default attributes, you can use the random color option to have a different color for each created shape of the document. To satisfy the TopSolid V6 users, a right click on the color palette allows to quickly change the color of an element without changing the current color. You can also select a part, open the color palette and change the part color by right clicking on a color. Default line style. The icon changes according to the selected line. Default marker style (available on Drawing documents). The icon changes according to the selected marker.

The contents of this bar can be modified with the Tools > Customize command.

17 - Scale Bar The scale bar allows you to have an idea of the size of the item being modeled, its value is recalculated depending on the zoom performed on the view.

The scale bar can be displayed or hidden by checking or unchecking the Show Scale Bar option in the Display feature of the Tools > Options command.

18 - Project Management Window

When a project is created, its contents automatically displays in the project management window also called the pro This window, similar to Windows Explorer, allows you to manage the set of documents in your project; most of the be accessed from different displayed popup menus when you click a project item.

The most frequently used commands can be performed with the mouse:

Double-click an item to open it. Select an item then click the selected item again to rename this item. Select an item and move it to another folder by holding down the left mouse button and releasing the button to item. When an Assembly document is open, select an item (part, assembly, family, etc.) and move it to the workspac down the left mouse button. Releasing the left button allows you to include this item in the assembly. When a Draft document is open, select an item (part, assembly) and move it to the workspace by holding dow button, release the left button to create the main view of this item.

Informations about states of documents are displayed in the projects tree.

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19 - Project Tabs When multiple projects are open, these tabs allow you to change the current project. As with document tabs, you can quickly close a document by clicking the tab with the middle mouse button (wheel).

20 - Preview Area The preview area displays a preview of the selected document as long as this document was created by a TopSolid7 application. The preview of a document is calculated from shapes contained in the document with the Shadowed Rendering with Edges, Perspective Camera and Global Zoom settings. However, some types of documents, such as threading standards or unfolding rules, do not have a preview.

21 - Visualization tolerances Visualization tolerances can be modified by double-click on the text.

22 - Tools bar of tree Under the tree banner, a tools bar allows to display more or less information. The options are activated by clicking the icon (orange background) and are disabled by clicking a second time. Some icons are not available for some trees. You will the detailled description of each icon in the pages explaining the role of each trees.

Some modes are only available for some trees. For example, the projects tree as no Synchronizations mode .

23 - Measurement When you select one or more elements, a measurement is displayed on the bottom right of the screen without any command being selected. The result depends on the type of element selected: Selection Line Arc or fillet Circle or cylindrical face Two parallel lines or faces Two non-parallel lines or faces

24 - Parts tree

Result Line length Radius Diameter Distance between both lines/faces Angle between both lines/faces

Chat Links/Videos:

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This window allows to chat between TopSolid users (only with the client/server mode).

Creation stages / Use: The chat window can be shown/hidden by using the TopSolid7 button > View > Chat command.

1. All connected TopSolid users are listed in the upper section. Select one or several recipients or click All to select everyone, or None to unselect everyone. 2. Enter your message. 3. Click Send message.

There is no settings, chat uses the Pdm server. The messages are not kept when closing TopSolid. This window automatically opens when a new message arrives. A tooltip appears a few seconds upper the Windows clock.

Using the Mouse

In order to get the best TopSolid 7 scheme, it is highly recommended to use a 3-button mouse with a wheel on the center button. Functions assigned to each button are described in the image below: Button #1 (Left Button): Select an item (entity) or command from a menu or ic Double-click an item to modify it (for example, in the case of a dimension) or dis (for example, in the case of an extrusion). A click in the graphic area followed by a cursor displacement (by keeping the b allows to create a rectangular selection. The frame creation direction is importa strict selection (all elements completely inside the selection frame are selected) element in contact or inside the frame are selected).These 2 modes are differen color and type of line. (blue and solid line for the strict mode, green and dooted mode).

Strict mode: only the circle is selected

Non strict mode: The 2 segm the circle are se

Button #2 (Wheel): When the cursor is in the workspace, turn the mouse wheel to zoom in or out. When the cursor is in the tab bar, turn the mouse wheel to scroll the different m When the cursor is in a tab (Tool window, Document window, etc.), click once to Click in the workspace and move the cursor while holding down the mouse but a point. Double-cick in the workspace allows you to resize all elements in the graphic a Button #3 (Right Button): Displays the popup menu of an item or unwinds a m is in the tab bar. Click in the workspace and move the cursor while holding down the mouse but (panoramic) in all directions.

Rotative Selection: When multiple items are close to each other or overlap or when the selected item is not the one you want (selecting a face when you want to select an edge), you can use the rotating selection. To do this, proceed as follows: Position the cursor on the desired item. Press and hold down the left mouse button. Successively press the right mouse button several times until the desired item is highlighted. Release the left mouse button to validate the selection.

Using the 3D Mouse: In order to facilitate view rotations and moves, TopSolid 7 allows you to use 3D Connection SpacePilot, SpaceTraveler and SpaceExplorer mice. To do this, simply install the most recent drivers for your device, connect the device to your computer and launch TopSolid 7.

Save Document

This command saves the current document.

Creation Stages / Use: From the System Bar, click the icon to save the last modifications of the current document.

This command is accessible with the CTRL + S keys, it can also be launched from the File menu of the TopSolid button or directly from the popup menu of the documents tab.

An object from the project tree that has not been saved, but has been modified, has an asterisk at the end of its name. The rotation and the zoom do not turn the object into a "modified" object but it is possible to save it in order to, for example, keep its orientation.

Modifications / Additional information: The document is saved in the workspace, you must then use the check in command so that the modifications are made accessible to other users.

Save All

The command saves all open documents.

Creation Stages / Use: From the System Bar, click the icon to save the last modifications of all open documents.

This command is accessible with the Ctrl + Shift + S keys, it can also be launched from the File menu of the TopSolid button menu or directly from the popup menu of the documents tab.

Modifications / Additional information: The documents are thereby saved in the workspace, you then need to use the store into vault command so that the modifications are accessible to the other users.

Undo

This command cancels the commands used last before saving the document.

Creation Stages / Use: From the System Bar, click the icon to cancel the last command used, or select, from the drop-down list of the last commands used, a sequence of commands to cancel.

The command used last is displayed at the top of the list, the cancellation of the commands must be made from this last command. Saving or storing the document into the vault deactivates the Undo command.

This command is accessible with the Ctrl + Z keys, it can also be launched using the Edit menu from the TopSolid button.

Modifications / Additional information: The cancellation of commands is managed document by document.

Redo

This command restores previously deleted commands.

Creation Stages / Use: From the System bar, click the icon to restore the last canceled command, or select, from the drop-down list of the last canceled commands, a sequence of commands to restore.

The last canceled command is displayed at the top of the list; commands must be restored from this last command. Saving or storing the document into the vault deactivates the Redo command.

This command is accessible with the Ctrl + Y keys, it can also be launched using the Edit menu from the TopSolid button menu.

Modifications / Additional information: The restoring of commands is managed document by document.

Print

This command prints a document or a view.

Creation stages / Use: Click the

icon from the system bar or select File > Print from the TopSolid button.

Regarding the type of document to print, printing options below might change. To print a bill of material document, follow this link. 1. Select the area of the document to print. Scale 1:1: Only available in a Draft document. This mode allows you to print with the scale 1:1 on the chosen paper size. If the paper size is too small, the print will be incomplete. In frame: Only available in a Draft document. This mode allows you to print all entities in the draft format. The draft is printed with an optimized scale factor so all its elements will be printed on the paper format. View: This mode is not available in a Draft document. The complete graphic area of the 3d document is printed. Area: This mode allows you to define exactly the area to print using a resizable rectangular frame. In this case, an optimum scale factor is calculated so that the area defined prints in the format of the printer paper. Paper: The maximum printable area of the printer is displayed on the document, you can move this area on the part of the document you want to print, set the scale factor and orientation (using the option Landscape). Window: This mode is not available in a Draft document. It allows to print all views of the document when using the multi-view mode. 2. Click Preview to visualize what you want to print. 3. If the draft has several pages, select if you want to print all pages, the current page or select pages to print by separate them by a semi-colon. 4. Select the printer to use and its resolution. 5. Select the color mapping (colors or grey levels). 6. Select the size, the source (rack, roll or others according to the printer type) and the paper orientation of the printer. 7. Validate the printing of the document with the button or click the Preview button to display the print preview in a separate window.

Available Options: Printer: The list of proposed printers corresponds to the printers declared in the Control panel of Windows. The Properties button allows access to the printer settings, these settings depend on the printer drivers .

The Resolution allows the printing quality to be modified, a resolution between 300 and 600ppp (points per inch) allows a good quality result to be obtained. The color mapping option allows to print in colors or with grey levels.

The higher the resolution, the better the quality the result will be, but to the detriment of printing time.

Paper: The list of formats proposed corresponds to the formats defined in the selected printer driver. Depending on the printers, there can be several paper sources (several trays, several rollers, etc.). The Portrait mode corresponds to a vertical format whereas the Landscape mode corresponds to a horizontal format. Copies:: This section allows to enter the number of print copies. They can be collated or not. Advanced options: (only available when printing a draft). When it is unchecked, the Advanced masking option allows to reduce the printing time or the size of the generated pdf.

Preview options: Print: Prints from the preview.

Scale: The display can be enlarged or reduced by selecting a scale factor from the drop-down list. The Auto zoom automatically adapts to the size of the document to print.

Pages: Displays from one to six pages to print.

Close: Closes the preview window without printing.

Print Links/Videos:

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This command allows the current draft document to be printed.

Creation stages / Use: Click the

icon from the system bar or select File >Print from the TopSolid button.

1. Select the area of the document to print. To scale: The document is printed taking in account the format and the document's scale factor. In this mode the format of the printer paper must be equal to or greater than the document's format. Center paper: The document is printed by calculating the optimum scale factor so that the frame of the document prints in the format of the printer paper. Rectangular area: This mode allows you to define exactly the area to print using a resizable rectangular frame. In this case, an optimum scale factor is calculated so that the area defined prints in the format of the printer paper. Paper: The maximum printable area of the printer is displayed on the document, you can move this area on the part of the document you want to print, set the scale factor and the orientation (using the option Landscape). 2. Select the printer to use and its resolution. 3. Select the format and orientation of the printer's paper. 4. Validate the printing of the document with the button or click the Preview button to display the print preview in a separate window.

Available Options: Printer: The printer list proposed corresponds to the printers given in the Windows Control Panel. The Properties button allows access to the printer settings, these settings depend on the printer drivers . The resolution allows you to modify the printing quality, a resolution between 300 and 600 dpi (dot per inch) usually gives a good quality result. The higher the resolution, the better the quality the result will be, but to the detriment of printing time.

Paper: The list of formats proposed corresponds to the formats defined in the selected printer driver.

Depending on the printers, there can be several paper sources (several trays, several rollers, etc.). The Portrait mode corresponds to a vertical format whereas the Landscape mode corresponds to a horizontal format. Margins: These options allow you to modify the unprintable areas of the paper, they generally correspond to feeding zones of the sheet. Line thickness: For each line thickness (fine, medium, large, very large), you can define the actual thickness on printing. Definition of dashes: For each line type (except continuous lines), you can define the actual printing length of the full lines and spaces.

Modifications / Additional information: The settings for line thickness and definition of dashes are specific to each document.

New document

This command allows you to create a new TopSolid document (part, assembly, draft, material, family, etc.).

Creation Stages / Use: Click the

icon on the Home > New Document... tab.

1. Select among the various tabs the document type to be created. 2. If several projects are opened, select the destination project in the drop-down list (bottom left). 3. Depending on the type of document to create, select, if necessary, the document template in the right window. 4. Validate with .

Only open projects appear in the drop-down list of destination projects. If the document is created from the project popup menu, the destination project will be grayed out and will be the displayed project. The last document template used is proposed when a new document of the same type is created.

Besides formats, 2 types of templates are proposed as standard for drafts. Draft for Part: Detailed draft with, among others, hidden strokes and visible threading. Draft for Assembly: Faster draft without visible hidden strokes or threading representation. With this template, if the threading

must be displayed, the style of the view must be modified and the threading must be changed to precise mode.

This command is also available by contextual menu from the project or one of its folders.

Available options: Creation of a Document Template: You can create different types of templates. The project document template is created by dragging the document to the Project Templates folder. My templates are created by opening my templates. These can only be used by the user that created them. Company templates are created by opening the company templates. These templates exist only in client/server mode.

TopSolid templates cannot be modified.

New project

This command allows you to create a new project.

Creation Stages / Use: Click the 1. 2. 3. 4.

icon on the Home > New project... tab.

Enter the project's name. Select a project template if necessary. Select the vault if necessary. Validate with .

The new created project will appear in the project list. You can rename the project later directly from the project tree when the project is open. The last template used will be proposed when creating a new project.

Available options: Creation of Project Templates: You can create different types of templates. My project templates are created by opening my project templates . These can only be used by the user that created them. Company project templates are created by opening the company project templates. These templates exist only in

client/server mode.

TopSolid templates cannot be modified.

New Library

This command allows you to create a new library.

Creation Stages / Use: Click the New Library icon on the TopSolid >File > New Library... button. 1. Enter the library's name. 2. Check or uncheck Library from a template. If this option is checked, it allows you to create a new library based on an existing library selected from the list. 3. Select the vault if necessary. 4. Validate.

The new created library will appear in the libraries list. You can rename the library at a later time directly in the project tree when the library is open. It is possible to deliver and encrypt a TopSolid user library like for example the standard TopSolid libraries. To do that, please read the file Library Designer's guide. This file is only available in English.

New universal library Links/Videos:

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This command allows to create a new universal library. It contains the needed dictionaries to be used with several languages, like the TopSolid standard libraries. For example, the screws are automatically translated to "vis" if TopSolid is started in French.

Creation stages / Use: Select the File > New universal library... command from the TopSolid button. 1. Enter the library name. 2. Validate by clicking . 3. You can now create your component as usually.

The Library designer license is required to be able to use this command.

You can consult the Library designer's guide which is in the Help menu. You will find all information about managing, naming your library, adding a dictionary and also how to encrypt and deliver this library. This document is only in English.

New standard document templates project

Links/Videos:

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This command allows to create a new project with templates of standard documents. When created a new document, templates are proposed (for example, the different templates for a draft). These templates are either in the project or either in the templates projects (My templates or Company templates). This command allows to create a new project of templates which can be delivered to customers or partners.

The Library designer license is required to be able to use this command.

You can consult the Library designer's guide which is in the Help menu. You will find all information about managing, naming your library, adding a dictionary and also how to encrypt and deliver this library. This document is only in English.

Creation stages / Use: Select the File > New standard document templates project... command from the TopSolid button. 1. Enter the project name. If the name is not changed, it will be automatically translated.

2. Select a language for which the standard document templates will be installed. 3. Validate with .

The standard document templates project is automatically installed when starting TopSolid for the first time with this language.The template is then available regardless the TopSolid language.

Use: TopSolid templates cannot be modified. After validation of the command, the culture can no longer be changed.

1. After creating the project, create your own documents templates. 2. Check them in and validate. 3. It is possible to export the package for delivery. If you answer No, a usual package export is created. If you answer Yes: The package can be incremental. In this case, only the latest major revisions never delivered are exported.(For example, if the last exported package had documents with A as major revision and now the new export is with documents with C major revision, then only B and C major revisions are exported). The package is exported with all the major revisions of each document. 4. The package to export must not contain family instances created by drivers. 5. Select the package folder.

Projects

This command allows you to select from a list the project you want to open in the project tree.

Creation Stages / Use: Click the

icon in the Home > Projects...tab.

1. Select from the list the project you want to open. 2. Double click the project to open it.

To search a project, you can enter the first characters of the project name in the Search field and click on to search. Click the blue arrows to move to found projects. Like in Windows search, the * character replace characters when searching. You can click the name of the column to file in alphanumeric order or in reverse order by clicking again the name of the column. Double-click the preview to open the main document of this project. By slowly double clicking the library, its name can be changed. A fast double click opens it.

The project state is displayed before its name: Icon

Command The project is created. It is no longer available for other

users (in client/server mode). It is located in the user workspace. The project has been checked in, but is under modification yet. The vault version is only available for consult in read only mode for another user (client/server mode). Project is into the vault, but not validated. It is available for other users (in client/server mode). Validated project. It is available for other users (in client/server mode). Obsolete project. The project is into the vault, but should no longer be used.

Available Options: You can create a new project and/or a new folder . You can display deleted projects by clicking the icon. An open deleted project is grayed out in the project tree. You can display project templates by clicking the icon. By opening a project template, you can modify the document templates. Click the icon to display an image in the right window if a main document is defined in the project. A right click on a column title allows to delete it or add other columns. The following popup commands are available in the project list: Open. Open Main Document. Delete. Add to Templates. Properties.

Libraries

This command allows you to select from a list the library you want to open in the project tree.

Creation Stages / Use: Click the

icon on the Home > Libraries... tab.

1. Select from the list the library you want to open. 2. Double click this library to open it.

To search a library, you can enter the first characters of the library name in the Search field and click on to search. Click the blue arrows to move to found libraries. Like in Windows search, the * character replace characters when searching. You can click the name of the column to file in alphanumeric order or in reverse order by clicking again the name of the column. Double-click the preview to open the main document of this project. By slowly double clicking the library, its name can be changed. A fast double click opens it.

The library state is displayed before its name: Icon

Command The library is created. It is not available for other users

(client/server mode). It is in the workspace of the user. The library has been checked in, but is under modification yet. The vault version is only available for consult in read only mode for another user (client/server mode). Library is into the vault, but not validated. It is available for other users (client/server mode). Validated library. It is available for other users (client/server mode). Obsolete library. The library is into the vault, but should no longer be used.

Available Options: You can display library templates by clicking . By opening a library template, you can modify the documents templates. Click the icon to display an image in the right window if a main document is defined in the library. A right click on a column title allows to delete it or add other columns. Following contextual commands are available in the libraries list: Open. Open Main Document. Delete. Add to Templates. Properties.

It is possible to deliver and encrypt a TopSolid user library like for example the standard TopSolid libraries. To do that, please read the file Help\en\How to deliver a protected Library.pdf in the installation folder. This file is only available in English.

Open My Templates Links/ Videos:

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This command allows you to open the project in which your document templates are found.

Creation Stages / Use: Select File > Templates > Open My Templates... from the TopSolid button. Create or modify documents. By checking them in, these modifications will be available when creating new documents. Delete Documents. By checking them in, they will no longer appear in the list of document templates.

My Templates is available with TopSolid Local. When using TopSolid in client/server mode, only the user that created these templates will be able to see them, no matter the PC, as long as it is the same user. A template is a base file. There are no links between the template and the document created from this template. If the template is modified or deleted, documents created from this template will not be impacted.

A user template is not shared and is only available to this user. It is not recommended to add materials, user properties, environments in the "My templates" (or company templates) projects.

In this case, if a template part uses a material saved in "My templates", the created part by using this template will be linked to this material. By exporting this new part as a package, and importing it in another pdm, it will create a duplicated "My templates" project in this other Pdm. These types of documents have to be created in a library.

You can also create other types of document templates. To create document templates for a project: 1. Open the project. 2. Create or drag the documents to be used as templates into the Templates folder. 3. Store the project into the vault. To create company document templates: Follow the procedure described in the help section Open Company Templates. Using a document template: To use a document template, click the New Document icon

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Open Company Templates Links/ Videos:

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This command allows you to open the project in which company templates are found.

Creation Stages / Use: Select File > Templates > Open Company Templates... from the TopSolid button. Create or modify documents. By checking them in, these modifications will be available when creating new documents. Delete Documents. By checking them in, they will no longer appear in the list of document templates.

A template is a base file. There are no links between the template and the document created from this template. If the template is modified or deleted, documents created from this template will not be impacted.

Company templates can only be accessed when used in TopSolid Client/Server Mode. It is not recommended to add materials, user properties, environments in the "My templates" (or company templates) projects. In this case, if a template part uses a material saved in "My templates", the created part by using this template will be linked to this material. By exporting this new part as a package, and

importing it in another pdm, it will create a duplicated "My templates" project in this other Pdm. These types of documents have to be created in a library.

You can also create other types of document templates. To create document templates for a project: 1. Open the project. 2. Create or drag the documents to be used as templates into the Templates folder. 3. Check in the project. To create my documents template: Follow the procedure described in the help section Open My Templates. Using a document template: To use a document template, click the New Document icon

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Open My Project Templates Links/ Videos:

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This command allows you to open my project templates to complete, modify or delete one or more user project templates. A project template is a project used as a base for newly created projects. If a project template contains folders and files, these will be automatically created in a new project that uses this template.

Creation Stages / Use: Select Templates > Open My Project Templates... menu of the TopSolid button.

from the File

1. On the project name in the project tree, click Add Project Model from the popup menu. 2. In the list of projects, select the project that will become the template. 3. Validate by clicking .

Only the user that created the project template can view, modify, complete or destroy it. It cannot share it.

Available options: You can create a company project template that can be used by all users (in client/server mode only). Another way to create a project template:

1. Open a project. 2. Select it from the project tree. 3. Use the Define as Project Template command from the popup menu. You can also delete project templates.

Open Company Project Templates Links/ Videos:

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This command allows you to open the company project templates to complete, modify or delete one or more project templates common to all users. A project template is a project used as a base for newly created projects. If a project template contains folders and files, these will be automatically created in a new project that uses this template.

Creation Stages / Use: Select Templates > Open Company Project Templates... the File menu of the TopSolid button.

from

1. On the project name in the project tree, click Add Project Template from the popup menu. 2. In the list of projects, select the project that will become the template. 3. Validate by clicking .

Available options: You can create a project template that can be used only by the user that created it. Another way to create a project template: 1. Open a project. 2. Select it from the project tree.

3. Use the Define as Project Template command from the popup menu. You can also delete project templates.

Import TopSolid V6 Library

This command allows you to reconstruct a TopSolid 7 library from TopSolid V6 library files.

Creation Stages / Use: Click the TopSolid button and use the File > Translators > Import TopSolid V6 Library... command. 1. Select the folder that corresponds to the V6 library standard to import. 2. Validate with the OK button.

This command will create explicit families without generic documents. These families only contain one code column with all V6 component codes (component settings are not found in this document). To include a code from a V6 library import, you can drag the family to the assembly (TopSolid will ask you for the code to include) or drag the code directly. In the tree structure of the library, codes are situated under the affected family. If your V6 component contains driver settings, they will not be recovered during import.

Import Cadenas component

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This command allows to import a component form the PARTSolutions Cadenas components software.

Creation stages / Use: Select the File > Translators > Import Cadenas component... command from the TopSolid button. 1. Start Cadenas. 2. Select the component in Cadenas. 3. Click on CAD export (ParaSolid) from the Cadenas exportation menu.

Cad export from Cadenas

4. The result is converted and saved in an explicite family with the corresponding code. The library is named "Cadenas + Standard name". The folder uses the decomposed standard name (for example 8140). And the explicit family uses the name of the component.

TopSolid explicit family

The PARTSolutions Cadenas software must be installed on the computer, it must be running with a valid license and must be started. The Cadenas version must be at least 9.0.4. The version 10 is also compatible. The installation and the support of this software is not provided by TOPSOLID, nor by one of its resellers.

Modifications / Additional information: Future import of a component: of the same family: If a component of the same family has already been converted as an explicit family, during the import of a second component of this family, the existing explicit family will be completed with the code of the new component.

Import TraceParts component

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This command allows to open your internet browser on the www.tracepartsonline.net website to allow you to find a component which will be included in TopSolid.

Creation stages / Use: Select the File > Translators > Import TraceParts component ... command from the TopSolid button. 1. 2. 3. 4. 5.

Open an assembly. Run the upper command. Select a component on the website. Click CAD Insertion. It is also possible to download it to include it later. The component appears in the assembly. You just have to add some positioning constrains.

TraceParts online must be installed on the computer. Its installation is explained in the Miscellaneous chapter of the Installation guide. An account on the TraceParts website has to be used. A license can be needed. All questions about the TraceParts website, its use, its license have to be asked to TraceParts support. Some authorisation to execute JAVA tools or others can be asked and must be accepted.

On the website, select a component then click on the CAD insertion button. If you aren't logged in, yo

The component appears in the TopSolid assembly which is automatically in pos

The component is converted and saved in an explicite family with the corresponding code. The library is named "TraceParts + Standard name". The folder uses the decomposed standard name (for example 8140). And the explicit family uses the name of the component.

The connection to the TraceParts website is still active even if the internet browser is closed. To close this connection, use the Quit TraceParts command.

Quit TraceParts Links / Videos :

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This command allows to close the TraceParts website connection.

Creation stages / Use: Select the File > Translators > Quit TraceParts... command from the TopSolid button.

This command allows to close the TraceParts website connection. Even if the internet browser is closed, the connection is still active. Close this connection with this command.

Available options: Name of the option: Description

Name of the option: Description

Modifications / Additional information: Text

Import OpenPackage Links/Videos:

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This command allows to import Openpackage document( extension is .TopOpnPkg). This kind of document has an opened format based on the xml language and companion files. This format is used only by developers to be able to fill package files by programing.

Creation stages / Use: Select the File > Translators > Import OpenPackage... command from the TopSolid button. 1. Select the OpenPackage document to be imported. 2. Validate by clicking .

Import file into document Links / Videos:

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This command allows you to import a document to convert on the fly into a part or assembly document.

Creation Stages / Use: Select the File > Translators > Import file into document... command from the TopSolid button. 1. Select the document to be imported. 2. Choose the import options. 3. Validate by clicking .

The file is converted on the fly. It is placed on the destination frame. To move it, use the Transformation command. When the file is being imported into the part document, an import operation is created in the tree. The imported file will also be found in the list of shapes. The imported document does not become a PDM document, and is not referenced in the project tree.

The import in an assembly is only possible if the imported file contains several parts.

Import project

In this mode, objects can be imported as is, keeping the original identifiers. It is then possible to send an object to another TopSolid PDM belonging to another client who can modify the object. Once modifications are complete, the object can be sent back. Example: A main contractor exports a package (all documents are checked-in) and send this package to his subcontractor. The subcontractor imports this package with this command. He modifies documents, checks them in, exports the package and send it back to his main contractor. The main contractor imports the modified package by also using this command, all documents are recognized and will update original documents they are coming from.

Creation Stages / Use: Click on TopSolid button > File and select Import project ... command or click icon in Home tab. 1. Select the package document (TopPkg) to import. 2. Select the vault into which the project will be imported. 3. Validate.

Additional information: During this import as replication, TopSolid first verifies major revision to import and compare it to the possible equivalent major revision referenced in the vault. Different scenarios can apply at this stage: The major revision already exists in the vault:

- The life cycle status of the major revision in the vault is "design" -> update with the minor revision to be imported. - The life cycle status of the major revision in the vault is "validated" -> update not possible, a new local revision must be created to be able to update it, which will then have a "design" status. - The life cycle status of the major revision in the vault is "obsolete" -> update not possible, a new local revision must be created to be able to update it, which will then have a "design" status. - The life cycle status of the major revision in the vault is "deleted" -> update not possible, a new local revision must be created to be able to update it, which will then have a "design" status. The major revision does NOT exist in the vault: - The life cycle status of the latest major revision of the vault is "design" -> update by major revision of import and update of life cycle status of previous major revision. - The life cycle status of the last major revision in the vault is "validated" -> update by adding the major revision to be imported. - The life cycle status of the last major revision in the vault is "obsolete" -> update by adding the major revision to be imported. - The life cycle status of the last major revision in the vault is "deleted" -> update by adding the major revision to be imported. Minor revision update: - The revision to import is older or the same at the one currently in the vault -> no update to perform. - The revision to be imported is more recent than the last revision in the vault without any conflict since no local change was done since the last export. -> import the new minor revision keeping its minor index.

- The imported revision in conflict with the changes done locally. -> the index of the imported minor revision becomes the max index of the last local minor revision + 1. The filename of the imported minor revision is updated in the workspace as well as all document references pointing to the imported minor revision and whose index had to be changed on account of the conflict.

To use import by replication, it is imperative that all documents be checked in before exporting the package. If this condition is not correct, it is import project as distinct copy command which will be automatically used.

Available options:

Comment: This field is not used yet.

Vault of new project(s) to add: Each project is attached to a vault. Several vaults might have been defined by the administrator. In this case, select the vault to use in the drop-down list.

Conflict management in case of update: By importing a package as replication, it can contains a document which also exists in a project or in a library, with the same revision, but this document is different. There is a conflict to solve. For example, a subcontractor has modified a part you sent him, but during this time, you have also modified this part and they have both the same revision. Keep local version: The document which is in your vault will be kept and will replace the imported document. Update with imported version: The document which

Import project as distinct copy

This command allows you to import a package as a new project.

Creation Stages / Use: Select File > Import project as distinct copy... command from TopSolid button. 1. Select the package document (TopPkg) to import. 2. Select the vault (if there are more than one) into which the project will be imported. 3. Validate. The project is created as it was when exported.

The project and the documents created are completely independent from those exported, for example, by importing the project in the same vault as the initial project. If imported documents have to be « recognized » and updated in the original PDM where they are coming from, use Import project command instead.

Available options:

Comment: This field is not used yet.

Vault of new project(s) to add: Each project is attached to a vault. Several vaults might have been defined by the administrator. In this case, select the vault to use in the drop-down list.

Conflict management in case of update: By importing a package as replication, it can contains a document which also exists in a project or in a library, with the same revision, but this document is different. There is a conflict to solve. For example, a subcontractor has modified a part you sent him, but during this time, you have also modified this part and they have both the same revision. Keep local version: The document which is in your vault will be kept and will replace the imported document. Update with imported version: The document which

Close document

This command closes the current document and saves the last modifications if any. From the TopSolid button, open the File menu, then chose the Close command to close the current document. If the document has already been saved, it will close directly, if not TopSolid will ask you whether to save the document or to close it without saving, the last modifications will then be discarded.

This command is accessible by clicking on the "X" displayed in the upper right-hand of the document or directly from the popup menu of the documents tab.

Close all documents

This command closes all open documents and saves the last modifications if any. Using the TopSolid button, open the File menu, then select the Close all documents command to close all the documents that are open. After verification of the status of all open documents, TopSolid will ask you whether to save all the documents that were modified (and not saved) or to close them without saving them, the last modifications will then be discarded.

This command is also accessible directly from the popup menu of the documents tab.

Close all

This command allows you to close all open documents and projects and saving the latest changes. From the TopSolid button, open the File menu, and then select the Close all command to start closing all open documents and projects. After checking the state of each opened project, TopSolid will propose to save each modified project (and not saved) or to close them without saving. In this case, the last modifications are lost.

The items will be saved in your local workspace. This command does not allow you to check the items in.

Modifications / Additional information: The items are saved in the workspace; you must then use the Check in command to make the changes accessible to other users.

Save document as This command allows you to make a copy of the existing document by saving it in the same project under another name.

Creation Stages / Use: Click the Save Document As icon or select File > Save Document As... from the TopSolid button. 1. The document is automatically copied in the project. Rename your document if necessary.

A synchronized document (a part created in place in the assembly) is not managed by the Save Document As command.

The resulting new document will be of the same type. A saved-as part document will remain a part document.

Export Document with Conversion

This command allows you to export a TopSolid document into another format. (ParaSolid, Step, etc.) Creation Stages / Use: Click the TopSolid button or select File > Export Document with Conversion... from the drop-down menu. 1. 2. 3. 4.

Select the destination directory. Select the name of the file. Select the file type. Click the Save button.

You cannot export unless one or more documents are open. It is the current document that will be exported.

Background document

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This command allows you to add a background document (sketch of another document...) and use it as support for a new sketch in repassing mode, for example.

Creation Stages / Use: Choose the command File > Add a background document... from the TopSolid button. 1. Choose, from the drop-down list, the document to add as background, this one will be stored in the Backgrounds folder of the entities tree. 2. Validate.

The document to be added as a background document must be previously opened in a TopSolid window.

The document to be added as a background document is linked to the document in which it is inserted. Any modification of the background document has an effect on the document which uses it. If the document used as Background documents is deleted, the document using it will become invalid.

Available options: Transparent : When this option is checked, the shapes contained in the background document are displayed with a transparency and the wireframe elements are display in half tone color.

Modifications / Additional information: Background document modifications are available in a popup menu in the folder Backgrounds in the entities tree. This menu allows you to hide, open a background document or show it in the project tree. The Isolate command allows you to break the link with the background document. You can also avoid any undesired hooking using the Selectable command which allows to forbid the selection of a background document elements

Virtual document

This command allows you to convert a document into a virtual document. A virtual document is a document that should not be a document, but is required to create other documents. A virtual document is not proposed during a search or when selecting a document in a dialog. For example, to do a profile family, the main part is only used for parametrization but must not be used in an assembly. By changing this part to a virtual document, of parts, the base is a part. If it has not to be used, it should be transformed into a virtual document, only family instances of this profile will be proposed when searching or using the Profile command.

Creation Stages / Use: Choose the command File > Virtual document... from the TopSolid button when the document to be made virtual is open. 1. Check Virtual document. 2. Validate.

Modifications: In order to no longer make a document virtual, all you need to do is open it, choose the File > Virtual document... command from the TopSolid button and uncheck the option.

Unexportable document

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This command allows you to lock a document to avoid its export with conversion.

Creation stages / Use: Select the File > Unexportable document command from the TopSolid button.

1. Check the option. 2. Validate. This command is only available with the library Designer license.

Modifications / Additional information: It will not be possible to export with conversion a document defined as unexportable.

Unsynchronizable Document

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This command allows to forbid the synchronization of a document during an operation made from the assembly document.

Creation stages / Use: Select the File > Unsynchronizable Document... command from TopSolid button. 1. Check the option. 2. Validate.

A boolean parameter named Unsynchronizable is created in the parameter folder of the entities tree.

Modifications / Additional information: When a document is defined as unsynchronizable, it is no longer allowed to apply a drilling, a trimming, etc... or to make the process of a component directly from an assembly document.

Ghost document

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This command allows you to convert a document into a ghost document. This kind of document allows a user to include a component into an assembly, without filling automatically representations with this component. It can be useful in the case of tools components. They are only used to make processes, they aren't a part of the assembly, they mustn't appear in the bill of materials or in the draft.

Creation Stages / Use: Choose the command File > Ghost document... from the TopSolid button when the document to be made ghost is open. 1. Check Ghost document. 2. Validate.

Modifications: In order to no longer make a document ghost, all you need to do is open it, choose the File > Ghost document... command from the TopSolid button and uncheck the option.

Unmovable Document

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This command allows to forbid the moving of a document into the project tree.

Creation stages / Use: Select the File > Unmovable document... command from TopSolid button. 1. Check the option. 2. Validate.

This comand is available in advanced mode only (with the "-a" argument in the TopSolid shortcut), a boolean parameter named Unmovable is created in the parameter folder of the entities tree.

Modifications / Additional information: When an in-place part or parameter is created, this parameter is automatically created. When a document has been defined as unmovable, the Tools > Options > PDM > PDM > Enable documents moving into document option has no effect.

Copy

This command allows you to copy items from operations so that you can paste them later in a non-associative way.

Creation Stages / Use: Select the items or the operations to copy, then launch the Copy command using the mode of your choice: Press the Ctrl + C keys on your keyboard. Right-click to make the popup menu appear, then select the Copy command. From the Home toolbar, click the Copy icon. From the TopSolid button, select the Edit menu, then the Copy command.

Quick Copy/Paste: Select the items to copy/paste then press the Ctrl key while leftli ki th

Modifications / Additional information: This command does not allow you to copy/paste items into another Windows application.

Paste

This command allows you to paste, in a non-associative manner, previously copied items.

Creation Stages / Use: Launch the Paste command using the mode of your choice. Press the Ctrl + V keys on your keyboard. Right-click to make the popup menu appear and select the Paste command. From the Home toolbar, click the Paste icon. From the TopSolid button, select the Edit menu from the Paste command. Click the destination point (in order to copy a sketch) or select the items (edges, faces, etc.) on which to apply the operation.

Quick Copy/Paste: Select the items to copy/paste then press the Ctrl key while leftclicking on the mouse

Modifications / Additional information: Copied elements have no links with copied elements.

Delete

This command deletes selected items.

Creation Stages / Use: Select the items to delete, then launch the Delete command using the mode of your choice: Press the Del key on your keyboard. Right-click to make the popup menu appear, then select the Delete command. From the Home toolbar, click the icon. From the TopSolid button, select the Edit menu, then the Delete command.

Inadvertently deleted elements may be retrieved by using the Undo command.

Basify

This command allows to basify (break associativity) of a sketch, a part or other. The result is the same than after importing, there is no operations.

Creation stages / Use: Select the Edit > Basify... command from the TopSolid button. 1. Select entities to basify. 2. Click the blue arrow to validate.

This operation is irreversible. When a sketch is basified, it has no more constraints or dimensions. It becomes magenta. When a part has been basified, there is only a shape in the operations tree.

You can partially basify a shape by moving the inserting cursor. Operations done above the cursor will not be basified, basification will only operates operations under this cursor.

Edit error

This command allows an error/invalidity of a document to be edited.

Use: Click the icon or select Edition > Edit Error... from the dropdown menu. TopSolid displays this icon when an error is detected. A detected errors folder is available in the entities tree.

The icon will appear in the document tab if this contains an error. If not, the icon will not be there and access via the menu will be grayed out.

Isolate

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This command allows to break the link with a linked document like an environment or a background document.

Creation stages / Use: Select the Edit > Isolate... command from the TopSolid button. 1. Select the linked document to isolate. 2. Validate by clicking .

This operation is irreversible and elements hooked on elements of the isolated document are becoming basic elements. For example, if a sketch is created using a plane of a background document, after isolating, the sketch will be still valid but the support plane of the sketch will be no longer hooked on a geometry.

By checking the Report isolations option, a Isolations folder is created in the entities tree. It lists all basified entities by this command. The folder can be emptied with the Empty contextual command..

Modifications / Additional information:

If the part or the assembly to isolate is a synchronized part or assembly, you have to use the Isolate as contextual command. If the part or the assembly to isolate has to be replaced by its copy, use the Isolate as and replace contextual command.

Refresh This command allows updating all the operations of a document.

Creation Stages / Use: The rebuilding is carried out as soon as the command Edit > Refresh is launched from the TopSolid button.

You can also rebuild only one operation, one entity or one parameter with the contextual menu from the entities or operations tree. The command Refresh is generally found in the submenu Others.

Modifications / Additional information: When a document contains operations which must be manually updated, this contextual command is available. It allows to update at once all operations who need to be updated. This command is also present in the TopSolid system bar, it can also be launched with the F5 keyboard key.

Rebuild

This command allows forcing the recalculation of all the operations of the current document.

Creation Stages / Use: The rebuilding is carried out as soon as the command Edit > Rebuild is launched from the TopSolid button.

You can also rebuild only one operation, one entity or one parameter with the contextual menu from the entities or operations tree. The command Rebuild is generally found in the submenu Others.

Upgrade

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A document made with an old version of TopSolid may not have all information which it could have if it has been created with the latest version of TopSolid. This command allows to upgrade to the newest version.

Creation stages / Use: Select the Edition > Upgrade... command from the TopSolid button.

This command is only available in advanced mode (TopSolid is started with the -a argument).

This command is also available via the contextual menu of an operation from the operations tree.

Auto update

This mode allows automatic updating of the entities being modified to be enabled or disabled.

Use: Click the

icon in the icon bar of the Home tab.

During the modification of complex parts, assemblies, drafts, the automatic updating of documents can reduce performances, it is then advised to disable this mode. Example: An assembly of 4000 parts is drafted, modifications are made on this assembly, it is advised to disable the automatic updating so as not to recalculate the draft immediately. When the command is disabled, the Update command appears in the graphic to allow a manual update.

Additional information: This mode is enabled when the icon is pressed down. (background stays in color). This mode applies to all the documents in the TopSolid session. When this mode is disabled, updating can be done manually by clicking on update.

Update

This command allows the documents to be updated manually.

Use: Click the icon in the icon bar of the Home tab. When automatic updating is disabled, the update icon allows the documents to be updated manually.

In some cases, in order to improve performances, Automatic updating is disabled. In this case, the command is located in the graphic, and the update is done manually, if needed.

Update all

This mode allows all the document information to update manually.

Use: Click the

icon in the icon bar of the Home tab.

TopSolid documents are partitioned into different sections, like for example, the modeling section and the analysis section. When using Automatic update, Update or Update heals, only the modeling section is updated. If the section Analysis is not updated automatically, it is not recalculated and its information may not be up to date (mass, volume, center of mass, etc...). In this case, you have to Update all.

In order to improve performances, updating the analysis elements (mass, volume, center of mass, etc...) can be disabled in order not to recalculate this information with each modification. In this case, updating the document is done manually if required. The Update all command appears in the graphic when editing a part in place in an assembly for reassembly. For a part created in place, the command does not appear because updates to the two documents are synchronized. That is, updating the part document also updates the assembly.

Changes

This command allows you to view all changes made to documents. (New, Checked Out, etc.).

The various commands are explained by clicking this link.

Checked-in documents do not appear in this list.

Modifications / Additional information: Popup commands on the document allow you to: to cancel changes (only on the document being modified). to go up the project tree. to open the document. to check in.

The entity window allows you to display the entity tree. This tree consists of folders that contain entities. The last entity created is placed at the top, if this order is not suitable, you can move the entities. To do this, simply click and hold down the left mouse button, move the mouse and release the button when you reach the desired destination. When selecting a folder or entity, an echo of the item displays in the workspace. Depending on the state of the entity, the text can display in different ways: Color Black Bold Gray Green Blue Red

Entity Status Normal State. The entity has been inherited and cannot be directly edited (for example a mechanism joint inherited wh including). The entity is not available at this time. The entity is being edited. The entity must be refreshed. The entity is invalid.

The entity window can be displayed/hidden with the TopSolid7 button > View > Entities command.

Under the tree banner, a tools bar allows to display more or less information or columns: Icon Command Collapse all: Allows to collapse all opened sub-folders. Show search: A field appears to fill the beginning of a word to find it in the tree. The tree is automatically unrolled and the first matched word found is highlighted. The icon allows to empty the field. Show folders counts: Display the information counts found in the tree. For example, in the entities tree, Sketches (5) means that there are 5 sketches in this folder. Show definitions: If this mode is disabled, a fillet in the operations tree does not display any information. By enabling this option, an information node appears under the fillet and displays its parameters. Show references: Allows to display a subnode named References under the elements which depend on other elements. These latter elements appear in a list when you expand the subnode. Show back references: Allows to display a subnode named Back References under the elements that other elements depend on (in the same document). These latter elements appear in a list when you expand the subnode. Show parent and children operations: Display the parent and children operations. For example, if this mode is activated in the entities tree of an assembly, in the Parts folder, you are able to unroll ( ) a sub-assembly and display its positioning and inclusion. If the mode is disabled, you are not able to unroll this sub-assembly. Show entities: This mode, only available for the operations tree, allows to display the operations entities. By unrolling the operation, an entities sub-folder will be displayed ( ). For example, by unrolling a extruded, the shape and the height dimension will be displayed. Track entities/operations: When selecting an entity or an operation in the graphic area, it is also highlighted in the tree. By default, this mode is disabled in the projects tree. Sort entities in alphabetical order: This mode, only available for the entities tree, allows to sort entities in alphabetical order to find them easier. Show entities that are not available. This mode, only available for the entities tree, allows to show entities even if they are not available, like for example a created plane when the inserting cursor is under it. Options: Allows you to display additionnal columns in order to manage the visibility, the transparency, the color and the layer of the entities.

Visibility : Allows you to show or hide the entities. - When a check mark is located in front of a folder, all the entities of this folder are shown. - When a small square is located in front of a folder, not all the entities of this folder are shown. - When no check mark is located in front of a folder, all the entities of this folder are hidden.. Color and transparency : Allows you to change the color and the transparency of an entity. The color is displayed in front of the entity as well as the transpency value. Layer : Allows you to change the layer of the entity. The number of the layer is displayed in front of the entity. Show all: Allows you to show all the entities of the document except the publications and the compass. Hide all: Allows you to hide all the entities of the document except the publications and the compass. Invert visibility: Allows you to invert the visualization of the document's entities, visible entities are hidden and hidden entities are shown.

The operations window allows you to display the operations tree. This tree consists of the list of operations that allowed you to complete your document. Operations are filed in chronological order, the last operation displays at the top of the tree. Each operation is automatically named. You can rename an operation by selecting Other > Rename from the popup menu or by clicking an operation that is already selected. When selecting an operation, an echo of the selected operation displays in the workspace. As with the entity tree, depending on the operation status, the text representing each operation can be in different colors: Color Black Bold Gray Green Blue Orange Red

Operation Status Normal State. The operation has been generated by an other operation and can't be directly edited. The operation was not executed. The operation is being edited. The operation is in manual refresh mode and needs to be refreshed. The operation is out of date, it was modified, but not executed again. The operation is invalid.

Also, if a sketch is under constrained, (some of its entities are magenta), it will be displayed with (-) as prefix You can view the different construction stages of the document by moving the insertion cursor to the tree. When this cursor moves down, all operations above are turned off (displayed in green), if you perform a new operation, it will be inserted just below the cursor. You can move the cursor up by moving it manually, right-clicking the cursor and selecting End Insertion from the displayed popup menu or clicking the icon found on the document tab. Example of using the insertion cursor:

Stage #1: Part with insertion cursor up.

Stage #2: Lowering of the insertion cursor under the hollowing out operation.

Stage #3: Drilling Creation.

Stage #4: Moving up the insertion cursor, the hollowing out operation takes into account the previous inserted drilling.

You can also move an operation. To do this you must select the operation by left-clicking and holding down the left mouse button, then releasing the button in the desired position. Operations can be categorized into folders, folders can be created by right-clicking the insertion cursor and selecting the Folder command. To move an operation to a folder, you must select the operation to move with the left mouse button, hold down the button, move the operation under the folder name, then release the button. As with operations, a folder can be moved or renamed.

Example of operations filed in different folders:

The operations window can be displayed/hidden with the TopSolid7 button > View > Operations command.

Under the tree banner, a tools bar allows to display more or less information or columns: Icon Command Collapse all: Allows to collapse all opened sub-folders. Show search: A field appears to fill the beginning of a word to find it in the tree. The tree is automatically unrolled and the first matched word found is highlighted. The icon allows to empty the field. Show folders counts: Display the information counts found in the tree. For example, in the entities tree, Sketches (5) means that there are 5 sketches in this folder. Show definitions: If this mode is disabled, a fillet in the operations tree does not display any information. By enabling this option, an information node appears under the fillet and displays its parameters. Show references : Allows to display a subnode named References under the elements which depend on other elements. These latter elements appear in a list when you expand the subnode. Show back references: Allows to display a subnode named Back References under the elements that other elements depend on (in the same document). These latter elements appear in a list when you expand the subnode. Show parent and children operations: Display the parent and children operations. For example, if this mode is activated in the entities tree of an assembly, in the Parts folder, you are able to unroll ( ) a sub-assembly and display its positioning and inclusion. If the mode is disabled, you are not able to unroll this sub-assembly. Show entities: This mode, only available for the operations tree, allows to display the operations entities. By unrolling the operation, an entities sub-folder will be displayed ( ). For example, by unrolling a extruded, the shape and the height dimension will be displayed.

Show synchronizations: This mode, only available for the operations tree, allows to display synchronizations (for example, parts modified according to an assembly geometry). Track entities/operations: When selecting an entity or an operation in the graphic area, it is also highlighted in the tree. By default, this mode is disabled in the projects tree. Sort entities in alphabetical order: This mode, only available for the entities tree, allows to sort entities in alphabetical order to find them easier. Show entities that are not available. This mode allows to show entities even if they are not available, like for example a created plane when the inserting cursor is under this plane or a parameter created in a stage located after the current stage (parameter created in the Analysis stage when the document is in the Design stage).. Options: Allows you to add the Execution duration column for each operation. Execution duration: Allows to know the execution time of each operation. It allows to identify the most time consuming operations and may be try to optimize the design.

The options window allows you to display the options tree. This tree allows you to set the appropriate options of the document, such as units, language, visualization tolerance, etc. Contrary to software options common to all documents, these options are saved in the document, which allows different settings depending on the document (for example, the visualization tolerance will be different depending on the size of the modeled part) and allows you to find them when opened on another station. Under the tree banner, a tools bar allows to display more or less information. The different icons are explained here.

To manage more quickly the assemblies, this tree allows to: modify the parts visibility modify the parts attributes show or hide selected parts invert the selected parts visibility sort parts in ascending or descending order. modify one or several parts via the contextual menu filter parts by set or by function (for the components). Under the tree banner, a tools bar allows to display more or less information Options are activated by clicking the icon (orange background) and are disabled by clicking a second time. Icon

Command Collapse all: Allows to collapse all opened sub-folders. Show search: A field appears to fill the beginning of a word to find it in the tree. The tree is automatically unrolled and the first matched word is highlighted. The icon allows to empty the field. Show folders counts: Display the information counts found in the tree. When several parts have the same name (repeated), only one is displayed as a folder. 8754 (4) means that there are 4 parts named 8754. Track entities: Allows to highlight in the tree, the selected part (in the graphic area).This mode is disabled by default. Allows to display the sets list to be able to use them with a filter.(For example, hide all parts of the selected set). Allows to display the functions list to be able to use them with a filter. (For example, hide all parts with a screw function). Allows to divide vertically or horizontally the filters section. when the icon is on (orange background) it is the vertical division. Check the different parts to show. Unchecked parts are hidden. This command has to be used part by part. Allows to change the attributes (color, transparency, layer) part by part. Allows to change the layer by modifying the attributes (color, transparency, layer) part by part. Allows to show all parts. Allows to hide all parts. Allows to invert the visibility. Hidden parts become visible and vice-versa. Allows to sort parts in ascending order. Allows to sort parts in descending order. Allows to display parts as hierarchical view or not. Allows to display or not the table columns (

,

,

).

Requests Links/Videos:

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This command allows you to view user approval requests and pending approvals for approving users. The tab is near the search tab (bottom of the screen).

Creation stages / Use: Click the Requests tab. If the tab is not displayed, click the Requests command in the View folder of the TopSolid button. Click the icon to display the user issued requests or the icon to display the requests the approving user has to treat.

When the icon is grayed, it means this request is displayed.

: ( by user) The table indicates the Name of the document subject to the request, the date of the request, the comment entered by the requester and the state of the request. The following popup commands are available in the document: Show to display in tree. Open to open document. Cancel to cancel the approval request.(only for pending requests)

Close to delete the document from the list when it is approved or rejected.

: (by approving user) The table indicates the Name of the document to approve, the question asked by the requester, the date of the request, the name of the requester and the comment entered by the requester. The following popup commands are available in the document: Show to display in tree. Open to open document. Answer to accept or reject the approval. Enter the comment displayed to the requester. If Accept is selected, the approval is in effect and the state of the document is changed as set in the workflow actions. Information is indicated in the document history, the hourglass is removed on the document icon and the requester's request passes to the state defined by the action. If Reject is selected, the approval is rejected. The information is indicated in the document history, the hourglass is removed from the document icon and the state of the request is changed to Rejected. If Cancel is selected, the answer is cancelled and the approval request remains pending.

When a request is in progress, an hourglass overlaps the document icon until the request is accepted or rejected. All requests, request cancellations and accepted or rejected approvals are saved in the document history. When the workflow uses several actions, the state of the document changes once the last accepted action is accepted. If an action is rejected, the following are no longer proposed.

A pending approval document can only be opened for consultation. You cannot modify it.

A pending document may not appear in the list while its state has changed and the approving user project has not been updated. (the document is bold in the projects tree). Just use the Get latest revision (recursive) contextual command from the document, folder or project.

Available Options: Allows you to select the project in which to view current user requests or approvals. Projects display in the Name column. Click "+" to unroll and display the approval state of the document. Approved documents are listed in green, refused documents are in red and pinding documents in black. Allows to display the selected document preview.

Work Manager

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The Work Manager panel (can be abbreviated to WM) allows to centralize the tasks to be processed, to group them and to select them to produce works, all in a multi-users environment.

This module is protected by a license.

Creation stages / Use: The Work Manager panel can be shown/hidden by using TopSolid7 button > View > Work Manager... command. The usual WM operating process consists of: Create tasks. Create supports (if necessary). Select tasks to be processed. Select supports to use (if the process deals with nesting). Create work with these tasks and supports. Configure and execute processes of the associated Work document.

Check and validate the work.

Tasks / Supports: A task describes an object to be treated by the WM. This will be done through a Work. A support is used as a task but it will be used for work documents with nesting processes. Create task / support can be done by: Drag-and-drop of a check-in document in the Document column of the WM panel. Right-click on a chek-in document from the project tree, then select the Work Manager > Tasks / Supports command. Right-click on a BOM document (for tasks creation only). Double click on a task / support allows to open its characteristics to modify them. Delete task / support: Select the task / support to be considered and click the Delete task / support icon. A task / support whose the process is in progress cannot be deleted. Process in progress tasks cannot be used to create new work document.

Works: This tab allows to create and manage Work documents use to execute processes. Create work: To create a work, you must select tasks first in the Tasks tab by checking the cells (if necessary, select supports too in the Supports tab).

Then from the Work tab select the Create work icon. A dialog box allows to select the project and the destination folder of the work document. Possibility to use a work document template. The Work document is created, and the corresponding work is created in the WM panel. Once the processes executed, and if results suit you, you can achieve the work using the Achievment command. Delete work: To clean WM panel, you can delete achieved works. Select the work to be considered and use the Delete work icon. An option allows to delete the work document too. When a work is achieved, delete it delete associated tasks too. A work document created from the WM is linked with it. To make the difference with a free work type document (created outside the WM), the icon of the Work tab of the work document created from the WM is symbolized with a chain. Deleting a Process in progress work, status of associated tasks change from Process in progress to Processable. It is recommended to delete the associated Work document simultaneously. If a work is deleted from the Work Manager without delete the associated work document you will have a work document created from the Work Manager but without work into the WM. The Free command allows to break the link with the Work Manager in order to have a free work document. The icon describes above is modified and there is no chain anymore.

Available options: Filters:

Quick filters: On the top of each columns a field allows to enter string. This text will be used to filter display of the corresponding column. Icon on the right of this field allows to choose how to filter (right click on the icon). Available options change according to data display in the column. Filters configuration: Filters created here will be available for user who create them only. There are created as usual adding properties. Filters can be done on user properties (see below) define on tasks / supports. These properties are available in Company Configurations (Work Manager) of User section. Company filters configuration: Identical to the filters above. Allows to create filters available for all users. This command is available for Admin user only (and so only in Pdm server mode).

Columns configuration: This option allows to customize the contain of Tasks and Supports windows in order to add/delete properties. In this Columns configuration window, it will be possible to modify order of properties, to force column title and to modify format.

Save / Synchronize: Using Work Manager in Pdm server mode with several users, this command allows to update WM information and make them visible for users. Example 1: Admin creates tasks and save the WM. User will see these tasks once he will select the Save / Synchronize command too.

Example 2: Admin assigns tasks to U1 (with right click on the User column), he does not save the WM, tasks status change to Modified. As long as U1 does not use Save / Synchronize, he will not see this change (and he will have an error message trying to modify a task). As U1 activates the Save command, tasks status are updated and change to Locked. Now Admin save the WM too, tasks are modified to Up to date. And the same for U1 as he will select Save / Synchronize.

User properties configuration: It is possible to define user properties associated to tasks and supports. Creating tasks and supports, these properties will be available for each entity. This data will mainly be used for information, sorting and selection (by filters) of tasks and supports, before the creation of work. Once the dialog box is validated, it no more possible to delete a property created before (tasks and supports could use them). However, it is possible to Disable an existing property. This one will not be available anymore in all dialogs using tasks / supports.

On / Off: This icon allows to start or stop the Work Manager. Green icon: Work Manager is started. Red icon: Work Manager is stopped.

Connection parameters: This dialog box allows to manage connection to WorkManager

server from TopSolid. Enter the computer name (or IP adress) of machine hosting the WorkManager service (see below). Data service listening port (enter the same value as in the WorkManager service describe below). Lock service listening port (enter the same value as in the WorkManager service describe below).

Manage local WorkManager server: This command allows to administer and manage the setting options of the local WorkManager server. It is not available in Pdm server mode. In this case the WorkManager server is manage outside TopSolid using the TopSolid'WorkManager Server service. See Help dedicated to this command for more information.

Preview: This icon opens a window to display document preview.

Modifications / Additional information: Multi-users work: The WM also aims to organize the processing of tasks between several users. In Pdm server mode, tasks and works are assigned to users. By default, tasks are assigned to the user who creates them. Options for assigning users are different depending on whether you are an administrator or a standard user.

Administrator can assign any task to any user (if the task is not Process in progress). It is also possible to assign a task to no user. Standard user can modify task user only if they are assigned to him or assigned to nobody. Assignation to users is done making a right click on the User column. See also the Save / Synchronize section above.

Work status: The work status information, available in the Work status column of the Works tab of the WM, is also visible in the icon bar of the Work document, between the Achievment and Free commands. This information is available in this menu if the work is manage by the WM only.

Search Links/ Videos:

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This command allows you to make all sorts of searches to find libraries components, parts or assemblies depending on certain criteria. 1. Presentation. 2. The different icons. 3. Search types. a. Refined Search. b. Multi-criteria search. c. Classification. 4. Results. 1. Presentation: Create a new Search document. This document can be checked into the current project, into the My searches project or the Company searches project. My searches project and Company searches projects can be found in the Searches tree. To display this tree, use the View > Searches command of the TopSolid button.

The search tool is composed of 3 zones: The upper part allows to select the type of documents to search for, the classification to use, projects where to search and the visualization of the result. The intermediate part allows you to make refined and multi-criteria searches. The lower part is displayed the result either in preview or in drop-down windows. 2. The definition of different icons search toolbar is on this page. 3. Search types: There are several types of searches: To search just by a name, a description or a part number, use the quick search by clicking the icon on the upper right of the screen. a.

Refined search: For this search, the first line of the detailed search will be used as well basic syntaxes. The simple search is not sufficient, if the search must be done for one screw. By refining the search, it is possible to specify, hexagon head screw. To search for a hexagon head screw: Select the type of document. For the screws, select Family.

Select which projects to search in. In the Properties column, select Function > Screw > Type of head. In the Operator column, select Equal. In the Value column, select Hexagonal Head. Click the Refresh icon. b.

Multi-criteria search: For this search, several queries can be entered in order to search, for example, for all steel nuts available from such-and-such supplier, made from such-andsuch material. To search for a steel hexagon head screw: Select the type of document. For the screws, select Family. Select which projects to search in. In the Properties column, select Function > Screw > Type of head. In the Operator column, select Equal. In the Value column, select Hexagonal Head. In the And/Or column, select And. In the Properties column, select Standard > Material > Name of the material. In the Operator column, select Equal. In the Value column, select Steel. Click the Refresh icon.

c.

Classification search: For this search, a classification criterion has to be defined. To search a classified screw: Select the type of document. For the screws, select Family. Select which projects to search in. Click the classification button. Select the criterion. Validate the window. Click the Refresh icon.

All parts or assemblies of the chosen class and its subclasses will be found.

4. Result. Search results are displayed in the lower part of the search window. These results can be displayed in preview or in a drop-down list be clicking on the icon. One of the results can be dragged into the graphic zone. Thus, the part or the screw that was found will be directly in inclusion mode. It is possible to select the columns to display.

If the message "Too many results: Refine your search criteria" appears, you must: Modify the criteria by being more precise. Modify the number of results in the Tools - Options menu. This modification may result in longer search times.

To accelerate the search time, being as precise as possible and avoiding ambiguities is advised. A search for "Screw" will be less effective than a search for "Hexagon head screw" If you know that the part is in such-and-such project, then do not search in all the projects. It is possible to reduce the number of results in the Tools - Options menu.

Full screen Links/Videos:

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This mode allows to switch TopSolid in a full screen mode. The system bar, the banner, context tabs and the different trees are not displayed.

Creation stages / Use: Click the icon in the Home tab, or select the View > Full screen... command from the TopSolid button.

By moving the mouse to the top of the screen, icons bars appear without the banner.In this case, opened documents tabs aren't visible. By moving the mouse to the top of the screen, it is possible to pin to be able to display icons bars and opened document tabs. The F11 kay allows to switch from full screen to normal screen and vice versa.

Dialog on document

This command displays the dialog of the different functions in the documents window and not in the tree. In this case, the dialog will still be visible on the document, as long as the corresponding function is not validated or canceled.

Creation Stages / Use: Select the Display > Dialog on document... command from the TopSolid button.

When the background of the icon is colored, the option is activated.

Home Page

This command allows you to display the home page where you can quickly access the last opened projects and documents and documents related to TopSolid.

Creation Stages / Use: Click the Home Page tab. If not displayed, select the Display > Home Page command from the TopSolid button. The home page is divided into several sections: from left to right New document: Allows you to directly create a new document. When TopSolid is first started up, the order of proposed documents is found in the Common tab of the New Document command. Then, the most frequently used document types are proposed.

Documentation: Allows quick access to TopSolid documents. (Tutorial, User Guide, What's New, Help).

Internet: Allows quick access to all TopSolid tools requiring Internet access (Search for updates, Update Notes, TopSolid on the web).

Recent Documents: In the middle pat of the home page, double-click the document to open. You can modify the preview size by clicking the

Recent Projects: Allows quick access to last open projects.

icon.

You can access the home page at any time by pressing CTRL+Q.

The version of TopSolid is indicated under the Internet section.

Available options: Display this Page at Startup: Check this open to display the home page each time TopSolid is launched.

Modifications / Additional information: You can reset recent document and project lists by using the Erase All popup command in the sections to empty.

Lock windows Links/Videos:

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This command prevents an unfortunated click to modify the setting or the position of windows defined by user. Windows can not be moved/hidden/folded anymore, but they can be resized. Projects are excluded from this rule and can be closed.

Creation stages / Use: Select the View > Lock windows... command from the TopSolid button.

The projects window is not taken in account and can be closed. Non pined windows or outside the application (for example when the trees window is in a second screen) are not taken in account.

When the Windows lock mode is activated, a small padlock is displayed in the window banner (near the pin and the X to close the window).

Preview mode

This mode activates or deactivates the preview of the functions during the creation or modification of shapes.

Use: Click the Preview icon in the Home tab icon bar.

During the creation or modification of functions in very complex parts, the preview display can slow down computer performance, therefore deactivating this mode is advised.

Additional information: This mode is enabled when the icon is pressed down. (the background remains in color). This mode applies to all the documents in the TopSolid session. When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

History

This command allows you to search the history to find all the PDM actions done by a user during a set period of time, regardless of the documents.

Creation Stages / Use: Select the PDM > History... command from the TopSolid button. Select the different settings to find the history. For example, to consult all what the user U1 has checked in during this last month: Start date: enter the date (one month before). End date: Insert the day. User: Select U1 from the list. Actions: Select Storing into vault.

Available Options: Refresh: Allows you to update information after changing the search criteria.

Date: Allows you to set the start and end dates for the history.

User: Allows you to select from the users list which one you want to see the modifications history for.

Actions:

Allows you to select one or all PDM actions (storing into vault, validation, etc.)

Each line displayed represents a PDM action. The information they contain match the confirmation window of these actions. By double-clicking on the line, the details of the PDM action are displayed (contents of the actions' confirmation window). To view a document's history, use the History function in the popup menu on the document.

Viewing: By double-clicking on the displayed line, a new window opens to show all the information about the action. The window has two parts. On the left is a summary of the information: Action date, user performing the action, action type, comments entered during the action, and in the minor revisions section, the name and minor version of the document. On the right is an overview of the document.

The comment can be modified via this window or via the Others > History contextual command from the project. A double click on the preview allows to zoom and rotate the document.

Connection

This command allows you to connect to the PDM by identifying yourself.

Creation Stages / Use: Click the Connection icon or select PDM > Connection... from the TopSolid button. 1. Select the PDM server from the drop-down list. It can be local or remote. 2. Enter the user name known by the PDM. Doing so is not possible if the PDM server is local. 3. Enter the password, the letter case is case sensitive. 4. Validate.

Available Options: New server connection. Click this link to create a new connection to another PDM server.

Server connections. Click this link to modify an existing connection to a PDM server.

Don't show at startup. Check or uncheck this option. If an identification is requested with a password, this dialog will appear upon connecting, even if the option is not checked.

Read-only mode.

Check this option to allow a same user to be connected to several TopSolid (by in read-only mode = only to consult).

Declare New Connection to Existing Server and Configure Server Connections are only used during the first use of TopSolid or in case of change of the Pdm server address. If an authentication is requested with a password, this connection dialog will appear, even if the option is not checked.

During the first connection, it is asked to import libraries. If you answer YES, import time can take several tenth of minutes .If you answer No, only needed libraries like TopSolid Mechanical (for TopSolid'Design) will be imported. This library contains some templates, main matters, threading standards, ... The same type of libraries exists for other TopSolid modules (TopSolid'Cam, ...). If you have answered NO or after an update of the application, during next connections, it will be proposed again a list of nonimported libraries. In this case, check the libraries to import and select one of these 3 options: Always ask to install available libraries:As soon as a new library or a library's update is available, it will be proposed. Ask to install only updates of installed libraries:If, during an update, new libraries are available, they will not be proposed in the list. Only updates for installed libraries will be proposed. Never ask to install available libraries:New libraries and libraries updates will not be proposed. This kind of libraries import can be modified with the Tools > Options > PDM command.

My account

This command allows you to configure a PDM account.

Creation Stages / Use: Select the PDM > My account... command from the TopSolid button. 1. Change the desired information. You can modify the last name, first name, initials and password. The value entered for the initials will automatically populate the Author fields in the title block. 2. With the client/server mode, you can enter your e-mail address which can be used with the workflow. The mails are sent to your external mailbox (Outlook, or other). 3. With the client/server mode, you can configure the SMTP outgoing mail server allows to configure it to be informed for example, when working at home. Your professional e-mail address must be accessible from the extranet.

The password allows you to secure your identity. It should not be shared. In case of loss when using the client/server, the PDM administrator can configure again your account. When using the local PDM, please contact the support. The password has to be entered a second time. The copy/paste is not allowed. The case sensitive must be respected. The e-mail address can only be used with client/server mode and by the workflow. To be used, you have to configure a mail server. It is not possible to receive mails.

It is not recommended to configure the SMTP server with your personal mail id and password for confidentiality reasons.

In client/server mode, the Groups tab displays groups in which the user is defined.

Users

This command is only available in remote PDM mode. It allows you to create and modify users, and enable or disable an account.

Creation Stages / Use: Select PDM > Users... from the TopSolid button. Click Add. Click Edit.

1. 2.

Click Delete. Select one or several names from the list. Allows you to delete one or several users. Deleted users can't be restored.

If a user has documents under modification or creation, it is not possibl delete him. On the other hand, if he has checked in or canceled his cha his deletion is possible. The deletion is never done in the database, the user is just non usable

Click Disable. Allows you to disable a user account. The user will not be able to log into the PDM. Click Enable. Allows you to enable a disabled user account. Click Export users. Allows you to export a list of users in a .csv file.

Into the .csv file, dates are saved with US format (only format supported

Click Import users. Allows you to import a list of users. For example a list coming from Microsoft Active Directory can be used to create users in TopSolid. The file has to be a .csv file.

To know the this csv format, just create a user in TopSolid and export it have an example.

Additional information: The Show disabled users option allows to display them in the list.

User is really created in the database when the window of creation is closed. An user can only be deleted if no document is out of the vault. But, it will be not deleted of the database because some documents like draft (title block) references it in the property "author". Suppression of user is irreversible. The Initials field allows you to automatically populate the Author field (title block, etc.)

Only users with administration rights are authorized to use this command (by default, only the "Admin" account get them).

User Groups Links/ Videos:

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This command allows you to manage user groups. By managing securities, you can assign them to either each user one by one, which can take a long time, or assign them to a user group. (For example, there can be a consultation group, a designer group, etc.)

Creation Stages / Use: Select PDM > User Groups... from the TopSolid button. 1. Select Add or Modify. 2. Enter the name and the group designation, then add or remove users from the group by clicking Select or Remove. 3. Validate.

Available options: Add: Allows you to add a group. Modify: Allows you to modify an existing group by selecting it and click Modify.

A user removed from the group is not permanently deleted. It no longer belongs to the group, securities assigned to the group will no longer be affected.

Only users with administration rights are authorized to use this function.

Security

This command allows you to manage TopSolid security by granting or not users or groups to perform actions on projects, folders or documents.

It is strongly recommended to use the security by using groups of users instead of directly users. Indeed, in case of adding a new user, he could be added in an existing group and will automatically inherit all these group rights.

Creation Stages / Use: Select Security... from the PDM menu of the TopSolid button. 1. Turn on security if necessary by checking this option. 2. By default, if a user is into 2 groups with different rights, the most permissive authorizations are applied. By checking Restrictive mode, the most restrictive authorizations will be applied. 3. Add or Delete the user or group by using the buttons, click the "+" in front of this user or group and select either Granted or Denied for each permission type. If both a user and a group are defined, the user security is applied even if the user belongs to this group.

Defined values are inherited by the Security command used from a project, a folder or a document. If Activate Security is not checked, the different authorizations are not taken into account.

Only users with administration rights are authorized to use this command (by default, only the "Admin" account get them).

The security can be defined in a project template. Then at each project creation, this security will be applied.

Available options: Protect with a password: The creation or the modification of a project, a library or a document can be protected by a password. For this, you have to choose the Protected mode and then click on the Modify button in order to define and confirm the password. Once the security with password has been defined, the Non protected mode allows you to de-activate it, however, the password is required to make this modification. The Reset button allows to delete all security definitions of the PDM. All projects, folders and documents will be impacted. The users and groups list used by the PDM security will also be cleaned. This button do not have any incidence on the protection with password.

Connection Links/Videos:

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This command allows you to connect TopSolid to TopSolid'Erp to retrieve data informations or to create new datas in TopSolid'Erp.

Creation stages / Use: Select Erp > Connection... command from TopSolid button. 1. Enter TopSolid'Erp server IP address or its name. 2. Validate by clicking .

If the address is empty, Erp commands will not be available on documents in the projects tree.

Available contextual commands are: Publish to Erp Unpublish to Erp Erp data

Exit

This command allows you to exit the TopSolid application.

Creation Stages / Use: Click the Exit (the upper right-hand "X" ) icon or select Exit... from the TopSolid button. If, after opening, no changes have been made to the documents or to the PDM, TopSolid will close. If any documents or projects have been modified, a warning message will be displayed for each open project undergoing modification.

Available options: Store objects into the vault and close: This option allows you to store modified objects into the vault before closing the project. Save the project and close it: This option allows you to save the modified documents and the project before closing. The files remain in the workspace and are not available to other users. Close the project and discard the last modifications: This option closes the project without saving the modifications. All of the modifications will be lost!

The documents that are modified, not saved or not put back into the vault have an asterisk next to the name in the tab of the window.

By using Close the project and discard the last modifications, all the modifications will be lost!

Tutorial

This command opens the tutorial, where you can follow simple exercises to learn more about TopSolid.

Creation Stages / Use: Select Help > Tutorial... from the drop-down menu or directly from the link on the home page in the documentation section.

A pdf reader has to be installed. There are several free readers available. When installing TopSolid, you are asked to install a PDF reader.

User Guide

This command displays the TopSolid 7 user manual.

Creation Stages / Use: Click the

icon from the Help button to display the user manual.

Displaying this manual requires a recent version of Adobe Acrobat Reader or equivalent.

What's New

This command opens the What's New document.

Creation Stages / Use: Select Help > What's New... from the drop-down menu or directly from the link on the home page in the documentation section.

A Pdf reader has to be installed. Several free readers exist. When installing TopSolid, you are asked to install a PDF reader.

Library Designer guide Links/Videos:

- - - Links - - -

This command allows to display the guide to design general libraries, standards or from manufacturers.

Creation stages / Use: Click the guide.

icon from the Help button to display the Library Designer

Displaying this manual requires a recent version of Adobe Acrobat Reader or equivalent.

Automation guide

Links/Videos:

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This command allows to start the guide that explains how to drive TopSolid from another application to automate some frequent tasks.

Creation stages / Use: Select the Automation > Automation guide... command from the button.

A PDF reader must be installed on the computer. The different commands are explained in the Automation help.

A development environment compatible with DotNet 4 like for example Microsoft Visual 2010 must be installed on the computer (not supplied by TOPSOLID).

Automation help

Links/Videos:

- - - Links - - -

This command allows to start help to explain how available commands work to be able to drive TopSolid from another software to automate some frequent tasks.

Creation stages / Use: Select the Automation > Automation help... command from the button.

Before starting, please read the Automation guide.

A development environment compatible with DotNet 4 like for example Microsoft Visual 2010 must be installed on the computer (not supplied by TOPSOLID).

Automation What's New

This command opens the Automation What's New document.

Creation Stages / Use: Select Help > Automation > What's New... from the drop-down menu.

A Pdf reader has to be installed. Several free readers exist. When installing TopSolid, you are asked to install a PDF reader.

Remote assistance

Links/Videos:

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This command allows the TopSolid support to have a remote access to your computer.

Creation stages / Use: Select the Help > Remote assistance... command from the dropdown menu. 1. Communicate the ID number and the password to your interlocutor to allow him to have a remote access to TopSolid.

An internet connection is required to use this command. The green light under your ID indicates that your connection is ready.

The connection is secured. It is active only during the opening of this command window. This command is only used with your agreement and only for maintenance. The TopSolid support has then a complete access to your computer, as if he was in front of your screen. To close the connection, just close the window by clicking the cross.

Search for Updates

This command allows you to search for TopSolid updates and its add-ins and to download them locally and/or to install them.

Creation Stages / Use: Select the Search for updates... using the Help button. A message indicates whether or not the installed applications are upto-date. The applications are up-to-date: Click OK to exit the window or Click Options to configure the behavior of future updates. The applications are not up-to-date: A window opens indicating the available updates. Click Download or Install Now to install the updates. In the case of installing, you must close TopSolid by clicking Close or click Install later to install the program later (only available after downloading in internet and server modes). Click Options to configure the behavior of future updates.

Available options: Update mode: Search for Updates on the Internet: This option allows you to verify the TopSolid website for the availability of updates. Updates are downloaded to be able to install them. An internet connection is required.

Client Mode: This option allows you to use the updates in a shared local directory when server mode is on. Please indicate the local directory for update repository by clicking on the Browse button. Server Mode: This option allows you to search for all existing updates on the TopSolid website, download them into a shared local directory and make the updates available on other workstations. Please indicate the local directory for update repository by clicking on the Browse button. An internet connection is required. Search for updates upon startup of TopSolid: This option allows you to search for updates each time TopSolid is launched Search for updates: This option allows to choose the frequency and the time to search for updates. Updates to keep in server folder: In server mode, it is possible to keep all updates, last 2 to 5 updates or just the last. Install updates: This option allows to automatically install updates after downloading. Applications to Update: The update search is global for all TopSolid products. If you do not use certain products, simply uncheck them in the list so as to not download their updates. For example, if you only have 64 bit versions, it is unnecessary to download updates for 32 bit

versions. Or if an old version of TopSolid has been uninstalled, you can unckeck it in the list.

During the update, TopSolid must be shut down. If TopSolid is started, you will be asked whether or not to stop it. If the server and client workstations haven't the same update, a warning message will appear when starting TopSolid.

When multiple workstations must be updated, it is preferable to configure server mode on one station and client mode on the others in order to prevent all workstations from downloading each update, so that only one workstation downloads the updates and provides them to the others. The release notes are also available from TopSolid'Update (in the right column).

TopSolid'Update uses the same port than the internet connection (generally it is the port 80). This port must be opened in the firewall. In some companies, the internet connection is done through a proxy. In this case, modify the proxy settings and/or thee proxy account by asking these settings to the network administrator.

Update Notes

This command allows to display a non exhaustive list of corrections et changes made in different TopSolid Service Packs.

A PDF file reader must be installed to view this document.

Update notes are also accessible when searching for updates (icons at the right).

Access to TopSolid'Store

Links / Videos :

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This command allows to access to the download of online products (libraries, applications, ...) on the TopSolid'Store shop. This shop contains textures. It is frequently completed.

Creation stages / Use: Click the icon or select the Help > Access to TopSolid'Store... command from the drop-down menu. This command is also available from the home page.

1. Select the language (upper left) then click on CAD or on the image. You can also use the search field.

2. Select the wanted product by clicking the image or the view details button.

3. Click on download. When the installation file is downloaded, it must be manually installed. TopSolid must be sto during this installation.

An internet access is required. Some products to download might be payable. An account has to be created or used to buy products. Free of charge products can be downloaded without account.

Modifications / Additional information: After the installation of the downloaded product, the checking in of the new library will be asked when starting TopSolid. If a client-server pdm is used, this download and this ckeck-in have only to be done once.

If several local pdm have to be installed with this downloaded product, simply install it on the different workstations. It is not necessary to download it on each PC.

TopSolid on the Web

This command allows you to go to http://www.topsolid.com

Creation Stages / Use: Select Help > TopSolid on the Web... from the drop-down menu or directly from the link on the home page in the documentation section.

This command opens Internet Explorer in a new TopSolid tab and connect to www.topsolid.com

Licenses

This command manages the licenses.

Creation Stages / Use: Click the Licenses... icon from the Help button. 1. The upper part of the window: Protection status: Indicates whether the license is valid or if it is in demonstration mode (no licenses). Available licenses: Show the list of available licenses, with its description, its status (valid or not), the type of license (key, etc. ), the expiry date if the license is temporary, and the licensing.

It is possible to delete a license from the list by using the popup menu and by choosing Delete the license. The check before each license allows to quickly activate or deactivate a license.

2. The lower part of the window is composed of 2 tabs. One for managing the standalone licenses and the other for network licenses. Standalone licenses: A standalone license is assigned to a protection key located on the machine. Download the licenses: When your licenses have been generated by your sales agency, click the Download licenses button to install them automatically. The downloaded licenses will appear in the list of available licenses. Add license file: Indicate the license file (TopLic extension) provided by TOPSOLID or one of its authorized resellers by clicking on the Add

license file button. The added file appears in the list of available licenses after confirmation of it having been added. Machine identifiers: The machine identifiers (key, etc.) indicated allow you to request codes that are specific to an identifier.To request the code, just click the Copy value button and paste the results in your e-mail message in your e-mail software program. Protection key is the identifier of the Sentinel protection key. Network adapter is the identifier of the network adapter. It is used only for temporary licenses. Floating licenses: A floating license is a license installed on a license server and which will be issued upon launching TopSolid. Many machines can log into the license server, up until the number of available licenses is reached. Additional machines trying to log in will start in demo mode. Name or IP address of license server: Indicate the name or the server's IP address, then click the Apply button.

It is possible to fill in several license servers by separating them with semi-colon (;).

Add a floating license: This list contains all of the floating licenses installed on the server. Select a license and click the Add license button, the license will appear in the available licenses list. Refresh updates the list. The Licenses in use button allows to display already used licenses and to know who uses them. Commuter licenses: A floating license can be "taken" for a maximum of 30 days. This option which is very practical for commuters, allows you leave with a license (it will no longer be available to other work stations). Simply click the floating license and from the popup menu, select Convert Mobile License. The license will be marked Floating (commuter) in the list of licenses. Upon your return, click the license and with the popup menu, select Uncommute License. The maximum duration can be chosen (number of days). If the commuter user connects gain before the end of the period, he can check-in commuter

license. After the defined period, the commuted license is automatically checked-in even if the user has not connected his computer. The expiration date takes in account the period.

It is possible to define the licenses to use in the TopSolid 7 shortcut. the "TopSolid'Design Light" license, the syntax will be ....\bin\Topsolid.exe" /lic "TopSolid'Design Light" The arguments list usable in the TopSolid shortcut are displayed by modifying it as follow : ....\bin\Topsolid.exe" /?

Only the user who converted the commuter license is allowed to Uncommute the commuter license. The commuter license is listed red. If the user who has checked out a commuted license reaches the en time, the license will be automatically checked in and available for ot users. The commuter user will have to connect to check out again th license. If the user who has checked out a commuted license reaches the en time, the license will be automatically checked in and available for ot users. The commuter user will have to connect to check out again th license.

3. Show license agreement allows you to reread the license agreement. 4. Validate.

Graphic Driver Links/ Videos:

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This command allows you to quickly provide all information on the card and graphic drivers and its compatibility with TopSolid.

Creation Stages / Use: Select Graphic Driver... command from the Help menu. Are displayed: the video card type, the installed driver and the recommend one. The card is not powerful enough to display the realistic rendering of work (old card or card without 3D acceleration) or the driver has known problems. In this case, contact TopSolid support. The card is supported and the driver is neither certified, or known to have particular problems. This is also the case for laptops who do not have an official video card driver, but rather a laptop constructor driver; the message indicates to use the latest driver provided by the laptop constructor; this is the case for GeForce Go 7xxxx; there are NVidia drivers for GeForce Go 8xxxx and more recent. If the driver is not certified, a link takes you to the constructor site for the update. The card and driver must work with TopSolid.

OpenGL Configuration: Useful information when the computer has several graphic cards. (example: an ATI FirePro or a Nvidia card AND an Intel or other card).It indicates which card manages the OpenGL (if it is managed by another graphic card than ATI FirePro or Nvidia card, a degradation of the display will probably be found).

If there is no validation (green checkmark), it is imperative to update the graphic drivers on the constructor site. If the problem continues, please contact your TopSolid support. To consult the recommended graphic cards, go to http://www.topsolid7.fr/requirements.html

About TopSolid

This command gives information on the TopSolid version (edition, update), the database version and that of the ParaSolid modeler.

Creation Stages / Use: Click the About TopSolid... icon from the help button. The highest part of the window indicates if the TopSolid version is a version for Windows (in this case 32-bit) or for windows 64bit. It indicates the exact version of TopSolid and also the current language. There are several tabs in the lower part. PDM: This tab indicates which PDM database is used and its version. When using as client/server, the name of the connection, the database type and its version. ParaSolid indicates the exact version of ParaSolid and ParaSolid Bodyshop modelers. Solver / Redway indicates the exact version of these 2 solvers. Startup indicates arguments added to the shortcut of TopSolid.

This information can be useful for the support. These informations cannot be modified except for language. The version can also be found in the application's banner and on the home page.

It is possible to change TopSolid current language by selecting a new one in the drop-down list. A restart of the application is required.

NOTE: The TopSolid improvement program is an optional functionality which allows to send static informations about your TopSolid activity. No personal information is collected, datas are anonymous. You can stop this program when you want by clicking again this link.

Activate preview Links/Videos:

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This mode allows to deactivate preview in certain operations.

Creation stages / Use: Click the icon or select the View > Preview... command from the TopSolid button. By clicking this icon, it is modified as follow: :

If deactivating the preview, it increases the performance during the operations calculation. If the background is orange, the mode is active. When the mode is active, it can be temporary deactivated in a command which manages this mode. If this mode is deactivated (no preview), it will not be possible to temporary activate it in the command.

List of the commands managing this mode: silhouette and revolved silhouette (2D sketch) silhouette (3D sketch) pattern union constrained transformation surface by formula deformation healing > adjust continuity offset

fillet draft trim trim by profile hollow thicken ....

Modifications / Additional information: You can activate again the preview in operations by clicking again the same mode.

Deactivated preview Links/Videos:

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This mode allows to deactivate preview in certain operations.

Creation stages / Use: Click the icon or select the View > Preview... command from the TopSolid button. By clicking this icon, it is modified as follow:

If deactivating the preview, it increases the performance during the operations calculation. If the background is orange, the mode is active. When the mode is active, it can be temporary deactivated in a command which manages this mode.If this mode is deactivated (no preview), it will not be possible to temporary activate it in the command.

List of the commands managing this mode: silhouette and revolved silhouette (2D sketch) silhouette (3D sketch) pattern union constrained transformation surface by formula deformation healing > adjust continuity parallelization

Modifications / Additional information: You can activate again the preview in operations by clicking again the same mode.

Overview of PDM commands

IT IS IMPERATIVE TO REGULARLY BACKUP THE DATABASE, VAULT AND WORKSPACES OF EACH CLIENT STATION ( if they are not centralized). ALL BACKUP INFORMATION IS INDICATED IN THE INSTALLATION GUIDE (DATA/BACKUP PROCEDURE CHAPTER ). FOR SECURITY REASONS, THESE BACKUPS HAVE TO BE SAVED ON ANOTHER DISK OR BETTER, ON ANOTHER SERVER.

Summary 1. 2. 3. 4. 5. 6. 7. 8. 9. 10. 11. 12. 13. 14. 15. 16. 17.

General Information. Installation. Listening port. Operation. Projects. Libraries. Documents. Templates. Vault. Cache. Workspace. Revisions. Collaborative work. Transfer. Bill of material. Back-up. Commands.

1. General Information. The PDM (Product Data Management) or TDM (Technical Data Management) allows you to manage in a flexible and secure way he data being handled; it is the backbone of the company and must simply be accessible to everyone. Basic services include the following: • A more advanced storage system than what is offered by Windows (Project Concept, Libraries, etc.). • Manage data associated with purely dealing CAD (Quotations, Explanatory Notes, etc.). • Quickly retrieve a part or assembly with certain properties (Business Number, Creation Date, Prix, xxx). • Know which assemblies use a given part (back references). • Automating updates and printing of all plans impacted by a change. • Managing part, assembly and drawing revisions. • Prohibiting changes to a part by two users simultaneously (collaborative work). • Secure data in a vault, as opposed to a work zone on the client side, with concepts of storing into the vault and taking out of the vault. • Managing the local "cache" concept to avoid systematically loading data through the network. • Managing access privileges. • Managing the work-flow, i.e. the sequence of steps required for the design and validation of a product. TopSolid’PDM is a simple PDM software that uses a free database engine that does not require administration. It must however ensure the basics: Project Management, Revisions, Secure Vault, ... TopSolid'PDM consists of a database that manages the information and location of documents, and a vault used to secure and store files. It is also necessary to set up a working directory on a local drive. Many types of usage are possible:

Single user In this case, TopSolid'PDM is setup in local vault mode. This light mode has a local PDM and vault. This set-up does not allow collaborative work. (When several people are working on the same project.) Teamwork In this case, the PDM server and the file server are centralized on one or more dedicated machines and users log in to work. Multiple PDMs When a user works in a team, they may wish to perform some work independently (drafts, prototypes, etc.) on their workstation, while benefiting from the project management features. They can access several local or remote PDMs. But each TopSolid session only allows you to login to a single PDM server. To switch servers, you must log out and log in again each time you switch or start a 2nd session of TopSolid.

2. Installation: Local installation For a single-user installation, TopSolid’PDM is only installed locally; you simply have to specify a particular directory necessary for proper operation. • The local directory where are datas and database (e.g. C:\TopSolid\Local). It is recommended that they have plenty of space and be regularly backed up.

Each terminal has its own vault and is stand-alone. Please read the installation guide for all information about installation, backup, migration to the new version, transfer to a new computer, migration to a pdm server, ... Client/server installation: When you have to centralize data, it is better to install an SQL database server. It is better to install an server application called TopSolid’PDM Server on a dedicated server machine, which is reliable and well-maintained, has plenty of disk space and is regularly backed up. This is a Windows service type server (it starts automatically when the machine is started). During installation, the administrator must define some specific directories required for the operation of the PDM server. The administrator must provide some information, such a name that will be used to identify the server from the client terminals.

In the case of the SQL server, the file server and the data server have to be one. Please read the installation guide for all information about installation, backup, migration to the new version, transfer to a new server, ... 3. Listening ports. TopSolid'Pdm Server is a netxwork service, communication between clients and servers are done through the network via the listening

ports. These ports have to be opened inlet and outlet.

8086: The PDM's main listening port. This port is used for the client connection. If it is changed, it has to be changed on the server and on all clients.

It is essential that the different required ports for proper operation of the PDM are opened in the clients' and servers' firewalls.

4. Operation. When first logging in to a remote server, the user has to log in. Then he is recognized and can access to projects and documents. A new PDM entry appears in the main menu, which contains several commands allowing you to control the PDM directly. Server administration is done from contextual commands of TopSolid'Pdm Server.

5. Projects. The data managed by the PDM is arranged in projects. A project can contain folders. Projects and folders can contain documents. This organization allows the user to perform a hierarchical division of the work based on a simple Windows file system-type method. This allows displaying the structure as a project tree similar to Windows Explorer, where everyone can immediately be comfortable using. You can simultaneously open several projects which leads to having several project trees displayed at the same time in the application window. A document can belong to only one project. Each project has certain properties that can be modified: Access Rights, ... You can also add other user-defined properties to each project, which can vary depending on the organization: business number, ... A project can reference other projects, in which case the documents it contains can reference documents from other projects. it can also reference a library. It is not possible to convert a project as a library.

6. Libraries.

Data having a similar nature, corresponding to frequently used items within projects, can be grouped in libraries. A library is managed like a project but with some specificities:. A library cannot reference a project. It can be delivered with a protection. It is not possible to convert a library as a project.

7. Documents. The PDM allows you to generate different types of documents. The primary goal is to manage documents from applications based on TopSolid, such as the bill of material, back references, the impact of changes, automatic update, etc. However, it also allows you to manage other types of companion documents (Word, Excel, etc.) but with fewer functions, yet retaining the management of revisions. It is possible to edit a document directly in TopSolid by doubleclicking on it in the project tree, which launches the associated application (assuming it is installed).

8. Templates. A project template is a predefined project which already has data, references and/or documents. Such a project template can be used as a basis to create a new project. All information, references and/or documents defined in the project template will then appear in the newly created project. A project template can be either personal (My Project Templates), or common to all users (Company Project Templates). Create My Project Template. Create a Company Project Template Using a project template. A document template is predefined document already possessing properties (units, frame step, form, etc.). Such a document

template can be used as a basis to create a new document. All properties defined in the template will appear in the newly created document. A document template can be either personal (My Templates), or common to all users (Company Templates). Create My Template. Create a Company Template. Use Document Templates.

There is no link between the template and the projects or documents created. When documents or projects created from templates are modified, the template itself is not modified and viceversa. Company templates can only be accessed when used in TopSolid Client/Server Mode.

It is not recommended to add materials, user properties, environments in the "My templates" (or company templates) projects. In this case, if a template part uses a material saved in "My templates", the created part by using this template will be linked to this material. By exporting this new part as a package, and importing it in another Pdm, it will create a duplicated "My templates" project in this other Pdm. If a template document must reference other documents (material, coating, unfolding rule, ...), these documents should be in a library.

9. Vault. The PDM server data (local or remote) is stored in a secure vault, it is not directly accessible by the user (through Windows Explorer, for example). These files are stored in a unique directory selected during installation.

Obviously, this directory must be backed up regularly (daily) since it contains all the data; in case of a problem, simply restore it to start working again.…

When the user wants to switch documents for consultation, the PDM server finds the location of the file which causes it to be loaded as read-only by TopSolid. When the user wants to change a document, the PDM creates a copy of the document on the client's terminal, in an area called the workspace. These files are stored in a unique directory selected during installation. When a document is being modified on a client terminal, no other client terminal can modify it (it can only be checked out once); it does, however remain accessible for consultation. Once modifications to the document are done, the user can put the modified version in the vault. That is called checking in. The changes now become accessible by all. In addition, the document becomes editable again. When checked in, the document disappears from the client's workspace.

The vault can be either a Windows directory on the server or an FTP server (used mostly for security reasons, if the file server is not on the same terminal as the PDM server).

10. Cache (only in pdm client/server mode). When the PDM server is on a remote terminal, loading the files directly over the network can be taxing. It can be useful to manage a cache on the local terminal where a copy of certain documents from the vault will be temporarily stored.

When the user asks to view a document, the PDM will first look in the cache to see if it is there, if not, it will make a copy from the server's vault, and then cause TopSolid to load the local copy. The contents of this directory can be deleted without any problems, its contents does not need to be saved.

11. Workspace. When the user checks out a document for modification, the document is transferred to a working directory called Workspace. The document will remain there until the document is checked in. By default, the workspace of each user is centralized in the same folder than the vault. It facilitates the data back up and the user will have his workspace regardless the workstation he is working on.

The cache and the local workspace folders are merged in the same folder. For performances reasons, it must be on a local disk. If the workspace is centralized, this local folder can be purged and doesn't need to be daily backed-up.

12. Revisions. The PDM allows you to track all the changes to the managed documents, thanks to the revision concept. A revision consists of two parts, major revision and minor revision. When you change a major revision, it means that your are going from one real part to another, both having their own existence: there could be machines (old) using the part Platen.A, and more recent machines using part Platen.B. Both parts can have different references, different prices… On the other hand, a minor revision change means the evolution of the same part being designed.

The real part corresponds to the one with the latest minor revision. For example, if assembly Machine.B.6 uses the part Platen.A., and a new revision Platen.A.4 is put into the vault, the assembly is considered as not up-to-date. Next time it is checked out it will be automatically redirected to Platen.A.4 and updated. On the other hand, if a new revision Platen.B.1 is stored into the vault, the assembly is considered up-to-date. If the user wants to use the new revision in the assembly, the latter will have to be modified (at the risk of changing the major revision of the assembly). Platen.A.1 Platen.A.2 Platen.A.3 Platen.A Transfer to another server chapter of the installation guide. If the database is manually backed-up with MicroSoft SQL Studio Management or by script, the Read-only Backup option must be checked. if not, the incremental backup after this manual backup will not be done and a complete backup will be done instead. See the installation guide (Data / Manual backup) to activate this option. It is recommended to select this location on another disk or better on another server. In this case, the user of the TopSolid'Local Pdm Server service can't be "local" but has to be changed with a domain user with writing rights in the destination folder. It is recommended to use the domain administrator. To change the user of this service, run the services.msc command, right click on the TopSolid'Local Pdm Server service and select properties. then change the user in the log on tab. The service has to be restarted.

The database as well as all data from the vault and the workspace are saved. A complete and 2 incremental backups can be done per day. The planning doesn't create a Windows planning task. If the maximum number of kept backups is reached, the next backup replace the first one.

Use for the restoration:

Select the Backups... command from the TopSolid button.

1. In the list of created backups (4), select the one to restore. 2. Use the Restore contextual command.

The Restore command can't be used when transferring to another pc. In this case, use the Extract contextual command which is explained below. When a incremental backup to restore is selected, the complete backup and all intermediate incrementals are also restored. They are displayed on a yellow background.

The database as well as all data from the vault and the workspace are restored in their previous location.

Available options by contextual menu on the listed backups:

Delete:

This command allows to delete a listed backup.

Extract:

This command is only available when starting TopSolid as advanced mode (by adding the -a argument to the shortcut). It allows to extract files and database contained in one of the listed backups (4). It is useful to transfer to another pc (read corresponding chapter in the installation guide. In the case of incremental backups use, you have to extract the main complete backup and all incremental backups.

Global Part Numbering

Links/Videos:

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This command allows you to define the part numbering of each document types with texts, data (project name, customer name,...) an a counter. This is a global part numbering for all the new projects.

Creation stages / Use: Select Pdm > Part Numbering... from the TopSolid button. Click Add Type to select the type of document on which you want to define the reference then use the Add counter, Add string and Add data buttons to define the information to display in the reference of the documents. An example of the defined part numbering is displayed at the bottom of the window.

Part numbering can also be defined locally on the project level by using the Part Numbering contextual command from the project tree. As a reminder, the reference of a document is visible (and can be modified) from the project tree using the Properties contextual command of this document or from the Parameters > System parameters folder of the

entities tree when the document is opened.

The defined part numbering does not affect existing documents. To modify the part number of an existing documents, use the New part number option of the Properties contextual command from the document.

Available Options: Add counter: The counter increments for each new creation. It can be made of numbers (numerical) or letters (alphabetical). The initial value corresponds to the start value of the counter. The minimum number of characters allows you to get a reference with always the same number of characters. The fill character allows you to define the character to use when the minimum number of characters if different than 1. For example with a minimum number of 3 and the fill character 0, you will get the following counter: 001, 002, etc For example with a minimum number of 3 and the fill character -0, you will get the following counter: --1, --2, etc

Add string: Allows you to enter characters (or separators).

Add data: Select the data type to display, such as project name, folder name, creation date or other. For the creation date, you must also enter the date format.

Apply part numbering at creation: When this option is checked, the part numbering is applied as soon as the document is created.

Check part numbering during input: This option allows you to check the unicity of the reference during its modification. It can be activated even when no part numbering has been defined.

Modifications / Additional information: You can change, delete or re-order the part numbering using the Modify, Delete, Up or Down buttons.

Part Number Checking Links/Videos:

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This command allows to list all documents of all projects with the same part number. Only part numbers used several times are listed.

Creation stages / Use: Select the PDM > Part Number Checking... command from the TopSolid button.

This command checks all projects. This operation can take a while according to the projects quantity and the number of documents in each project.

Available Options:

Folder view:

In the first column, are listed all part numbers used at least 2 times. Unroll the part number to see the documents using them.

Flat view:

In the first column are listed all documents with a common b ih h d

Life cycles Links/Videos:

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This command allows you to define the sub-states of the life cycles. The current states are: Design, Validated, Obsolete and Deleted. The life cycle can be used manually from the project tree by using the (Life cycle) popup menu on the document.

Creation stages / Use: Select Pdm > Life Cycles... from the TopSolid button. 1. Select the state to complete. 2. Click the Add button. 3. Select which document types will be concerned by this substate: All types. Only selected types: Select them in the list and click the green arrow to move them in the right side column. All types except selected ones: Select types which are not concerned by moving them on the right side column. 4. Enter a sub-state name and the document types. 5. Validate by clicking

Main states cannot be renamed. The scheme is displayed below.

When sub-states are not defined in the right order, simply select one from the tree and drag it to the right place. The search tool also allows you to search by state or sub-state. The option Publishable allows to choose which Life Cycles is publishable to the ERP/PLM connected.

When using TopSolid in client/server mode and if a workflow is defined, you cannot manually select a sub-state. This is automatically changed based on workflow progress.

Available Options: All Types: The defined sub-stated is available for all types of documents (Part, Assembly, Draft, Bill of Material, etc.)

Only selected types: From the list at the left, select the types of documents that use this life cycle sub-state and click the arrows to move them to the list at the right.

All types except those selected: From the list at the left, select the types of documents that do not use this life cycle sub-state and click the arrows to move them to the list at the right.

Modifications / Additional information: You can delete or rename a sub-state using the popup menu of this sub-state.

Life cycle scheme:

Workflow Links/Videos:

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This command allows you to define a document state change cycle based on the life cycle (Workflow) and by respecting the internal process of the company. These state changes can be submitted for approval.

Creation stages / Use: Select Pdm > Workflow... from the TopSolid button.

Workflows: Add workflow: allows you to create a new workflow including one or more actions. Modify workflow: allows you to modify an existing workflow by adding, modifying or deleting one or more actions. Delete Workflow: Allows you to delete the selected workflow. 1. Validate by clicking .

This command is only available in client/server mode.

Mail server

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This command allows to set the connection settings to an outgoing mail server. It allows to receive workflow notifications in case of modifications, without being connected to the PDM server.

Creation stages / Use: This window opens by using the PDM > Mail server command from the TopSolid button (to configure the general settings of the company e-mail server), or by using the Configure outgoing mail server > Add or Modify button from the Configure my account command.

Ask your system and network administrator the different settings to fill below.

1. Enter a name, for example your company name. This name only allows to distinguish the used mail server when several mail servers are set (for example, the company SMTP server and the company SMTP server accessible from home). 2. Enter the SMTP server address which is often a SMTP type SMTP.company_name.com. 3. Enter the port (generally 25).

4. Activate the SSL encryption if the server needs it. In this case, also enter the id and the password. 5. Enter a test mail address and click Send a test message to check settings. 6. Validate by clicking .

The e-mail address can only be used with the client/server and for the workflow. There is no link between TopSolid and your mail. The e-mail can only be automatically sent by the workflow. It is not saved in TopSolid. It is not possible to receive mails. It is not recommended to configure the SMTP server with your personal mail id and password for confidentiality reasons. Check that [email protected] is not in the blacklist.

File Extension

This command allows to list the extensions of the documents managed by the PDM of TopSolid.

Creation stages / Use: Select the PDM > File Extension... command from the TopSolid7 button (located at the top left of the application banner). The list of the document's extensions used in the PDM is displayed in a dialog box, these extensions can be declared in your antivirus software in order to not scan them and then improve the performances. Thanks to the Copy button, you can store all the extensions and paste them during the declaration into your antivirus (or other) software.

Add Project Template

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This command allows you to add a project to the list of project templates.

Creation Stages / Use: 1. Open My Project Templates or the Company Project Templates from the File > Templates folder of the TopSolid button. 2. Select Add Project Template... from the popup menu on the project in the project tree. 3. In the list of projects, select the project that will become the template. The Show Project Templates option allows you to select a project template that will be used as a base for the new project template. 4. Validate.

When a project is defined as a template, its entire contents (folders, documents, etc.) will be copied when creating a new project that uses this template. The new project created from a template is completely independent, that is, if the template changes (modified, deleted), the project created from it will not change.

Another way to create a project template is to open a project and use the Others > Add to Templates popup command.

Modifications / Additional information: To delete a project template, use the Delete Project Templates command. To modify a template project, open the project by checking Show Template Projects.

Add to Templates Links/ Videos:

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This command allows you to define the active project as project in the list of project templates.

Creation Stages / Use: 1. Select Others > Add to Templates... from the popup menu on the project. 2. Select the location of the template (My Templates or Company Templates). My templates can only be accessed by the user that created them. Company templates can be accessed by all users. 3. Add a folder if necessary with the popup menu on My Templates or Company Templates. 4. Validate.

When a project is added to the templates, its entire contents (folders, documents, etc.) will be copied when creating a new project that uses this template. The new project created from a template is completely independent, that is, if the template changes (modified, deleted), the project created from it will not change.

Another way to create a project template is to open My Project Templates or Company Project Templates and use the Add Project Template popup command.

Modifications / Additional information: To delete a project template, use the Extract Project Templates command. To modify a template project, open the project by checking Show Template Projects.

Extract Templates Links/ Videos:

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This command allows you to delete all templates from the list of project templates.

Creation Stages / Use: 1. Open the project to display it in the project tree. 2. Select Others > Extract Templates... from the popup men.

Another solution is to open My Project Templates or the Company Project Templates and delete the project that must no longer be a template.

This function does not destroy the project, it removes it from the list of project templates, then reappears in the list of classic projects that can be accessed with the Open Project command.

Back references

This command allows you to find an object's back references. For example, you can find out if a part to be changed is used and in which assemblies. The reverse function is References. The different functions are explained below.

You can add a new column (Project name, Author or other...) by right clicking a column title.

This command allows you to go back to the previous display.

This command allows you to go to the next display.

This command allows you to refresh the display. If a yellow triangle appears on the button, you need to refresh.

This command allows you to switch to reference mode.

This command allows you to switch to back references mode.

This command allows you to filter the document types to display.

Back references mode: (This command is only available with the Back references command.) This command allows you to filter the back references modes: Back references: This filter allows you to view all related documents. If assembly Assy.A.0 uses Part.A.0, the back references for modified Part.A.1 will show assembly Assy.A.0 since the latter will automatically be redirected to Part.A.1 when it is opened. Validated back references: This filter allows you to view only the validated back references. A part's back references only shows the validate assemblies that use it, not the minor revisions of this assembly. Non-obsolete back references: If a part is used in an obsolete assembly, the back references of the part will not show the assembly in this mode.

Back references of minor revision: If assembly Assy.A.0 uses Part.A.0, the back references of modified Part.A.1 will not show any assemblies. This filter is more restrictive than the first (Back references).

Another example about this last mode: Let an assembly Asm and a part Prt; with Asm.A.0 that has Prt.A.0 as reference (Prt.A.0 is included into Asm.A.0), but Asm.A.1 does not have anymore Prt.A.0 as reference (Prt.A.0 has been deleted from Asm.A.1). The references wil display: - Asm.A.1 => no reference - Asm.A.0 => Prt.A.0

The back references will display: - In mode "Back References" : Prt.A.0 => no back reference - In mode "Back references of minor revision" :

References

This command allows you to find an object's references. For example, an assembly's references are the parts and sub-assemblies it is made of. The reverse function is Back references. The different functions are explained below.

This command allows you to go back to the previous display.

This command allows you to go to the next display.

This command allows you to refresh the display. If a yellow triangle appears on the button, you need to refresh.

This command allows you to switch to reference mode.

This command allows you to switch to back references mode.

This command allows you to filter the document types to display.

Back references mode: (This command is only available with the Back references command.) This command allows you to filter the back references modes: Back references: This filter allows you to view all related documents. If assembly Assy.A.0 uses Part.A.0, the back references for modified Part.A.1 will show assembly Assy.A.0 since the latter will automatically be redirected to Part.A.1 when it is opened. Validated back references: This filter allows you to view only the validated back references. A part's back references only shows the validate assemblies that use it, not the minor revisions of this assembly. Non-obsolete back references: If a part is used in an obsolete assembly, the back references of the part will not show the assembly in this mode. Back references of minor revision: If assembly Assy.A.0 uses Part.A.0, the back references of modified Part.A.1 will not show any assemblies. This filter is more restrictive than the first (Back references).

Another example about this last mode: Let an assembly Asm and a part Prt; with Asm.A.0 that has Prt.A.0 as reference (Prt.A.0 is included into Asm.A.0), but Asm.A.1 does not have anymore Prt.A.0 as reference (Prt.A.0 has been deleted from Asm.A.1). The references wil display: - Asm.A.1 => no reference - Asm.A.0 => Prt.A.0

Import package. Which to select?

There are different ways to import package files depending on the result you want. What do you want to do? Do you want to import a complete project? YES

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NO

Export package

This command allows you to export documents or a complete project in package format (TopPkg). This format can only be used by another TopSolid user or with TopSolid'Viewer. This command is only available from the popup menu.

Creation Stages / Use: 1. Right-click to select one or more documents or a project and select the Import/export > Export package... command. 2. The window shows if your selection can be exported. 3. Check or uncheck Export only the view. The file you get if you check this option will be of small size, but can only be processed with TopSolid'Viewer. To be used only for consultation, for example. 4. Select the location of the package file on your drive and click Save.

Export options : Export all major revisions: During export, the last minor revision of the last major revision is exported. By checking this option, all major revisions will be exported. Export only the visualization: By checking this option, the generated file will only contain the visualization and it will only be possible to open it with TopSolid'Viewer.The file size is very small.. Create a self-executing package: The export generates an visualization executable file (.exe) which can be open by double-click without installing TopSolid'Viewer.This kind of files can be blocked by some antivirus or some mail software. When opening, it might be a warning Windows message..

Forbid to analyze geometry and to create graphical cuts in TopSolid'Viewer: By checking this option, the measurement and graphical cuts will be forbidden on the document, if the receiver uses TopSolid'Viewer.

You can export multiple files from the same project in the same package file by using multiple selection (holding the CTRL key down while selecting).

The documents do not have to be in the vault. However, if they are not in the vault, you cannot use the Import as Replication command and a new project will be created. If exporting for visualization (or auto-extractible) from a document, referenced documents by the selected document aren't exported to preserve the data confidentiality.

During export, the database information required for the selection, as well as the associated files, is included in the package (except in case of export for visualization).For example, exporting a package for an assembly should include all the required files, as well as the project name and the different folders if the documents used were in those folders. All other documents from this project which are not necessary to the assembly will not be exported, of course. By checking Create a self-extracting package or forbid to analyze geometry and create graphical cuts, the Export only the visualization option is automatically checked. The extension of the package export file is .TopPkg if the export file must be imported in TopSolid, it is .exe if the option "Create a self-extracting package" is checked and is .TopPkgViw if the package is for TopSolid'Viewer and only contains the visualization.

Import Package

This command allows you to import exported documents as a package. All the necessary references for these documents will also be imported. This command is only available from the popup menu on a folder or project.

Creation Stages / Use: Select Import/Export > Import Package... from the popup menu on a folder or project. 1. Select the package file (TopPkg) to import. 2. Validate. The documents contained in this file will be added to the selected project's tree.

The project and documents created are completely independent of those exported. It is an import of project as distinct copy. If documents to import have to be « recognized » and updated in the original PDM from where they come from, you have to use the Import project (by replication) command.

Available options:

Comment: This field is not used yet.

Vault of new project(s) to add: Each project is attached to a vault. Several vaults might have been defined by the administrator. In this case, select the vault to use in the drop-down list.

Conflict management in case of update: By importing a package as replication, it can contains a document which also exists in a project or in a library, with the same revision, but this document is different. There is a conflict to solve. For example, a subcontractor has modified a part you sent him, but during this time, you have also modified this part and they have both the same revision. Keep local version: The document which is in your vault will be kept and will replace the imported document. Update with imported version: The document which

Import Package as Associative Copy

This command allows you to import a package as read-only. An import folder will be created in the project tree. No notification can be made by the users on the files contained in this folder.

Creation Stages / Use: Select Import/Export > Import Package as Associative Copy... from the popup menu on a project. 1. Select the package document (TopPkg) to import. 2. Validate.

A folder named Import folder is automatically created in the project tree. The documents are read-only and cannot be edited. They can only be updated by re-importing the package with the Update by importing contextual command.

This importation mode can be useful for machining sub-contractors, for example. The sub-contractor receives from the client the part to be machined as an associative copy. This part cannot be modified; it will be identical to the one sent by the client. If the client makes changes, he will send a package which will then be imported using the Update by importing command. The versions will be verified.

Available options:

Comment: This field is not used yet.

Vault of new project(s) to add: Each project is attached to a vault. Several vaults might have been defined by the administrator. In this case, select the vault to use in the drop-down list.

Conflict management in case of update: By importing a package as replication, it can contains a document which also exists in a project or in a library, with the same revision, but this document is different. There is a conflict to solve. For example, a subcontractor has modified a part you sent him, but during this time, you have also modified this part and they have both the same revision. Keep local version: The document which is in your vault will be kept and will replace the imported document. Update with imported version: The document which

Update by importing

This mode works only with Import as an associative copy. It is only available on an import folder previously created with Import as an associative copy. It updates the contents of the import folder.

Creation Stages / Use: Select the Import/Export > Update by importing... from the dropdown menu. 1. Select the package document (TopPkg) to import. 2. Validate.

Update by importing is the only way to update documents imported in associative mode

Import file without conversion

This command allows you to import file from other CAD software, images, videos, Word or Excel documents, etc., but without converting them. It allows you to reference the files in the PDM to track or convert them later. This command is only available from the popup menu.

Creation Stages / Use: 1. Right-click a project or folder and select Import/Export > Import File Without Conversion.... 2. Select the document to be imported from the window.

You can drag and drop files from the Windows Explorer to the desired project or folder. If convertible files are dragged and dropped, you will be asked whether or not they must be converted.

Import file with conversion

This command allows you to import files from other CAD software by converting them to the TopSolid format through the interfaces. Some interfaces are optional and are therefore not available. To view the interfaces and the supported versions, click here. This command is only available from the popup menu.

Creation Stages / Use: 1. Right-click a project or a folder and select Import/Export > Import File with Conversion.... 2. Select the document to import from the window. Depending on the type of file, some options are available that simply need to be checked: Transfer assembly structure. If the file to be imported is an assembly, each part and subassembly will become TopSolid documents. If the file to be imported is a part or if the option is not checked, only one document will be created in TopSolid. Create an assembly document for files containing multiple bodies. A part may contain multiple bodies, for example, when you subtract a form from another. In this case, if the option is checked, the part imported into TopSolid will become an assembly with multiple referenced part documents. Transfer attributes. Some interfaces also allow you to retrieve the attributes (color, level, description) of imported parts. 3. A results window shows if the conversion was successful.

Importing a file requires converting the data. This operation requires system resources and can take some time depending on the size of the file. Documents that cannot be converted to TopSolid format (images, videos, Word, Excel, and CAD files without an interface) will be imported without conversion. The list of options can evolve depending on the types of documents.

You can drag and drop files from the Windows Explorer to the desired project or folder. You will be asked whether or not they must be converted.

Reference Library

This command allows you to reference one or more libraries in the current project in order to use certain items from the referenced library in the current project; such as, for example, screws, components, material....

Creation Stages / Use: In the project tree, right-click References, then select Reference Library from the popup menu. Next, select the library or libraries to reference from the window.

Additional information: You can delete a library reference. To do this, simply right-click the reference in the project tree, then select Delete.

Reference Project

This command allows you to reference another project in the current project in order to use certain items from the referenced project in the current project; such as, for example, parts, assemblies...

Creation Stages / Use: In the project tree, right-click References, then select Reference Project from the popup menu. Next, select the library or libraries to reference from the window.

Additional information: You can delete a reference to a project. To do this, simply right-click the reference in the project tree, then select Delete.

Convert file

This command allows you to convert files imported without conversion into the TopSolid format via the interfaces. Some interfaces are optional and are therefore not available. To view the interfaces and the supported versions, click here. This command is only available from the popup menu.

Creation Stages / Use: 1. With a right click on a non converted file, select the Convert File... command. 2. Depending on the file type, some options are available that simply need to be checked: Transfer assembly structure. If the file to be imported is an assembly, each part and subassembly will become TopSolid documents. If the file to be imported is a part or if the option is not checked, only one document will be created in TopSolid. Create an assembly document for files containing multiple bodies. A part can be made up of multiple bodies, for example when one form is subtracted from another. In that case, if the option is checked, the part imported into TopSolid will become an assembly with multiple referenced part documents. Transfer attributes. Some interfaces also allow you to retrieve the attributes (color, level, description) of imported parts. 3. A results window will show if the conversion succeeded.

Importing a file requires converting the data. This operation requires system resources and can take some time depending on the size of the file.

Open document

This command allows you to open a TopSolid document (part, assembly, draft, material, family, etc.) in your workspace.

Creation Stages / Use: Select the Open Document... popup command from the project tree or double-click the document in the project tree.

This command only opens the document. if no change is made to the document, it can be closed without saving. The document is in consultation mode until a change is made, in which case, it becomes a modification. Rotating and zooming are not considered as changes.

Double-clicking on the document will also open it.

By default, opening a document is in consultation mode, any change takes it out of the vault, which means incrementing the minor revision.

Open Main Document Links/ Videos:

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This command allows you to open the main document of the project.

Creation Stages / Use: Select Open Main Document... from the popup menu on the project.

This command is only available if a main document is defined.

When opening a project or if a preview appears when clicking on the project, a main document was defined.

Copy

This command allows you to copy one or more documents in the same or another project.

Creation Stages / Use: 1. Select one or more documents by holding the CTRL key down. 2. Select the Copy... command from the popup menu or use the Ctrl+C shortcut.

The documents are in the memory. You can paste them in the same project or a different one. The documents are renamed Copy of ... The copied documents are completely independent of the base document. If the base document is changed, the copied document will not evolve, and vice-versa. If the copied document must be independent from the original document, use the Derived part command. To copy only document entities (segments, operations, etc.), use the Edit > Copy function.

Redirect references

This command allows you to redirect the current documents references. For example, if an assembly uses parts that have evolved (P1.A has become P1.B), you can redirect the assembly to part P1.B instead of P1.A.

Creation Stages / Use: Select the Redirection > Redirect References... command from the popup menu on the object in the projects tree.

You can click in the last column to manually select the desired major version of the object, or the last minor revision of the last major revision. For example, if P1's history is P1.A.1 (minor), P1.A.2 (minor), P1.A (major), P1.B.1 (minor), P2.B.2 (minor), you can select P1.A and P1.B.2

Click the part of the assembly to highlight the corresponding line and click one of the lines to highlight the corresponding part in the open assembly document.

Available Options: Redirect all to the last validated version: This command is identical to the Redirect references to the last major revision command but only relates to the current document. It allows you to redirect references to the last major revision. For

example, an assembly consists of 2 validated parts (Part1.A and Part2.A). These 2 parts have changed independently from the assembly (Part1.A has become Part1.Ben and Part2.A has become Part2.Edo); you can redirect the assembly to their latest revision. The assembly will then reference Part1.A and Part2.E.

Redirect all on latest: This command allows you to redirect all references to the latest available minor revisions or the last major revision. For example, if the last major revision (P1.B for example) has not been modified, it will be selected for redirection. It the last major revision has been modified, the latest minor revision will be selected (for example, P1.C.4).

Preview: When clicking on this command, the display updates itself depending on the redirects you selected.

Redirect references to the last major revision

This command allows you to redirect references to the last major revision. For example, an assembly consists of 2 validated parts (Part1.A and Part2.A). These 2 parts have changed independently from the assembly (Part1.A has become Part1.Ben and Part2.A has become Part2.Edo); you can redirect the assembly to their latest revision. The assembly will then reference Part1.A and Part2.E.

Creation Stages / Use: Select the Redirection > Redirect references to the last major revision... contextual command from the project or from one or more objects.

This command can be used in multiple selection or from a project.

This command automatically redirects to the latest major revision of all objects.

Available Options: To manually select the major revision of each object, use the Redirect references command.

Redirect back references

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This command allows you to, when the minor revision of a document is modified, modify the revision of all documents that reference this document. It also allows to replace the selected document in all documents using it. For example, the Steel material can be replaced by another material in all parts with steel. (see the Replace by explanation below).

Creation Stages / Use: Select Redirection > Redirect back references... command from the popup menu on the document in the project tree. 1. Select the revisions to redirect by indicating the revision to redirect to. If Part p1 has the following revisions: p1.A.1, p1.A.2, p1.A.3, p1.A, p1.B.1, p1.B.2, p1.B, p1.C.1, you may wish to redirect all minor revisions A.x to C, so select Major A to Major C. In this case, all documents (assemblies, drafts, etc.) using p1.A.x will then use part p1.C.1. Documents using p1.B.x will continue to use p1.B.x. 2. Click the blue arrow to go to the next stage. 3. In the tree, check the different documents that will be impacted. 4. Click the blue arrow (right) to go to the next stage, click the blue arrow (left) to return to the previous stage. 5. Validate. This validation will display the result. The green checkmark indicates that the redirection was done, red crosses

indicate that the redirection failed.

If an assembly appears multiple times in the impact tree, selecting it once selects it everywhere. If an assembly is not selected, neither will its subsets.

Affected documents are opened, updated, then closed again. This operation can take a long time depending on the number of documents to modify and the complexity of the documents. Impacting a document creates a new minor revision to this document.

Additional information: The Replace by button allows to replace the selected Material or Coating document in all documents using it. For example, use this command from the Steel material of the Mechanical TopSolid library. Click this button, select a replacement material, then check all steel parts which must use this other material.

Main Document Links/ Videos:

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This command allows you to attach a document that will become the preview of a project or library.

Creation Stages / Use: Select Others > Main Document... from the popup menu on the document that will become the main document (Part, Assembly, etc.)

Only one document per project/library can be the main document. If a project/library already has a main document and this command is used from another document, the new document will become the main document. This command can be accessed from the popup menu on the project by selecting Open Main Document.

To modify the orientation of the document before defining it as main document, use the Visualization > Document preview command.

Workflow Links/Videos:

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This popup command allows you to assign a workflow to a project.

Creation stages / Use: Select Others > Workflow... from the popup command, on the project. 1. In the drop-down list, select the workflow to use. 2. Validate by clicking

A single workflow can be assigned to a project. All documents must be checked in to assign a workflow to an existing project.

For example, if a workflow is activated for a change from the substate of Design called "Prototype" to validated, you have to add a workflow for all each states, even without approving users (for example from Design sub-state None to sub-state Prototype).

Modifications / Additional information: In order for a workflow to no longer be assigned to a project, simply relaunch the command and select None from the drop-down list.

Security

This contextual command allows you to modify the security of the project, folder or selected document.

It is recommended to give authorizations to a group of users instead of users. When creating a new user, if he is integrated in an existing group, he will automatically inherit the same authorizations than others users of this group for each existing projects / folders /documents with securities.

The global Security of TopSolid must be activated. The project security must be activated to be able to visualize or modify authorizations of its folders or documents.

Creation Stages / Use: Select Security... from the popup menu of the project, the folder, the document to modify. 1. Activate security of the project if necessary by checking this option. 2. You can add or delete users or groups by using the and icons.

3. To define security by user or group, click "+" and select either Granted or Denied for each permission type. By default, for folders or documents, the authorization is inherited from the direct parent. If both a user and a group are defined, the user security is applied even if the user belongs to this group. 4. The Inherit information indicates that the security comes from the direct parent. For example, if an authorization is given to the project, all folders and documents are modified to take into account this authorization.

Default values are inherited by the Security defined by the PDM. If Activate security is not checked, the different authorizations are not taken into account. Activate security is only available on a project.

Only users with administration rights are authorized to use this command. If a user has administration rights, he has all rights even if some others are "Denied". If a user is in several groups, each with different authorizations, it is the authorization the most permissive which will be applied except if the Restrictive mode option is checked in the Security defined by the PDM. When the permission is Inherited, all customized security rights of children are replaced by permissions of the parent (folder or project).

The security can be defined in a project template. Then at each project creation, this security will be applied.

Available options: Protect with a password:

The creation or the modification a document can be protected by a password. When the global security has been activated and a password has been defined with the PDM > Security... command, then the protection with a password is inherited and it is not possible to deactivate it. However, another password can be defined locally on the project, a folder or a document. For this, choose the Protected mode, type the global password and then define the local password and confirm it. For this, you have to choose the Protected mode and then click on the Modify button in order to define and confirm the password. Once the local password has been defined, you can get back to the global password by choosing the Inherited mode, the local password is required to make this modification. When the global security has not been activated, you can define a password locally on the project, a folder or a document. For this, you have to choose the Protected mode and then click on the Modify button in order to define and confirm the password. Once the security with password has been defined, the Non protected mode allows you to de-activate it, however, the password is required to make this modification.

Delete

This command allows you to delete a document.

Creation Stages / Use: Select the Deletion > Delete... command from the popup menu on one or more documents in the project tree. 1. 2.

When deleting, a confirmation window shows the various documents that will be deleted, if the action is possible and, if not, the reason why. Validate.

You can delete by using the Del key on the keyboard. You can do multiple selections by holding the CTRL key down while selecting before deleting. A document under modification can be deleted without canceling changes. With the keyboard shortcut Shift(Maj)+Suppr, it is possible with one action : Delete + Check in + Purge. This action is definitive, it is impossible to restore the files deleted.

If the documents are unknown to the vault, (never checked in), they will be permanently deleted. As long as the project has not been purged, it is possible to restore deleted documents from the vault, by selecting them and by using the Cancel changes contextual command. A document from a deleted vault must be put back into the vault so that it disappears from the project tree.

Deleted documents are in the project recycle bin. To restore documents, select them and click Restore. Empty Recycle Bin (popup menu on the recycle bin) permanently deletes the documents. When a part used in an assembly is deleted, the deletion validation box specifies the name of the first assembly found by using the latter in the Comment column. After deleting the part, documents that reference it are marked as being out of date. When you open one of these documents, an update is performed and if Auto Heal Mode is turned on, the inclusion will be destroyed or become invalid.

Deleted vault documents are crossed-out in the project tree and preceded by a blue X. Storing the project into the vault deletes the crossed-out documents from the project tree.

Purge This allows you to purge deleted objects from the project.

Creation Stages / Use: Select the Deletion > Purge command from the popup menu on the object in the project tree. 1. Validate 2. When purging, a confirmation window displays the various objects to be deleted, if this action is possible and, if not, the reason why. 3. Validate.

Validating the purge permanently deleted the objects. This operation is irreversible.

Restore

This command allows you to cancel the deletion of the selected documents when they have been deleted and then checked in.

Creation Stages / Use: Select the command from the popup menu in the project tree on the deleted document(s).

It is possible to make multiple selections by holding the CTRL key while selecting before canceling the deletion.

Documents not known by the database (never saved or never checked in) and deleted are lost. Before being able to restore deleted documents checked in, you must use the View all documents contextual command.

Deleted documents from the vault and then checked in appear with a gray icon in the projects tree.

Rename

This contextual command allows you to rename an object or project.

Creation Stages / Use: Select the Rename... command from the popup menu in the project tree, or select the object or project and click again 1. Modify, then validate.

This command is only available from the popup menu in the project tree.

Pre-action summary window

This window summarizes the requested action before its validation and shows the effects of the change. For example, when storing a project into the vault, all the objects in this project will be listed and will show in the status column whether the action is possible or not. In case it is not possible, the reason why will be displayed and you will not be able to validate before resolving the problem.

Creation Stages / Use: This window appears whenever you attempt a PDM action requiring verification (check in, export, check out or cancel checking out, etc.). 1. Validate or cancel.

If none of the objects has an impossible status, the action can be validated. If at least one document has an impossible status, you have to cancel and resolve the problem before retrying the action.

Validate

This command allows you to validate one object. This object will move to major revision.

Creation Stages / Use: Select the Life cycle > Validate... command from the popup menu on one object. When the confirmation window opens, validate.

To be validated, an object has to be in the vault (blue padlock before the object in the project tree). A validated object becomes a major revision. Modifying a validated object moves it to the next minor revision. For example, part A.1 (minor revision) becomes part A (major revision) when it is validated. If it is modified, the new revision should be the same then the previous one. When it is saved, TopSolid analyzes if it corresponds to a true modification. If it is the case, the text of the major is incremented and changed to B. If not, it satys with A. In the case of a hardly in place assembly, it is synchronized with n parts. If the assembly is validta A and one of the part is modified, there are new major for the assembly and parts. When saving, the part really modified will have a revision B when all other parts will have A. - In some cases, A(1) is displayed because several majors have the same letter and TopSolid has to different them. (redirection, tree,...) - The analyze of the part is only be done when saving for performance reasons. The major is called A(i) by waiting the

save. If the user has a doubt, he can save to see if A(i) becomes B or will stay with A(i). Previous minor and major revisions can be viewed by clicking on the "+" sign before the object in the project tree and scrolling through the Revisions folder. When a document should no more be used, you have to make it obsolete.

In the context of exchanging data with import package by replication, validation must be done by one person only. This in order to avoid conflict / import failure if the same document is validated on two different PDM. Once a document is validated, it is no more possible to go back in a Design state for the same revision.

Additional information: Document in the vault, but not validated validated document Obsolete document

Make obsolete

This command allows to make obsolete a validated document, so that it is no longer used.

Creation stages / Use: Select the Make obsolete... contextual command on the needed revisions. 1. In the projects tree, click on the "+" in front of the document, then on the "+" in front of Revisions. 2. Select the Make obsolete contextual command on the validated revision you want to make obsolete.

To cancel this command, you have to validate again the revision.

Additional information: Checked-in document, but not validated Validated document Obsolete document

Check In

This contextual command allows you to check in one or more documents into the vault, as well as the whole project.

Creation Stages / Use: Select the Check In... command from the popup menu on one or more documents or in the project tree. Confirm checking in of the listed documents.

You can do multiple selections by holding the CTRL key while selecting before checking in.

Check in moves the document(s) from the workspace to the vault. When documents are again checked in, they are again available for all users. Check a document out to modify or open it allows you to take one or more document out of the vault.

Each instance of checking in creates a new minor revision of the document.

Check out For Edit

This command allows you to check one or more document out to modify it. The document is restricted but not opened in TopSolid.

Creation Stages / Use: Select the Check out for edit... command from the popup menu on the documents or in the project tree. Confirm checking out of the vault.

You can do multiple selections by holding the CTRL key while selecting before checking in or out.

You can only check out for modification documents that are checked in (blue lock in the project tree). The blue lock turns into a red check mark.

Checking out for edit creates a minor revision of the document. It is no longer available to other users.

Additional information: To be able to work on the document checked out for modification and display it in TopSolid, select the Open document contextual command when hovering on the document.

To cancel the check-out for edit, select the Undo changes contextual command on the document. No change made to the part since it was checked out will be taken into account. There will not be any command for the administrator to directly unlock a document checked out. The current solution is simple: - The administrator searches for the concerned user's password. - The administrator logs in with the user's login and password. - The administrator uses the Undo changes command on checked out documents.

Undo Changes

This command allows you to cancel check-out for edit or cancel the deletion of a part.

Creation Stages / Use: 1. Select Undo Changes... from the popup menu on the object or project in the project tree. 2. Confirm Undo

You can only cancel taking out of the vault for objects known by the PDM and taken out of the vault (they show a red check mark in the project tree). Following the canceling, they are again displayed with the blue padlock Undoing changes on a deleted document will cancel its deletion. You can make multiple selections by holding down the CTRL key before undoing changes. To restore the document state before it was saved, use the Restore Last Save command.

If the document was never checked-in (new or saved document), undo the change to destroy the file. Unkown documents by the database (never saved or never checked in) and deleted are lost. If they do not appear in the tree (the project was validated after deletion), you must use the View all documents contextual command. Deleted documents will be grayed out. In this case, click Restore.

Get Latest Version (Recursive)

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This command allows you to update the project manually. If a user checks a document in , this command allows other users to view this document.

Creation Stages / Use: Select Get Latest Version (Recursive)... from the popup menu on the project.

This command is only available in client/server mode. New documents not checked in can't been seen by other users.

Restore Latest Save Links/ Videos:

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This command allows you to return to the state of the document as it was before being saved.

Creation Stages / Use: 1. Select Restore Latest Record from the popup menu on the object or project in the project tree. 2. Confirm Undo.

Documents removed from the vault may have been saved multiple times. This command allows you to return to the document as it was before the last save. If you wish to restore the document as it was before removing it from the vault, use the Cancel Changes command.

You cannot restore the document by deleting multiple records.

History

This command allows you to see a document's history, as well as compare the overview of two different versions of the document.

Creation Stages / Use: This command is available only as a popup menu on the document. Select the document and select Others > History... The first column shows the dates and times of the different modifications. The second column shows the actions that were performed (storing into vault, validation, etc.). The third column shows the users who performed these actions. The fourth column allows you to see the different versions of the documents. The last column shows the comments entered by the users during the action.

You can select 2 lines to display the overview of the 2 documents for comparison. Comments can be modified via this command, or via the Modifications history command, by double clicking the corresponding line.

To view the history of all PDM actions regardless of the documents, use the command Modifications history in the PDM menu of the

TopSolid button.

Add to favorite Links/Videos:

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This command allows to create in the Favorite folder of a project, a shortcut to a document frequently used.

Creation stages / Use: Select the Others > Add to favorite... contextual command from a document. 1. Select the project whose the selected document must become a favorite.

When a project or library document is frequently used with another project, it is useful to set this document as a favorite of the project. A shortcut to the document is created in the Favorite folder of the project. It can be used instead of using the real document in the most common commands. It avoids to have to search the document in its original location (open the library, unroll folders...).

It is possible to drag a or several documents (multi-selection with CTRL) from the projects tree, directly to the Favorites folder of this same project. All types of documents can be added to favorites.

Workflow Links/Videos:

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This popup command allows you to request approvals from a document.

Creation stages / Use: Select the Workflow... popup command from a document. 1. Select a life cycle action from the drop-down list. 2. Enter a comment before validating. This comment will be visible to the approving user. 3. Validate by clicking .

When a request is in progress, an hourglass overlaps the document icon until the request is accepted or rejected. The Requests tab at the bottom of the screen allows you to view pending requests. All requests and request cancellations are saved in the document history.

A pending approval document can only be opened for consultation. You cannot modify it.

Modifications / Additional information:

On the Requests tab, you can move the document up the tree and move and delete the request using the corresponding popup commands.

Unpublish to Erp

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This command allows you to unpublish a published document, to be sure it will not be created in TopSolid'Erp.

Creation stages / Use: Select the Erp > Unpublish to Erp... command from the document contextual menu in projects tree.

To be able to unpublish a document, this document must be published to Erp and must not have been created in TopSolid'Erp.

Erp data

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This command allows you to display Erp informations for documents known by TopSolid'Erp.

Creation stages / Use: Select the Erp > Erp data... command from the document contextual menu in projects tree. All document ERP datas are displayed in a window.

Publish to Erp

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This command allows you to publish a document to TopSolid'Erp. Then, this document could be created in TopSolid'Erp, by using TopSolid'Erp command.

Creation stages / Use: Select the Erp > Publish to Erp... command from the document contextual menu in projects tree. 1. Validate window by clicking on

icon.

To be able to use this command, connection must have been defined. To be able to publish to Erp and to create data in TopSolid'Erp, the data must at least have a part number. the data must be checked in and validate. In case of problem during publishing, a comment is displayed in Comment column.

Modifications / Additional information: It is possible to unpublish a published to Erp document.

Defer operations

This mode allows to defer operations like (drilling, drillings group, pocket and boss) and also their repetitions.

Creation stages / Use: Click the icon or select the Edit > Defer operations... command from the TopSolid button. This mode allows to not calculate the geometry of these operations in this document. A significant increase in performance is observed with very complex parts (mold part, ...). Drillings are replaced by surface shapes allowing to visualize operations positions and to modify their parameters.

The deferred operations are displayed between [] in the operations tree.[Drilling 1]. This mode is only activated for the current document. This mode allows a significant increase in performance when modeling very complex parts (mold part, ...).

Available Options: Do not defer: When this mode is active, it is possible to not defer an operation via the right button, by selecting Others > Do not defer (from the operations tree or from the operation in the graphic area) .

As operations do not exist anymore after activating this mode, all entities hooked on these operations will become invalid (example: the drilling axis, the chamfer on the drilling edge, ...). Some operations can be automatically deleted if the update heals is active during the use of the defer operations command (case of the chamfer of the edge of the drilling).If the update heals is deactivated, this chamfer will be invalid.

Modifications: The deferred operations can now be refreshed manually in order to prevent their recalculation when saving. This mode might be needed for very complex parts and has to be used appropriately. If the Auto Refresh has been deactivated, operation can be updated from the Refresh button of the system bar.

Overview of sketch commands

In most common cases, the creation of a part or of an operation begins by a sketch. 2D sketch and 3D sketch menus propose you all functions for creation and for elements modifications. The 2D sketch menu is for the design of 2D sketches, the 3D sketch menu is for the design of 3D sketches. The different commands are going to allow you to model both simple geometric elements like lines, circles, rectangles... and more complex elements like splines, helices, curves by formulas...

Colors of the elements: In order to rapidly visualize the level of constraints of the sketch elements, TopSolid displays them in different colors. A totally constrained sketch will be represented in blue, whereas an under-constrained sketch will be represented in magenta.

Colors of dimensions: Like for sketches, dimensions are displayed with different colors to quickly distinguish constraints (dimension driving the geometry) to passive (dimension displaying a distance). A constraint will be represented in black, whereas a passive dimension will be represented in gray. If there are too many constraints, the sketch becomes overconstrained and TopSolid displays dimensions in red.

Construction elements and internal elements:

In some cases, it is necessary to model elements only useful for the construction of other elements. These elements will be able to be defined as construction elements, they will be represented by fine mixed lines and will not be taken into account during automatic sewing of the sketch elements, nor during the creation of a shape but they will remain visible outside the sketch, which will possibly allow other elements to be hooked on above. You can modify the type of element at any time by selecting it and launching the Construction command, which is available from the popup menu that displays by right-clicking the element. When an element of construction type is defined, it is possible to make it inside the sketch, it will have the same characteristics as a construction element but will not be visible outside the sketch. You can make a construction element internal at any time by selecting it and launching the Internal command, which is available from the popup menu that displays by right-clicking the construction element.

Modes: Different modes are available through the icon bars, modes are displayed on the right of the bar. They are also available from the 2D sketch > Modes or 3D sketch > Modes drop-down menus. Modes allow: automating the creation of some types of elements like for example construction elements. modifying the values of the dimensional constraints during their creation visualizing certain type elements like for example relations.

Creating the sketch "on the fly" In all commands requiring that a sketch be selected (extrusion, pocket, embossment, etc.), it is possible to create a sketch "on the fly", if it doesn't yet exist. To do this, use the corresponding command in the dialog's advanced options ( icon).

Sketch

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A sketch is created by selecting the support plane of the sketch among the predefined planes or directly from the graphic area by selecting a planar face on a part. A sketch is an element composed of geometric and constrained elements.

Creation Stages: Select the 2D sketch > Sketch... command from the drop-down menu. In a Draft document, select the Sketch > Sketch... command from the drop-down menu. If the document does not contain any sketches, launching the command automatically creates a sketch in the XY plane of the absolute frame. If the document already contains a sketch, you must select the support plane of the sketch. Once the sketch has been created, all of the commands of the Sketch menu become accessible. This mode is symbolized by the button containing the name of the sketch displayed in the top center of the graphic area, this button also allows you to exit the Sketch mode by validate it by clicking near the blue check. By clicking the red cross, you will quit the sketch edition and will cancel all what you have done during this edition.

Additional Information: This command is automatically launched by the entity creation command such as Point, Line, Rectangle,etc. Leaving the sketch mode is also possible through the popup menu by clicking on the name of the sketch or by selecting a creation command or shape modification command (Extruded, Sheet Metal on Sketch, Revolved, Pocket, Embossment).

Position sketch

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This command allows you to fix the origin and the axes of your sketch on a particular point of your part. A sketch is positioned by selecting a support plane, an origin and a direction (horizontal or vertical).

Creation Stages: You must first create a sketch. Once the sketch is created, click on the icon or choose the command 2D Sketch > Position Sketch... from the drop down menu. 1. 2. 3. 4.

Select the sketch's support plane. Select the point defining the origin of the sketch. Choose the direction you wish to define (X or Y). Select the direction defining the X or Y axis.

Modify grid

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This command allows the appearance of the entry grid and entry mode of the coordinates to be modified.

Modification steps: Click the icon or select the 2D sketch or 3D sketch > Modify grid... command from the drop-down menu. In a Draft document, select the Sketch > Modify grid... command from the drop-down menu. Choose the grid type from the 3 modes proposed: None The grid is not displayed the cursor is then free of all movement.

Points type grid (Cartesian)

Lines type grid

Choose the coordinate entry mode: In Cartesian mode the points are entered by indicating the X and Y coordinates In Polar mode the points are entered by indicating a radius and an angle. This mode is then used in all the sketch creation commands. Depending on the coordinate entry mode, set the different pitches of your grid. The Magnetization option corresponds to the number of intervals between two grid points. E.g.: On a grid with a pitch of 10mm in X and in Y and a magnetization of 5, it will be possible to position every 2mm in X and in Y. Adjustment of a grid in Cartesian mode

Adjustment of a grid in polar mode

The small red points represent the magnetic grid, in these examples magnetization has been set at 2.

The grid has an auto-adaptive pitch, i.e. depending on the zoom, the pitch is multiplied or divided by a factor 2, 5, 10,...

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This command allows you to define the revolution axis of the sketch for the commands: Revolution dimension, Revolved shape, Trim by profile (revolved) ...

Creation Stages / Use: Click the icon or select Sketch > Define Revolution Axis... from the drop-down menu. Choose the sketch's X or Y axis or an axis defined outside the sketch (external axis).

The default revolution axis is the X axis.

Available Options: Delete revolution dimensions: This option allows you to delete all of the previously created revolution dimensions.

Contour Links / Videos:

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The Contour command automatically allows a succession of lines and arcs to be created with coincidence relations.

Creation Stages: Click the icon or select the 2D sketch > Contour... form the drop-down menu. In a Draft document, select the Sketch > Contour... form the drop-down menu. 1. Chose a creation mode of the segment, the Line mode is chosen by default. Line

Creation of a line by two points. This mode contains 4 sub-modes allowing to move the cursor free vertically or both. : The cursor can move freely in the sketch plane : The cursor can move horizontally or vertically. : The cursor can move horizontally only.

Tangent arc

: The cursor can move vertically only. Creation of an arc tangent to the last element of the contour.

Perpendicular arc

Creation of an arc perpendicular to the last element of the contour

Arc

Creation of a circle arc by three points.

Passing

Creating a contour by passing over the existing geometries (edges sketch, etc.).

2. Enter passing points coordinates of the segment or click points in the graphic area.

If you wish to create a closed contour, finish your contour by clicking the start point of the contour again segment of the contour. Otherwise, click the icon or press the Esc key to exit the command and crea contour. The selected creation mode is used one time, after it switches to Line mode except if the Lock option is case the Interactive mode is not useful.

You can use the "A" key to switch from a line to an arc and vice versa. It allows to quickly create an obround.

Available Options: The Lock mode allows to lock the interactive mode to stay permuted. For example, if you move the cursor to the last segment of a line in progress, TopSolid automatically switches to tangent arc. When

the arc is done, it switches again to line. By checking this mode before position the arc, it will stay active and after position it another tangent arc is proposed Interactive mode allows to switch between different Line mode, Tangent arc and Perpendicular arc by moving cursor on the last edge of under construction contour. By default, in the circle, tangent circle or perpendicular circle mode, the circle arc is created in the trigonometric direction (counter-clockwise), check the Additional arc option to change to clockwise.

Additional Information / Modifications: When a contour vertex is selected again, the construction mode is automatically enabled. When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the element is created.

Contour wizard Links/Videos:

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This command allows to quickly create the sketch contour. For example, after cleaning an Autocad imported sketch, it will be possible to retrieve its contour with this wizard and then extrude it.

Creation stages / Use: Click the

icon or select the 2D sketch > Contour wizard... command from the drop-down menu.

1. Select Path or Region. 2. Validate. Path

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Select the first segment. Arrows on this segment allow to Invert, to continue on the left or on the right. The colo color of the icon in the dialog.

By clicking arrows in the workspace area, the path is defined until the next intersection. It is also pos the left side as needed. By clicking the direction icon in the dialog, this direction will be taken in account on each intersection

Imported sketch

The yellow arrow indicates the direction, the blue one the left.

Result by c

Imported sketch

In this case, you have to click the corresponding arrow to continue until the next intersection.

Result by se

Region: Select background sketch. When the sketch contains internal and external contours, you have to click near the c create the contour. It is possible to click outside the part to create its external contour. On below examples, the c on the background sketch.

Imported sketch

Click outside the sketch

C

It is possible to start a contour with the region mode, then continue it with the path mode.

Available Options: Detect real intersections: If this option is checked, and if the support sketch entities are not joined by one point, but cross themselves, they passing mode of the contour). If it is not checked, extremities must be coincident.

Support sketch

Without real intersections detection

Modifications / Additional information: If the wizard do not finish the contour (superimposed line, or other reason), you just have to edit the sketch and use this command again to continue the contour.

With re

Point

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A point is created either by entering the coordinates in the dialog panel, or directly from the graphics zone by locating a point or selecting an element.

Creation Stages: Click the icon or select the 2D sketch > Point... command from the drop-down menu. In a Draft document, select the Sketch > Point... command from the drop-down menu. Creation by the dialog panel: 1. Enter the points coordinates. Creation from graphic area: 1. Locate a point on the grid or select an element.

Modifications / Additional Information: Click on a point and move your mouse while holding down the left button to modify the position of the point.

When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the element is created.

Line

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A line is created either by entering the coordinates of the start point and end point in the dialog panel, or directly from the graphics zone by locating two points on the grid or on elements.

Creation Stages: Click the icon or select the 2D sketch > Line... command from the drop-down menu. In a Draft document, select the Sketch > Line... command from the drop-down menu. 1. Select the construction mode: 2 points: Creation by the dialog panel: Enter 2 points coordinates. Creation from graphic area: Locate two points on the grid or on elements. This mode contains 4 sub-modes allowing to move the cursor freely, horizontally, vertically or both. : The cursor can move freely in the sketch plane : The cursor can move horizontally or vertically.

: The cursor can move horizontally only. : The cursor can move vertically only. Point and angle: Enter the angle. The angle can be inverted regarding X axis by checking the option. (45° becomes -45°). Creation by the dialog panel: Enter start point coordinates. Creation from graphic area: Position a point on the grid or on an element. 2. Validate by clicking

.

It is possible to mix these creation mode. For example, enter the start point coordinates and click the end point in the graphic area.

Modifications / Additional Information: Displacement of an end: Click the end of a line and move your mouse while holding down the left button to modify the position of this end. Displacement of the line: Click the line and move your mouse while holding down the left button to modify the position of the line.

Available Options: Infinite: The checked option allows to make this line infinite and using the construction. mode In this case, this line will be displayed as a sketch

axis. It is defined by 2 passing points.

When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the element is created

Circle

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A circle is created either by entering the coordinates in the dialog panel, or directly from the graphics zone by locating a point or selecting an element.

Creation Stages: Click the icon or select the 2D sketch > Circle... command from the drop-down menu. In a Draft document, select the Sketch > Circle... command from the drop-down menu. Creation by Center and passing point: 1. In the Size topic, select Free size mode. 2. Check Given center. 3. Enter the coordinates of the center point and of a passing point of the circle.

Creation by 3 passing points: 1. In the Size topic, select Free size mode. 2. Uncheck the box Given center. 3. Enter the coordinates of circle passing points.

Creation by Center and Diameter or Radius: 1. In the Size, select the Diameter or radius mode. 2. Enter the diameter or the radius value of the circle. 3. Check Given center.

4. Enter the coordinates of the center point.

Creation by Diameter or Radius and 2 passing points: 1. 2. 3. 4.

In the Size, select the Diameter or radius mode. Enter the diameter or the radius value of the circle. Uncheck the box Given center. Enter the coordinates of 2 passing points.

No matter which creation mode is chosen, the circle is created with its center point.

Additional Information / Modifications: Click the circle or its center point and move your mouse while holding down the left button to modify the position of the circle. From the popup menu you can: Constrain the center of the circle on an element with the Define Center... command. When the center point no longer exists, recreate the center point of the circle with the command Create center. When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the element is created

Rectangle Links / Videos:

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A rectangle is created either by entering the coordinates of the rectangle diagonal points in the dialog panel, or directly from the graphics zone by locating two points on the grid or on elements.

Creation Stages: Click the icon or select the 2D sketch > Other curves > Rectangle... command from the drop-down menu. In a Draft document, select the Sketch > Other curves > Rectangle... command from the dropdown menu. 1. Choose a construction mode: Parallel to the axes

3 points, By base

The dimensions of the rectangle are parallel to the X and Y axes of the sketch's frame, the construction is done by giving the two points of the rectangle's diagonal. The rectangle is created by indicating the 2 points of the base then indicating the height:

3 points, By diagonal

The rectangle is created by indicating the 2 points of the diagonal then indicating the base position:

By size

The rectangle is created by entering its width, height and a positioning point key: Select the wanted key point (center, vertex or middle) by clicking it directly in the dialog panel (the point becomes cyan).

2. Depending on the mode chosen, enter the coordinates of the rectangle's construction points or locate them on the grid or on elements. Naturally, you can mix creation modes by indicating, for example, the coordinates of the 1st point of the diagonal in the dialog panel and describing an element to indicate the 2nd point of the diagonal.

Modifications / Additional Information:

A rectangle is composed of 4 segments. Each segment can be independently removed or modified independently. Click a segment or rectangle vertex and move your mouse while holding down the left button to modify the height, position or shape of the rectangle depending on the constraints that have been applied to it. When the mode Automatic dimensions is enabled, the dimensional constraints (driving dimensions) are also created. When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the element is created. To create a centered rectangle with an axis or with the sketch origin, you can position the first point of your rectangle, then move the cursor on the opposite side regarding the axis or the origin. When the center relation will be detected, TopSolid will framed the dimension with the = sign.

Regular polygon

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This command allows a regular polygon of n sides inscribed or confined in a circle to be created.

Creation Stages / Use: Click the icon or select the 2D sketch > Other curves > Regular polygon... command from the drop-down menu. In a Draft document, select the Sketch > Other curves > Regular polygon... command from the drop-down menu. 1. Choose the number of sides of your polygon. 2. Choose the construction mode: Internal diameter External diameter Internal radius External radius Internal free size External

The polygon is confined on the diameter indicated. The polygon is inscribed on the diameter indicated. Same as Internal diameter indicating a radius. Same as External diameter indicating a radius. Same as Internal diameter indicating the diameter in the graphics zone. Same as External diameter indicating the

free size

diameter in the graphics zone.

Length sides + center Length sides 2 points

The polygon is created by indicating the length of one side and its center point. The polygon is created by indicating 2 points determining the length of a side, the polygon can then be positioned either side of the line defined by the 2 points.

3. Depending on the construction mode chosen, enter the values and coordinates of your polygon.

Available Options: Polygon orientation: In internal modes (Internal Diameter, Internal Radius and Internal Free Size), you can orient your polygon by indicating the position of its first vertex or indicating the first tangency point of the side of your polygon. In the mode First tangency point, the tangency constraint is not kept.

Modifications / Additional information: The polygon constraints depend on the construction mode chosen: Construction mode Internal diameter

Constraints Equality constraints between the sides. Fixity constraint on the center. Dimensional constraint on the inscribed circle. Tangency constraints with

the inscribed circle. Coincidence constraints with the confined circle. Dimensional constraint of orientation. External diameter

Internal radius, External radius, Internal free size, External free size

Side + center length

Equality constraints between the sides. Fixity constraint on the center. Dimensional constraint on the inscribed circle. Coincidence constraints with the confined circle. Dimensional constraint of orientation. Same as Internal diameter and External diameter, only the constraint on the circles is a radius constraint and not a diameter constraint. Equality constraints between the sides. Fixity constraint on the center.

Coincidence constraints with the confined circle. Dimensional constraint of orientation. Dimensional constraint of the length of a side Side length 2 points

Equality constraints between the sides. Fixity constraint on the 2 points determining the length of a side. Coincidence constraints with the confined circle. Possibly, alignment constraints when the 2 points determining the length of a side are aligned horizontally or vertically

Standard profile Links / Videos:

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This command can quickly create sketches from remarkable shapes (oblong, keyhole, etc.).

Creation Stages / Use: Click the icon or select the 2D sketch > Other curves > Standard profile... command from the drop-down menu. In a Draft document, select the Sketch > Other curves > Standard profile... command from the drop-down menu. 1. Select the type of profile to include. 2. Choose the profile's insertion point. 3. Enter the coordinates of the profile's insertion point.

This command automatically generates segments. When the profile was included, there was no link between the sketch and the template document from the standard profile.

Available Options: Code: The standard profile can comes from a family. Select the wanted code.

Drivers: The driver section lets you specify the parameter values for the standard profile being included.

Modifications / Additional information: Creating a standard profile is similar to creating a component. To do this, create a 2D modeling document containing your sketch. It will provide the Standard Profile function from the TopSolid Library. The points published in your 2D modeling document will be offered as profile insertion points. You can also create a family document containing the drivers for your profile and perhaps a catalog.

Symbol Links/Videos:

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This command allows to position and fix the orientation of a symbol.

Creation stages / Use:

1. Click the icon or select the 2D sketch > Other curves > Symbol... command from the drop-down menu of a Part document or select the Sketch > Other curves > Symbol... command from the drop-down menu of a 2D Model or a Draft document. 2. Select an existing symbol. To create your own symbols, follow this link. 3. Select a key point. 4. Check Fix orientation to avoid the symbol to be oriented after its positioning. 5. Check the Profiles option to be able to use this symbol as a sketch. (Extrude, pocket, boss, ...). This option is only available in a sketch of a part. 6. Position and validate the symbol.

Specific options for drafts. The Profiles option is not proposed.

Arc

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A circle arc is created either by entering the coordinates in the dialog panel, or directly from the graphics zone by locating a point or selecting an element.

Creation Stages: Click the icon or select the 2D sketch > Other curves > Arc... command from the drop-down menu. In a Draft document, select the Sketch > Other curves > Arc... command from the drop-down menu. Creation by Center and 2 passing points: 1. In the Size topic, select Free size mode. 2. Check Given center. 3. Enter coordinates of the center point and of 2 passing points of the arc.

Creation by 3 passing points: 1. In the Size topic, select Free size mode. 2. Uncheck the box Given center. 3. Enter coordinates of passing points of the arc.

Creation by Center and Diameter or Radius: 1. 2. 3. 4.

In the Size topic, enter the Diameter or radius mode. Enter the arc diameter or radius value. Check Given center. Enter coordinates of the arc center point.

Creation by Diameter or Radius and 2 passing points: 1. 2. 3. 4.

In the Size topic, enter the Diameter or radius mode. Enter the arc diameter or radius value. Uncheck the box Given center. Enter coordinates of 2 passing points of the arc.

No matter which creation mode is chosen, the circle arc is created with its center point and its extremity points.

Available Options: The arc is created between selected points. By checking the Complementary option, it is the complementary arc (to close the circle) which is created. For example, if the arc angle is 60° its complementary is 300°.

Additional Information / Modifications: Displacement of an end: Click the end of a circle arc and move your mouse while holding down the left button to modify the opening angle of the circle arc. Displacement of the circle arc: Click the circle arc or its center point and move your mouse while holding down the left button to modify the position of the circle. From the popup menu you can: Constrain the center of the circle arc on an element with the Define center... command. When the center point no longer exists, recreate it with the command Create center. Create the complementary arc with the command Complementary. When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the element is created.

Ellipse Links / Videos:

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An ellipse is created either by entering the coordinates in the dialog panel, or directly from the graphics zone by locating a point or by selecting an element.

Creation Stages / Use: Click the icon or select the 2D sketch > Other curves > Ellipse... command from the drop-down menu. In a Draft or a Drawing document, select the Sketch > Other curves > Ellipse... command from the drop-down menu. Creation by the center and passing points: Allows to enter the center point and 2 passing points, one for the first diameter, the second for the other. 1. In the Size topic, select Free size mode. 2. Check Given center. 3. Enter the coordinates from the center point and 2 passing points. Creation by center and foci: Allows to enter the center point, 2 foci and a passing point to give the width. 1. In the Size topic, select Free size mode. 2. Check Given foci. 3. Enter the coordinates from the center point, 2 foci and passing points. Creation by center and diameters or radii: Allows to enter 2 diameters (or radii) and the center point. 1. In the Size topic, select Diameter or radius mode. 2. Enter the values of both diameters of the ellipse. 3. Enter the coordinates from the center point and 2 passing points.

Cardinal points display automatically when the ellipse is created and therefore become easier to constrain.

Ellipse and its 4 cardinal points.

Available Options: Align: This option allows an ellipse to be created whose foci are aligned horizontally.

Additional Information / Modifications: It is not possible to make a parallel of an ellipse, an ellipse arc, or a spline in a sketch. Yo

Ellipse Arc Links / Videos:

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An ellipse arc is created by entering the coordinates in the dialog panel, either directly from the graphics zone by locating a point or by selecting an element.

Creation Stages / Use: Click the icon or select the 2D sketch > Other curves > Ellipse arc... command from the drop-down menu. In a Draft or a Drawing document, select the Sketch > Other curves > Ellipse arc... command from the drop-down menu. Creation by the center and passing points: Allows to enter the center point and 2 passing points, one for the first diameter, the second for the other. In the Size topic, select Free size mode. Check Given center. Enter the center point coordinates and 2 passing points. Indicate both ends of your ellipse arc. Creation by center and Foci: Allows to enter the center point, 2 foci and a passing point to give the width. 1. In the Size topic, select Free size mode. 2. Check the Given foci option. 3. Enter the center point coordinates, 2 foci and passing points coordinates. 4. Indicate both ends of your ellipse arc.

Creation by center and diameters or radii: Allows to enter 2 diameters (or radii) and the center point. 1. In the Size topic, select Diameter or radius mode. 2. Enter the values of both diameters of the ellipse. 3. Enter the center point coordinates and 2 passing points coordinates. 4. Indicate both ends of your ellipse arc. After the ellipse positioning (it is represents with fine line), select the first extremity point and move your cursor on the ellipse to gibe the direction and the select the second point.

Available Options: Align: This option allows an ellipse to be created whose foci are aligned horizontally.

Additional Information / Modifications: It is not possible to make a parallel of an ellipse, an ellipse arc, or a

Spline Links / Videos:

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A Spline curve is created by indicated the points of the curve.

Creation Stages / Use: Click on the icon or select the 2D sketch or 3D sketch > Other curves > Spline... command from the drop-down menu. In a Draft o a Drawing document, select the Sketch > Other curves > Spline... command from the drop-down menu. 1. Select the type of spline between Passing points, Control points, Blend or Aspline : Passing points: The entering points are whose where the spline passes. Control points: The curve is constrained by the entered points.

Passing points

Control points

Blend: allows to create an tangent curve to two others. By default, the tangents length is equal to 1/3 of the distance between the vertices of the 2 curves. This constraint can be modified with 2 constraints. Aspline: The Aspline is composed of lines, by arcs or ellipses passing by entering points. It is possible to change the Aspline during its creation. For example you can begin with the line mode, and continue with the arc mode. 2. Position and/or enter coordinates of the spline points or for the blend, select the 2 entities to blend. 3. Validate with .

The ASpline is a specific Spline. It consists of lines, arcs or ellipses depending on the selected type. This type of spline allows moving a point along the curve and passing the various peaks. It has an actual advantage, such as, for example, for designing a parameterized staircase where it is necessary to move the boundary points of a step along a sketch.

Options available for the Spline with clearance points: Mode: (Usefull for the modification) Origin Spline :

Free

Balanced tangents

.

A free spline will be more malleable, it will be possible to move each interpolation points or tangents without change the geometry of the other points or tangents.

A spline with balanced tangents allow to modify easier a spline. The result will be more harmonious.

A tense spline or its interpolat

If we want to make a modification, we recommend to use the Balanced tangents mode.

Closed: Check Closed to create a closed spline curve.

Zero curvature: When this option is checked, it causes a null curvature at the two ends of the spline. These constraints, symbolized by a black circle, can be separately enabled/disabled by a popup menu option near one one of the curve.

Options available for the Spline with control points: Closed: Check Closed to create a closed spline curve.

Zero curvature: When this option is checked, it causes a zero curvature at the two ends of the spline. These constraints, symbolized by a black circle, can be separately enabled/disabled by a popup menu option near one of the curve.

Options available for the Blend: Tense: A tense spline will be less malleable when it or its interpolation points are moved. There is a popup menu option on a non-tense curve for making it tense. This can cause a change to the geometry of the curve in order to create a more constant curvature.

Zero curvature: When this option is checked, it causes a null curvature at the two ends of the spline. These constraints, symbolized by a black circle, can be separately enabled/disabled by a popup menu option near one of the curve.

Options available for the ASpline: Closed: Check Closed to create a closed spline curve.

Additional Information / Modifications: Tangents: Tangents at points of interpolation can be constraints.

To define tangency: Handles (yellow spheres) at the ends of the curve allow tangencies to be defined through the popup menu when creating the curve. After activating the command, select the start or end tangent (line, axis, etc.). When the spline is validated, constraints between the tangent and referent element will automatically be created.

Show curvature: A popup menu option on a spline makes it possible to view its curvature. The circle symbolizes the area with the greatest curvature.

Curvature circle: A popup menu option on a point of interpolation allows the curvature circle at the point to be displayed and constrained.

Global scaling: Global scaling is triggered when modifying a constraint between two points of interpolation on a largedimension spline. Displacement: By default, the dynamic movement on tangency constraints and interpolation points are local. But using the Alt key on the keyboard during movement triggers a global modification. (It may sometimes be necessary to authorize such a movement in order to achieve the desired result.)

It is not possible to make a parallel of an ellipse, an ellipse arc, or a spline in a sketch. You must use a parallel

Fillet Links / Videos:

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A fillet is created by entering its radius value and selecting the vertex of a sketch element.

Creation Stages: Click the icon or select the 2D sketch > Fillet... command from the drop-down menu. In a Draft document, select the Sketch > Fillet... command from the drop-down menu. 1. Select the type of fillet. Local: The fillet is applied on each selected vertex. Global: The fillet is applied on each vertex of the sketch. Internal external: Like for global mode, the fillet is applied on each vertex of the sketch, but with different values for internal and external radii.

Example of fillets on each vertex, on the left with the Global mode, on the right with the Internal External

2. Enter the fillet radius. In case of using Internal External mode, enter the internal and external radii. 3. Select a vertex of one element of the sketch. (With local mode) 4. Check Keep vertex to keep the selected point. Fillet with vertex kept

Fillet with vertex not kept

5. With Global and Internal External modes, it is possible to modify the angular tolerance. It is the minimum angle from which the fillet will be created. Under this value, there will be no fillet on this vertex. 6. Validate by clicking .

Additional Information / Modifications: A fillet is considered as a circle arc, from the popup menu you can: Constrain the center of the circle arc on an element with the Define center... command. When the center point no longer exists, recreate the circle arc's center point with the command Create center.

The Internal external mode only works with a closed sketch.

Chamfer

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A chamfer is created by entering the parameters of the chamfer and selecting the vertex of a sketch element.

Creation Stages: Click the icon or select the 2D sketch > Chamfer... command from the drop-down menu. In a Draft document, select the Sketch > Chamfer... command from the drop-down menu. By default, the chamfer is created by indicating lengths, choose the mode Given angle to create an angle and a length. 1. Enter chamfer parameters. 2. Select a segment close to a vertex. Check Keep vertex to keep the selected point. Chamfer with vertex kept

Chamfer with vertex not kept

When the two lengths are different or when the angle differs by 45°, the first length is applied on the selected segment.

Additional Information / Modifications: Once created, a chamfer is considered as a line, the modifications are therefore identical to those of the command Line.

Trim Links / Videos:

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This command allows one or more segments to be cut at the intersection of one or more other segments .

Use: Click the icon or select the 2D sketch > Trim... command from the drop-down menu. In a Draft document, select the Sketch > Trim... command from the drop-down menu. 1. Choose the type of geometry to be modified: Segment Profile

Only the selected segment will be modified. All the sketch elements joined to the selected segment will be modified.

2. Choose the limitation mode: Keep Delete Split

The part of the segment selected is kept, this part is temporarily drawn in a thick full orange line. The part of the segment deleted, this part is temporarily drawn in a thick orange and green dotted line. The segment is split at the intersection point with the intersecting segment.

3. Select the element to be limited.

It is not possible to use the sketch's X and Y axes to limit an element. This command does not allow a sketch segment to be extended.

Available Options: Geometries to be ignored: You can limit this command's field of action by checking options Construction segments and/or Internal segments, in this case the segments of construction and/or internal type are not taken into account in the limitation calculation. The Isolated vertices option allows not taking into account the points which are on the geometry to be limited and which are not connected to any other geometry.

Segments removing Links / Videos:

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This command allows to remove segments in a sketch. This command is more advanced than the Delete command ( DEL key). If segments have to be removed in a sketch operation, use the Segments removing of sketch operations.

Creation Stages / Use: Click the icon or select the 2D sketch > Other modifications > Segments removing... command from the drop-down menu. 1. Select the segments to be deleted. 2. Select a type of heal based on the options defined below. 3. Validate.

Available heal types:

The red crosses denote segments to be deleted.

Heal type: None The segments are deleted.

Heal type: Join The segments are deleted and replaced by a segment that connects the two end points.

Heal type: Extend/Limit The segments are deleted, and the remaining segments are extended.

Additional options for heal with Extend/Limit type: These additional options are effective only for extending circular segments. By tangency: Deleted segments are replaced by lines that run tangent to the circular segments having a common point with the deleted segments. (the segment to delete in blue and the preview of the result in orange).

By Curvature: Deleted segments are replaced by the extended circular segments that had a common point with the deleted segments. (the segment to delete in blue and the preview of the result in orange).

Parallel Links / Videos:

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The command Parallel allows a contour to be created parallel to another sketch element.

Creation Stages / Use: Click the icon or select the 2D sketch > Other modifications > Offset... command from the drop-down menu. In a Draft document, select the Sketch > Other modifications > Offset... command from the drop-down menu. 1. Select a sketch element: 2. By checking the Construction option, the selected profile will become a construction profile and will be internal. The offset will not be a construction profile. 3. Select a mode: One side: The parallel is on the side indicated by the arrow. Both sides: The parallel is on both side of the selected element. 2 different offset can be entered. Centered: The parallel is on both side of the selected element and centered. The entered value corresponds to the distance between the selected element and one of the two parallels.

3. Indicate the distance value(s). The Reverse option allows the dimension of the parallel to be changed, this action can also be carried out by double-clicking on the end of the arrow. It is not possible to create the parallel from a construction element or from an element inside the sketch. If the profile is opened, you can also use the Thickened command.

Modifications / Additional information: TopSolid displays an arrow with a label allowing the distance and the direction of the parallel to be modified dynamically: Dynamic modification of the distance Reversal of direction Modification of distance

Click the end of the arrow and move your mouse while holding down the button. Double-click the end of the arrow. Double-click the label displaying the distance and enter the distance value.

When the mode Automatic relations is enabled, the parallelism constraints between the reference profile and the parallel profile are automatically created.

When the mode Automatic dimensions is enabled, a dimensional constraint (driving dimension) between the reference profile and the parallel profile is automatically created.

It is not possible to make a parallel of an ellipse, an ellipse arc, or a spline in a sketch. You must use a p

Thickened Links/Videos:

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This command allows to thicken an open profile, with a centered, a one side or both sides mode. Extremities joints can also be managed.

Creation stages / Use: Click the icon or select the 2D sketch > Other modifications > Thickened... command from the drop-down menu. In a Draft document, select the Sketch > Other modifications > Thickened... command from the drop-down menu. 1. Select the profile to thicken. 2. The selected profile will be converted to a construction profile, by checking the Construction option. 3. Select the type of offset. The thickness is distributed on both sides of the reference profile. Enter the total thickness. The thickness is on one side of the reference profile. Enter the total thickness. Select the side by clicking the yellow arrow in the workspace area. The thickness is on both sides of the reference profile. Enter the thickness for the first side. Enter the thickness for the second side. Select the side by clicking the yellow arrow in the workspace area. The double arrow indicates the second side.

4. Select the extremity joint: External arcs: The center of extremity arcs is coincident with the extremity of the reference profile.

Internal arcs: The arc is coincident with the extremity of the reference profile.

Lines: Lines are perpendicular to the reference profile and coincident with the extremity of the reference profile.

5. Validate by clicking

.

If the profile is closed, use the Parallel command.

Example of creation of a thickened profile. (In blue: reference profile, in orange : the thickened profile with centered mode).

Modifications / Additional information: The result of this thickened profile is a contour. It is not possible to modify this result after validation. You have to edit the sketch and delete entities. If the thickened profile has to be associative and so modifiable by editing, you have to use the Thickened command.

Translated

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This command translates profiles from a sketch.

Creation Stages / Use: Select the 2D sketch > Other modifications > Translated... command from the drop-down menu. In a Draft document, select the Sketch > Other modifications > Translated... command from the drop-down menu. 1. Select the profile to be translated. 2. Select the translation direction. 3. Enter the translation value. 4. Validate creation of the projected elements with the button.

Translated elements are constraints with respect to the reference elements. A translation constraint with the symbol will be applied to each reference element and to each translated element. Changing the dimensions of a reference element will cause a change to the translated element.

It is not possible to translate a single segment when it is sewn together with other segments. It is not possible, for example, to translate a segment of a rectangular profile.

Modifications / Additional information: You can change the translation value by editing the sketch and double-clicking on the dimension.

Symmetric

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This command allows to symmetrize sketch entities.

Creation stages / Use: Click the icon or select the 2D Sketch > Other modifications > Symmetric... command from the drop-down menu. 1. 2. 3. 4.

Select profiles of the sketch to symmetrize. Select the type of symmetry: Single or Double. Select the axis or axes of symmetry. Validate with .

It is possible to symmetrize sketch entities dynamically during their creation. To do this, you have to activate the Dynamic symmetry mode. Created entities by the symmetry are displayed with small arrows in direction of the symmetry axis. By clicking one of these arrows, the 2 symmetrical entities are highlighted.

Only some simple entities (line, circle, arc, rectangle, ellipse, spline, ...) are taken in account during the symmetry. Some type of entities are not managed and cannot be selected (symbols, texts, hatches, ...).

Project

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This command allows the edges to be projected in the current sketch plane or in a draft view into its detailing.

Creation Stages / Use: Select the 2D sketch > Other modifications > Project... command from the drop-down menu. For a Drafting document, select the Sketch > Project... command from the drop-down menu. 1. Select the element type to project. 2. Select the elements to project. 3. Validate creation of the projected elements with the

button.

The elements are projected in the plane of the sketch and coincidence constraints are created between the selected elements and the projected elements.

In a Drafting document, the curves/edges mode is available only

Available Options:

Curves or edges: Allows you to project curves/edges/segments.

Profiles or loops: Allows you to project profiles/loops or boundary of a face.

Circles by diameter: Allows you to project only drillings circles or arcs. You just have to make a selection box to select them. All: All drillings parallel to the projection plane are projected. Diameter: Allows to select drillings diameters to project. If the drilling hasn't the entered diameter, it will not be projected. Tolerance: Allows to define the search tolerance. A 0.1mm tolerance allows to find all drills with a entered diameter +/0.05mm. Arc minimum: When a drilling is near the part border, it is not complete. the minimum arc allows to select only drilling with at least this angle.

Path between two edges: Allows you to project a path between tangent edges by selecting the first and the latest edges. Start edge: Select the first edge. The arrow indicates the direction of the path. Click Invert if needed. End edge: Select the latest edge. Border: This mode can only be used with edges of a face. It allows to select all edges of the face. They can be tangent or not. Angle: If the angle between 2 following edges is smaller or equal to the entered angle, the edge is selected.

Paths around faces:

Allows you to project the contours of the selected faces. The profiles are created as long as you select the faces: - If you select 2 neighbouring faces, the external profile on the 2 faces will be created only. - If you select 2 separate faces, two profiles will be created.

Modifications / Additional Information: This command is limited to the projection of lines, circle arcs, and plane faces, it is not possible to project ellipses, curves and non plane faces.

Intersection

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The Intersection command allows you to create the intersection curve between one (or several) face(s) of a shape and the sketch plane.

Creation stages / Use: Click the icon or select the 2D Sketch > Other Modifications > Intersection... command from the drop-down menu. 1. Select the sketch's support plane. 2. Select the intersection type. creates all intersection curves between a shape and the sketch plane. creates intersection curves between several faces and the sketch plane.

3. Select the shape or faces, depending on the option chosen above. 4. Validate the creation of the intersection curve with the button.

Only the shapes or faces that cross the sketch plane can obtain an intersection curve. An intersection constraint is created between each selected faces and the sketch plane. In some case like cylindrical faces for example, a rotative picking allows to select the cylindrical face (then the result of the intersection will be a circle or an ellipse), or the cylinder axis (then the result will be a point).

Examples:

Example of intersection between faces (in cyan color) and the sketch plane (in blue).

Example of intersection between the axis of a cylindrical face and the sketch plane, the intersection point is displayed in red in the center of the picture.

Modifications / Additional information: The intersection constraints created by this command can be edited, then you will be able to choose new geometries.

Profile Links/Videos:

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If a sketch is created with the sewing manual mode (option available in 2D or 3D sketch > Options...), this command allows to transform a batch of segments to profile. This can be used in an extrusion, trim, etc.

Creation stages / Use: Click the icon or select the 2D sketch > Profile... from the dropdown menu. In a Draft document, select the Sketch > Profile... from the drop-down menu. 1. Select the different segments. 2. Validate by clicking .

Selected segments are highlighted.

If the command is grayed, the sewing mode is set to automatic (option is available in 2D or 3D sketch > Options...).

Section This command allows you to create a section between different profiles. This section can be used in the Extrusion command to extrude the profiles included in the section without taking into account other possible sketch profiles.

Creation stages / Use: Click the icon or select the 2D sketch > Section... command from the drop-down menu. In a Draft or a Drawing document, select the Sketch > Section... command from the drop-down menu. 1. Select the different profiles. 2. Select the hatch type. 3. Select the spacing of the hatches, as well as the orientation and the offset according to X and Y.

The hatch type has no effect on using the sketch.

Available options: Style : By activating this option, you can select an haching style that has been previously defined in order to apply it on this section. The bouton

Offset:

allows to create a new style on the fly.

This option allows to apply an offset in X and/or Y in order to adjust the hatching position.

Standard hatching: When the Custom hatching option is not active,you can select an hatching type from those available in the drop down list. With this pattern options below are available: Spacing: allows to modify spacing between each line of the pattern. Orientation: allows to apply a rotation to the pattern. The rotation axis is the Z axis of the frame view or of the sketch in which the section has been created.

Custom hatching: Using this option, you can select the custom hatching pattern. With this pattern options below are available: Document: select the custom hatching template to use. Fiber type: the custom hatching template allows to define several pattern for one hatching. Select here the type to use. Scale type: allows to define the scale type to use. Automatic: sizing uses the Scaling type define in the custom hatching template. Absolute: enter the scale factor to apply to the hatching pattern.

Modifications / Additional information: You can change the sketch or section using the corresponding popup command.

Text

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The Text command allows you to insert text into a sketch. You can insert a text with methods below: Text created on insertion or selection of an existing text parameter in the drop-down list. Create a new Text parameter Convert a Document parameter to text Convert the setting of a set into text.

Creation Stages: Click the icon or select the 2D sketch > Text... command from the dropdown menu. 1. Enter the text or specify a type of parameter to use. An expression can also be entered. 2. Check Profiles or leave it unchecked. If this option is checked, the text becomes a profile (to be able to extrude it or to make a pocket).If it is not checked, the text remains internal to the sketch. 3. Enter the text angle. The angle by default is 0° (horizontal text). By changing the angle, the text turns with the entered value. 4. Position text 5. Validate the creation of text.

A text parameter that already exists in the document can be accessed directly from the drop-down menu of the text creation command. In order to reduce the document, you will not find it in the "Document parameter" list.

Available Options: Text style: Select the text style to use here: normal text style (default style) or customized text style.

Format:

Allows to change text settings (Justification, font, frame, color and others ...

Justification: To use a justification other than that offered by default, select the cell Ju Three justifications are available:

Left

Centered

Right

In a sketch of a part document, the justification is only useful for mu you have to create a text parameter and check the multi-lines option

Font: Displays the name and size of the font used

Displays the name and size of the font used. Check the Font option to activate the button and be able to modify settings (

Framing: Lines: Allows to define lines thicknesses of the text. Symbol line allows to change the text thickness. Leader lines allows to change the leader thickness.

You can constraint the text position by using following contextual commands:Annotation alignment and Annotation centering.

Modifications: To modify an existing text, just select it with the right button and select the Edit command.

Text on curve Links/Videos:

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This command allows to create a text on a reference curve.

Creation stages / Use: You can insert a text with methods below: Text created on insertion or selection of an existing text parameter in the drop-down list. Create a new Text parameter Convert a Document parameter to text Convert the setting of a set into text. Click the icon or select the 2D sketch > Text on curve... command from the drop-down menu. 1. 2. 3. 4. 5.

Enter the text or specify a type of parameter to use. Select the curve. Check Reverse to invert the text around the curve. Enter the offset between the text and the curve. Check Profiles or leave it unchecked. If this option is checked, the text becomes a profile (to be able to extrude it or to make a pocket).If it is not checked, the text remains internal to the sketch. 6. Position text 7. Validate the creation of text.

A text parameter that already exists in the document can be accessed directly from the drop-down menu of the text creation command. In order to reduce the document, you will not find it in the "Document parameter" list.

Available Options:

Text style: Select the text style to use here: normal text style (default style) or customized text style.

Format:

Allows to change text settings (Justification, font, frame, color and others ...

Justification: To use a justification other than that offered by default, select the cell Ju Three justifications are available:

Left

Centered

Right

In a sketch of a part document, the justification is only useful for mu you have to create a text parameter and check the multi-lines option

Font: Displays the name and size of the font used. Check the Font option to activate the button and be able to modify settings (

C ec t e o t opt o to act vate t e butto a d be ab e to

od y sett gs (

Framing:

Modifications: To modify an existing text, just select it with a right button and select the Edit command.

Wire text Links/Videos:

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This command allows to write a text the a wire font. It can be used for engraving.

Creation stages / Use: You can insert a text with methods below: Text created on insertion or selection of an existing text parameter in the drop-down list. Create a new Text parameter Convert a Document parameter to text Convert the setting of a set into text. Click the icon or select the 2D sketch > Wire text... command from the drop-down menu. 1. Enter the text or specify a type of parameter to use. An expression can also be entered. 2. Select a font in the drop-down list. This font must exist before using it. 3. Position the text 4. Validate by clicking .

The character must exist in the selected font otherwise it will be replaced by a rectangle.

Available options: Spacing: This option allows you to manage the distance between each letter of the text. The spacing value must be between 0 and 10, it corresponds to a percentage of the text height. Angle: This option allows you to rotate the text according to the horizontal direction. A wire text with an orientation angle cannot be transformed into a wire text on curve. Mirror: This option allows you to reflect the text. Profiles: When this option is checked, the text becomes a profile (it can be used for an extruded shape or a pocket). When it is not checked, the text remains internal to the sketch. Drivers (size): This option allows you to define the height of the wire text.

Modifications / Additional information: The wire text can be edited by using the contextual menu. It can also follow a curve by using the Text on curve contextual command.

Font creation for a wire text: The wire text needs a specific font. A wire font is supplied by TopSolid. Follow this link Creation of a font for wire text to learn how to create yours.

Deformation Links / Videos:

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This command allows a segment to be transformed into a circle arc.

Creation Stages / Use: Click the icon or select the 2D sketch > Deformation... from the drop-down menu. In a Draft document, select the Sketch > deformation... from the drop-down menu. This command does not have a dialog panel, select the line to be transformed into a circle and move the cursor keeping the left mouse button pressed down then release the button when the desired circle arc is obtained.

This command does not allow the reverse transformation to be made (transformation of an arc into a line). Depending on the constraints applied on the segment, deformation is not always possible, for example, it is not possible to deform a segment with an alignment constraint.

Constrain Automatically Links / Videos:

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This command allows you to automatically constrain a basic unconstrained sketch from an import.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Constrain Automatically... command from the drop-down menu. In a Draft document select the Sketch > Constraints > Constrain Automatically... command from the drop-down menu. 1. Select the different types of constraints to create. 2. Enter values for the linear and angular tolerances. 3. Validate the creation of constraints with the button.

To constrain a sketch from an import (Dxf, Dwg, Iges, etc.), you must copy the imported elements and then paste them into a new sketch.

Available Options: The linear tolerance will be used for concentricity constraints, while the angular tolerance will be used for orientation, tangency, and perpendicularity constraints.

Regarding the imported element quality, you will perhaps have to change tolerances. It will for example allows to consider that 2 circles have a concentricity if the distance between their center point are smaller than the entered tolerance, or to consider a segment as horizontal if its tilt is lower than the angular tolerance. The Diameter option allows a diameter dimension to be created for all circles in the sketch, while the Radius option is for the dimensions of the circle arcs.

Modifications / Additional information: The result of this command is identical to the result from the Constraint command. There is no specific option in the operations tree.

Constraint creation

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The Constraint... command allows dimensional constraints (driving dimensions) to be created or relations between the document elements.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Constraint... command from the drop-down menu. In a Draft document select the Sketch > Constraints > Constraint... command from the drop-down menu.

1. Select the first geometry. If you position the dimension, you obtain a length dimension (for a linear segment), the radius for an arc, the diameter for a circle, coordinates dimensions for a point. 2. If you select a second entity, you obtain the distance, the angle, .... 3. Position the dimension. A relation is created by selecting one or more sketch elements, then selecting from the proposed constraints in the popup menu that displays by right-clicking.

To create a dimension centered on an axis, before putting in your dimension, choose the command

Centered dimension from the popup menu that displays by right-clicking, then select an axis.

Modifications / Additional information: The modification of the value of a dimension is carried out by doubleclicking on the dimension text when no command is launched (neutral mode) or when the commands Constraint or Revolution dimension are launched. The type of extremity of a dimension depends on the selected element: the selection of an extremity of an element creates a dimension with a point type extremity and the selecting of an element creates a dimension with an arrow type extremity. As the dimensions and constraints are created, TopSolid changes the color of the sketch elements in order to indicate whether they are fully constrained. An under constrained element is displayed in magenta, a completely constrained element is displayed in blue. The same is true for the dimensions. When an over-constrained dimension is detected, TopSolid automatically disables the dimension being created and displays it in gray. The commands Enable and Disable in the popup menu of a dimension allow the types of dimensions to be modified. In case of over-constraint, the dimensions or relations in question are displayed in red. The Ask the dimension value mode allows to modify the value just after positioning it.

Revolution dimension Links / Videos:

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The command revolved shape dimension allows a sketch of a revolved shape to be dimensioned rapidly in relation to the X axis.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Revolution dimension... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Revolution dimension... command from the drop-down menu.

1. Select an element in the sketch (point, line, circle, ...). 2. Check Radius dimension to display it as a radius. If this option is unchecked, the dimension will be a diameter and will have the double of the measured value between the selected element and the reference axis. 3. Position the dimension.

By default, the reference axis is the X axis of the sketch, it is possible to modify it with the command Define revolution axis. This command does not allow Bspline curves to be dimensioned.

Modifications / Additional information: The modification of the value of a dimension is made by doubleclicking on the dimension text when no command is launched

(neutral mode) or when the command Constraint is launched. As the dimensions and constraints are created, TopSolid changes the color of the sketch elements in order to indicate whether they are fully constrained. An under constrained element is displayed in magenta, a completely constrained element is displayed in blue. It is the same for dimensions, when an over-constrained dimension is detected, TopSolid automatically disables the dimension being created and displays it in gray. The commands Enable and Disable in the popup menu of a dimension allow the types of dimensions to be modified. In case of over-constraint,, the dimensions or relations in question are displayed in red. Ask dimension value mode allows to modify the dimension value just after positioning it.

Length dimension Links / Videos:

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This command allows to dimension the length of a profile (line, arc, spline, circle, ...).

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Length dimension... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Length dimension... command from the drop-down menu. 1. Select the profile. 2. Position the dimension.

The length of the profile is one side. It accounts for the dimension style (number of decimals, unit). A length dimension is displayed with a ~ (tilde) symbol before its value.

Overview of relations

The relations of the geometric constraints that can be applied to sketch elements, in addition to dimensional constraints, will allow you to quickly obtain the shape you wish to model. The table below lists the characteristics of each relation: Name

Icon Symbol

Reference element

Resu

Perpendicularity

A line and a circle or a circle arc.

The angle between the two elements i

Concentricity

Two circles or two circle arcs.

The centers of the elements become c

Tangency

A line and a circle or a circle arc.

The two elements are tangent.

Orientation

One line.

The line is pivoted to the closest horizo

Alignment

Two points.

The two points are moved to the close

Coincidence

Two points. A point and a line, an arc, a circle or an edge. Two lines. Two elements (points or lines) and a line (axis). Two lines.

The points are superposed. The point is placed on the element or The lines are placed collinearly.

The point is moved at the intersection

Equality

A point and two elements (lines, circles or circle arcs). Two lines.

Fixity

Any type of element.

Translated

Any type of element, except points.

The element's position cannot be mod In the case of a line or an arc, the end the arc. Elements are constrained dimensiona This constraint is automatically added

Centering Parallelism Intersection

The two elements are moved equidista The two lines are oriented in the same

The length of the two lines becomes e

Automatic Relations When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the Likewise, the choice of the sketch's origin during creation of an element automatically creates a fixity relation. It is also possible to quickly create a tangency constraint between a line and an arc by selecting the line or the arc near the tangency point, then by moving it until the tangency symbol display is obtained. The relations display can be activated or not by changing the Show relations mode.

Perpendicularity relation Links / Videos:

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This relation allows an element to be positioned perpendicularly to another.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Perpendicularity... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Perpendicularity... command from the drop-down menu.

1. Select the two elements to be made perpendicular: the two elements are moved and the Perpendicularity symbol is displayed between the two elements. 2. In some cases, it is also needed to select a perpendicularity point. For example to add a perpendicularity between two splines. In this case, the filed is automatically ungrayed. In the common case of a perpendicularity between 2 lines, it isn't needed and stays grayed.

To delete the Perpendicularity relation, you must select the Perpendicularity symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the

Concentricity relation Links / Videos:

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This relation allows the centers of two circles or circle arcs to be made to coincide.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Concentricity.... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Concentricity... command from the drop-down menu. Select the two elements to be made concentric then place the Concentricity symbol: the two elements are moved and the Concentricity symbol is displayed between the two elements.

To delete the Concentricity relation, you must select the Concentricity symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch

Tangency relation Links / Videos:

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This relation allows an element to be positioned in tangency on another.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Tangency... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Tangency... command from the drop-down menu.

1. Select the two elements to be made tangent: the two elements are moved and the Tangency symbol is displayed between the two elements. 2. In some cases, it is also needed to select a tangency point. For example to add a tangency between two splines. In this case, the filed is automatically ungrayed. In the common case of a tangency between a line and an arc, it isn't needed and stays grayed.

To delete the Tangency relation, you must select the Tangency symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information:

When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the You can quickly create a tangency constraint between a line and an arc by selecting the line or arc close to the tangency point then displacing it until the display of the tangency symbol is obtained.

Alignment Relation Links / Videos:

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This relation allows two points to be aligned horizontally or vertically.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Alignment... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Alignment... command from the drop-down menu. Select the two points to align: the two points are moved towards the closest horizontal or vertical and the Alignment symbol is displayed in the middle of the two points.

To delete the Alignment relation, you must select the Alignment symbol, then press the Del key on your keyboard or choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the

Coincidence relation Links / Videos:

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This relation allows an element to be positioned on another.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Coincidence.. command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Coincidence... command from the drop-down menu. Select the two elements to be made to coincide: the two elements are moved and the Coincidence symbol is displayed between the two elements. Elements selected Two points A point and a line, an arc, a circle or an edge. Two lines

Result The points are superposed. The point is placed on the element or in its extension. The lines are placed collinearly.

To delete the Coincidence relation, you must select the Coincidence symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When a coincidence constraint has been defined between a point and a segment, the Fix ratio contextual command allows you to define the location of point proportionally to the segment dimension. In this case, the circle used for the coincidence constraint is replaced by a double arrow as shown below:

In the example above, the ratios of the coincidence constraints have been fixed to 1/3 (at the bottom) and 2/3 (at the top) of the segment lengths.

Then, these ratios are kept during the modification of the rectang

The Unfix ratio contextual command allows you to delete the ratio constraint and get back to an simple coincidence constraint.

When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the element is created.

Centering relation Links / Videos:

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This command allows two elements to be centered in relation to an axis.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Centering.. command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Centering... command from the drop-down menu. Select the two elements to be centered, the centering axis then place the Centering symbol: the two elements are moved at equal distance in relation to the axis and the Centering symbol is displayed between the two elements.

Centering can only be carried out with lines and points.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a

Symmetry

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This command allows to add a symmetry relation between two elements in relation to an axis.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Symmetry.. command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Symmetry... command from the drop-down menu. Select the two elements to be symmetrized and the symmetry axis: the two elements are moved at equal distance in relation to the axis and the Symmetry symbol is displayed between the two elements.

The symmetry can only be used with the same type of geometries. The second selected geometry is modified by the symmetry. It must not be completely constraint.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a

Parallelism relation Links / Videos:

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This relation allows two lines to be made parallel.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Parallelism... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Parallelism... command from the drop-down menu. Select the two lines to make parallel and then place the Parallelism symbol: the two lines are moved and the Parallelism symbol is displayed between the two lines.

To delete the Parallelism relation, you must select its symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the

Intersection relation Links / Videos:

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This command allows to create an intersection relation between 2 points at the selected point.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Intersection... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Intersection... command from the drop-down menu. 1. Select 2 elements to intersect. 2. Select the intersection point. Both elements are displaced and the Intersection symbol is also displayed at this 2 elements intersection.

To delete the Intersection relation, you must select its symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional Information: The relations display can be activated or not by changing the Show relations mode.

Equality relation Links / Videos:

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This relation allows to make equal the length of several lines.. It also allows to create an equality relation between circles radii. Segments with the same length or radius are displayed with a small graphic symbol signed (=1, =2, =3,… ).

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Equality.... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Equality... command from the drop-down menu. 1. Select segments to make equal. 2. Validate the Equality relation with the

button.

Lengths of the lines are modified and an Equality symbol is displayed in the middle of each line.

Graphic symbols allows to rapidly identify equal segments.

To delete the Equality relation, you must select its symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the element is created.

Fixity relation Links / Videos:

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This relationship allows a sketch entity to be fixed.

Creation Stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Fixity... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Fixity... command from the drop-down menu. Select the sketch entity to be fixed. The entity will change to black and will no longer be able to move.

To delete the Fixity relation, you must select its symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking. It is also possible to use the Remove fixity popup command. In order to clarify the entities tree, fixity constraint symbols are not displayed in the sketch constraints folder.

Group Links/Videos:

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This command allows to group several sketch entities together.

Creation stages / Use: Click the icon or select the 2D sketch > Constraints > Relations > Group... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Relations > Group... command from the drop-down menu. 1. Select geometries and annotations to group. 2. Validate by clicking .

The displacement of one entity will displace all other entities of the group. To delete the Group relation, select its symbol, then press the Del button of your keyboard or select the Delete command from the contextual menu.

Variable

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This command allows a variable of type Angle or Length to be defined in order to be able to create proportionality relations between the dimensions (like for example such a dimension must be equal to twice another, the dimension value being unknown).

Creation Stages / Use: Select the 2D or 3D sketch > Constraints > Variable... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Variable... command from the drop-down menu. 1. Choose the variable's type (Angle or Length). 2. Enter the variable's name.

Modifications / Additional information: When the variable is created, you can associate it with a dimension by selecting the dimension, and using the popup command Make variable. The variable name will then be displayed between the characters < > after the dimension text and this dimension will no longer drive the geometry, its value will be recalculated during the modification of the geometry (via modification of the sketch or via displacement of elements referenced by the dimension).

You can then use the command Equations to create equations between the variables (like for example: b = 2 * a). The equations are specific to each sketch, you can view them by unbending the sketch in the Sketches folder of the entities tree.

There is no chronology in the resolution of an equation, only the relation is important. Take for example the case of a variable "a" associated with a dimension which has the value of 60mm and a variable "b" whose equation is: b = 2*a. When the variable "b" is associated with a dimension whose value is 100mm, TopSolid can either modify the value of the 100 mm dimension and make it go to 120mm, or modify the value of the 60mm dimension and make it go to 200mm.

The variables are specific to each sketch, it is not possible to share them between several sketches or use them outside the sketch.

Equations

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This command allows equations to be defined between the different variables of a sketch.

Creation Stages / Use: Select the 2D or 3D sketch > Constraints > Equations... command from the drop-down menu. In a Draft document, select the Sketch > Constraints > Equations... command from the drop-down menu. 1. 2. 3. 4.

Enter your equation using different available operators. Validate your equation with the Enter or Tabulation key. Possibly repeat steps 1 & 2 to define the next equations. Validate your equations with the button.

"+" and "-" operators can be used between two variables. Ex: a+b or a+10 "*" and "/" operators cannot be used between two variables. Ex: a*2 et a/2 but a*b and a/b Functions cannot be used with variables E.g.: Log(10) but log(a)

Modifications / Additional information:

The equations are specific to each sketch, you can view them by unbending the sketch in the Sketches folder of the entities tree.

Overview of sketch operations

The sketch operations are going to allow you to create complex geometry (parallel, curve by formula, repetition, ...) from the elements of a sketch. The element thus created is an operation, its updating is carried out after solving the sketch.

Sketch operation repetition: To repeat a sketch operation you have to: Edit your sketch using the popup menu on a sketch element. Although sketch operations are hidden during sketch edition, use the 2D sketch > Operations > Repetition command. The sketch operations then become visible and you can select them when defining your repetition.

Point Links / Videos:

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This command allows an offset point to be created from a vertex of the sketch.

Creation Stages / Use: Select the 2D sketch > Operations > Point... command from the drop-down menu. 1. Select the reference point. 2. Enter the offset values in X and in Y.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch elemen The Tolerance contextual command allows to modify this approximation.

Line

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This command allows you to create a line from two points (vertices) of the sketch. It will be in particular used to complete (close) the elements created by sketch operations so as for example to obtain a closed contour allowing a solid to be built during an extrusion.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Arc or Circle Links/Videos:

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This command allows you to create an arc or circle from two or 3 points (peaks) of the sketch. It will be in particular used to complete (close) the elements created by sketch operations so as for example to obtain a closed contour allowing a solid to be built during an extrusion.

Creation stages / Use: Select the 2D sketch > Operations > Arc or circle... command from the drop-down menu, then select starting and ending points of the arc or the circle. 1. 2. 3. 4.

Check the Arc box to create an arc, otherwise a circle will be created. Enter its description. Select the type. (see below for more information) Validate by clicking Creation by center and clearance points: 1. In the Size topic, select Free size mode. 2. Check Given senter. 3. Select the center point and the clearance point(s) of the circle or arc.

Creation by 3 passing points: 1. In the Size topic, select Free size mode. 2. Uncheck the box Given center. 3. Select the 3 clearance points of the circle or arc.

Creation by Center and Diameter or Radius: 1. 2. 3. 4.

In the Size topic, select the Diameter or Radius mode. Enter the diameter or radius. Check Given center. Select the center point of the circle or the arc and for an arc, the 2 clearance points.

Creation by Diameter or Radius and 2 passing points: 1. 2. 3. 4.

In the Size topic, select the Diameter or Radius mode. Enter the diameter or radius. Uncheck the box Given center. Select the 2 clearance points of the circle or arc.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Circle involute

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This command can be used to create a tooth flank to model gears and pinions

Creation stages / Use: Select the 2D sketch > Operations > Circle involute... command from the drop-down menu. 1. Enter the base diameter value (primitive diameter multiplied by the cosinus of the pressure angle) . 2. Enter the start diameter value (root diameter). 3. Enter the end diameter value (outside diameter). 4. Specify the center point for these circles. 5. Specify the passing point (point on the base circle).

Example of a circle involute regarding the base diameter (in black), the start diameter (in blue) and the end diameter (in red).

To create the complete pinion from the circle involute: From the pop-up menu of the sketch, select Building sketch > Edit.. Use the 2D sketch > Operation > Repeat, to repeat this circle involute by a symmetrical pattern with symmetry axis regarding the passing point, divide 360° by the number of teeth, then divide this result When repeating the circle involute with straight joint, The tooth becomes a closed sketch. Use the Op Heal option set to None and remove the lower line of the tooth. Repeat this result by a circular pattern (360° x the number of teeth) with the "Circular" joint method

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch elemen limitation to the sketch element.

Available Options: Linear Tolerance: Allows to modify the calculation accuracy of the tooth flank (0.01mm by default).

Curve by formula

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This command allows you to create a 2d curve by giving its Cartesian equations.

Creation Stages / Use: Select the 2D sketch > Operations > Curve by formula... command from the drop-down menu. 1. Enter the formulas according to the X and Y axes of your curve. 2. Enter the minimum and maximum intervals of parameter t.

It is important to systematically specify the unit of the values entered in the expressions. Whereas the parameter t does not have to have a unit

This command does not manage the curves that are not continuous in tangency. So it is necessary to check that the provided formulas properly generate a G1 type curve within the given interval.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element no The Tolerance contextual command allows to modify this approximation.

Available Options: Tolerance: The curve obtained is an approximation of the true curve by a B-spline curve generated at the tolerance given, this option allows you to refine the curve obtained.

Examples : Parabola Equations

Hyperbola Curve

Equations

Curv

Sinusoid Equations

Cam Equations 0° Offset... command from the drop-down menu. 1. Select a profile to parallelize. 2. By checking the Construction option, the selected profile will become a construction profile and will be internal. The offset will not be a construction profile. 3. Select the parallelization mode: Local mode: The default offset distance is 0. It is necessary to provide a list of segments to offset with an offset value for each of them thanks to the Special Segments option. Global mode: An offset distance has to be entered. Select the side of the offset or if it is centered. Revolution mode: A distance for segments parallel to the revolution axis and a distance for other segments have to be entered. One side: The parallel is on the side indicated by the arrow. Both sides: The parallel is on both side of the selected element. 2 different offset can be entered. Centered: The parallel is on both side of the selected element and centered. The entered value corresponds to the distance between the selected element and one of the two parallels.

TopSolid displays an arrow with a label allowing the distance and the direction of the parallel to be mod Dynamic modification of the distance Reversal of direction Modification of distance

Click the end of the arrow and move your mouse while holding down the button. Double-click the end of the arrow. Double-click the label displaying the distance and enter the distance val

It is not possible to create the parallel from a construction element or from an element inside the sket This command is a sketch operation.

This command creates a new sketch profile. With Local mode, if the selected profile in the one of the edited sketch, the result will be superimposed sketches. Fillets near special segments are not built again. Blends are added in some cases.

Available Options: Reverse:

The Reverse option allows the dimension of the parallel to be changed, this action can also be carried o double-clicking on the end of the arrow.

Special Segments: This dialog allows to give a special offset value on some segments of the selected profile. You can apply the special value between the selected segment and an end segment thanks to the Until.. option available in the contextual menu of the special value label.Then the Reverse option allows you to change the way to browse the profile.

Number (only available in global mode): You can indicate an instance number, each instance will be offset from the distance indicated.

Rounded joins (only available in global mode): This option allows a fillet equal to the offset distance to be created on all the convex vertices of the parallel profile. This fillet will be reported on all the instances of the parallel profile.

Thickened Links/Videos:

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This command allows to create an operation to thicken on open profile with the mode centered, one side or two sides. Extremities joints can also be managed.

Creation stages / Use: Click the menu. 1. 2. 3.

icon or select the 2D sketch > Operations > Thickened... command from the drop-down

Select the profile to thicken. The selected profile will be converted to a construction profile, by checking the Construction option. Select the type of offset. The thickness is distributed on both sides of the reference profile. Enter the total thickness. The thickness is on one side of the reference profile. Enter the total thickness. Select the side by clicking the yellow arrow in the workspace area. The thickness is on both sides of the reference profile. Enter the thickness for the first side. Enter the thickness for the second side. Select the side by clicking the yellow arrow in the workspace area. The double arrow indicates the second side.

4.

Check or not Rounded joints.

Without rounded joints

5.

Select the extremity joint: External arcs: The center of extremity arcs is coincident with the extremity of the reference profile.

With rounded joints

Internal arcs: The arc is coincident with the extremity of the reference profile.

Lines: Lines are perpendicular to the reference profile and coincident with the extremity of the reference profile.

6. Validate by clicking

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If the profile is closed, use the Parallel command.

Example of creation of a thickened profile. (In blue: reference profile, in orange : the thickened profile with centered mode).

Modifications / Additional information:

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element n The Tolerance contextual command allows to modify this approximation.

Project

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This command allows the edges to be projected in the current sketch plane.

Creation Stages / Use: Select the 2D Sketch > Operations > Project... command from the drop-down menu. 1. Select the type of elements to project. 2. Select the elements to project. 3. Validate creation of the projected elements with the

button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch elem The Tolerance contextual command allows to modify this approximation. The elements are projected in the sketch plan and invisible coincidence constraints are created betwee elements and the projected elements.

Available Options: Curves or edges: Allows you to project curves/edges/segments.

Profiles or loops: Allows you to project profiles/loops or boundary of a face.

Circles by diameter: Allows you to project only drillings circles or arcs. You just have to make a selection box to select them. All: All drillings parallel to the projection plane are projected. Diameter: Allows to select drillings diameters to project. If the drilling hasn't the entered diameter, it will not be projected. Tolerance: Allows to define the search tolerance. A 0.1mm tolerance allows to find all drills with a entered diameter +/- 0.05mm. Arc minimum: When a drilling is near the part border, it is not complete. the minimum arc allows to select only drilling with at least this angle.

Path between two edges: Allows you to project a path between tangent edges by selecting the first and the latest edges. Start edge: Select the first edge. The arrow indicates the direction of the path. Click Invert if needed.

End edge: Select the latest edge. Border: This mode can only be used with edges of a face. It allows to select all edges of the face. They can be tangent or not. Angle: If the angle between 2 following edges is smaller or equal to the entered angle, the edge is selected.

Paths around faces: Allows you to project the contours of the selected faces. The profiles are created as long as you select the faces: - If you select 2 neighbouring faces, the external profile on the 2 faces will be created only. - If you select 2 separate faces, two profiles will be created.

Modifications / Additional Information: This command is limited to the projection of lines, circle arcs, and plane faces, it is not possible to project ellipses, curves and non plane faces.

Intersection

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This command allows you to calculate the intersection curve between a shape or faces and the sketch plane.

Creation Stages / Use: Click on the icon down menu.

or choose the command 2D Sketch > Operation > Intersection... from the drop

1. Select the sketch's support plane. 2. Select the intersection type. creates all intersection curves between a shape and the sketch plane. creates intersection curves between several faces and the sketch plane.

3. Select the shape or faces, depending on the option chosen above. 4. Validate the creation of the intersection curve with the button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element n The Tolerance contextual command allows to modify this approximation. Only the shapes or faces that cross the sketch plane can obtain an intersection curve.

Modifications / Additional Information: This command is limited to the intersection with respect to the sketch plane.

Silhouette Links / Videos:

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This command allows to create the silhouette of a shape following a direction.

Creation Stages / Use: Click on the icon down menu.

or choose the command 2D Sketch > Operations > Silhouette... from the drop

1. Select the shape. 2. Select the direction. By default, this direction is normal to the sketch plane. It is the envelope's projection direction on the sketch support plane. 3. The Merge option allows, when checked, to reduce the number of segments of the silhouette. This option is not available when editing an old silhouette created before TopSolid 7.7. 4. Validate with the button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element n limitation to the sketch element. The sketch plane can be outside of the shape. The envelope will be projected according to the indicated dir

Available Options: Trimming plane: This option allows an envelope to be projected onto only a portion of the part. Offset: Defines a trimming plane that is offset from the sketch support plane by the entered value. By checking Invert, the trimming plane will be the other side of the sketch's support plane. Point: Allows you to select a point in order to define the offset of the trimming plane with respect to the sketch support plane. By checking Invert, the trimming plane will be the other side of the sketch's support plane.

Silhouette without a trimming plane

Silhouette with a trimming plane

Additional information: When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Revolved silhouette Links / Videos:

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This command allows to create a silhouette of a shape following a revolved axis.

Creation Stages / Use: Click on the icon or choose the command 2D Sketch > Operations > Revolved Silhouette... from the drop down menu. 1. Select the rotated shape. 2. Select the revolution axis. 3. The Merge option allows, when checked, to reduce the number of segments of the silhouette. This option is not available when editing an old silhouette created before TopSolid 7.7. 4. Validate by clicking .

The created profile is rotated if the rotated shape is a solid.

Example of a turbine

Revolved silhouette creation

Raw obtained by creation of the revolved shape by using the revolved silhouette

Modifications: Modifications are made to the silhouette by the popup menu.

Additional information: When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Enclosing Profile

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This command allows to create an enclosing profile of segments,profiles or sketches.

Creation stages / Use: Click the icon or select the 2D Sketch > Operations > Enclosing profile... command from the drop-down menu. 1. Select the sketch plane in which to work (if the sketch has not been edited yet). 2. Choose the type of element to enclose: Points, curves, profiles and shapes: This mode allows you to select points created with the Constructio sketch (with a rotative picking) or shapes. Sketches and shapes: This mode allows you to select the whole sketch or shapes.

3. Choose the type of enclosing profile to create: Rectangle

The selected elements are contained in a rectangle. The direction of the enclosing rectangle can be automatically computed or manually defin rectangle according to a specific direction.

Exemple of enclosing rectangle with automatic Exemple of enclosing rectangle with fixe direction (in magenta) Circle

The selected elements are contained in a circle. The center of the enclosing circle can be automatically computed or manually defined us

Exemple of enclosing circle with automatic center

Exemple of enclosing circle with defined magenta)

Obround

The selected elements are contained in a obround. The direction of the enclosing obround can be automatically computed or manually defin according to a specific direction.

Exemple of enclosing obround with automatic Exemple of enclosing obround with fixed direction magenta) Rectangle with fillets

The selected elements are contained in a rectangle with fillets.The value of the fillets can The direction of the enclosing rectangle can be automatically computed or manually defin rectangle according to a specific direction.

Exemple of enclosing rectangle with automatic Exemple of enclosing rectangle with fixe direction (in magenta) Convex hull

The selected elements are contained in a contour where concave areas are automaticall

Exemple of convex hull enclosing profile.

4. Set the tolerance value in order to get a more precise enclosing profile especially when elements to enclose are containing b-splines. A low tolerance will increase the computation time. 5. Validate the creation of the enclosing profile by clicking on the button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element n The direction calculated automatically allow to minimize the surface of the enclosing profile.

Available options: Forced size:

The size of the enclosing profile can be forced except for the Convex hull type. When this option is checked, a preview of the minimum enclosing profile is displayed with a thin orange line and the forced size profile is displayed with thick orange line.

When the Check option is checked, when the given size is lower than the minimum size, the areas located outside the given size are displayed in red:

Margins: This option allows you to add margins on each side of the enclosing profile except for Circle and Convexe hull types where single margin can be defined only. By checking Single margin, the entered value is applied to each side.

Rounding: This option allows you to define the precision that you want to get by rounding the values to their greater values. It cannot be applied on Convexe hull type. With an enclosing rectangle type (with or without fillets), the value defined in the Step field is applied to all the dimensions except if you define a value in the Second step field. In this case, the value defined in the Step field is applied to the length whereas the value defined in the Second step field is applied to the width.

No rounding

Rounding with 0,1mm

Rounding with 1mm

When a step value has been defined, a preview of the minimum enclosing profile is displayed in thin orange dotted line and the computed profile is displayed in orange thick line.

Repetition

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This command allows a sketch element according to a chosen pattern to be repeated (duplication with link).

Creation stages / Use: Select the 2D sketch > Operations > Repetition... command from the drop-down menu. 1. Select the profile to repeat. 2. Define the pattern to be applied and its parametering.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch eleme The Tolerance contextual command allows to modify this approximation.

Possibility to created a projected pattern regarding a 3D sketch pattern. Create a pattern on profile on a 3D sketch (frames orientation must be the same, for example "Constant"). Create the 2D sketch to repeat. Repeat this sketch. When the cursor is in the repetition dialog field Pattern, select a point of the pattern from 3d sketch.

Available Options: Join methods: This option allows you to choose the type of join between the instances of the pattern: Type None

Definition The repetition's elements are not joined.

Example

Straight

Circular (only available for circular patterns).

The repetition's elements are joined by a line.

The repetition's elements are joined by a curve.

Additional Information / Modifications: Modify the repetition from the operations tree, select your sketch, then right-click on the repetition and choose Edit from the popup menu.

Fillet Links / Videos:

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This command allows you to create a fillet on the vertex of a sketch.

Creation Stages / Use: Click the

icon or select the 2D sketch > Operations > Fillet... command from the drop-down menu.

1. Select the type of fillet. Local: The fillet is applied on each selected vertex. Global: The fillet is applied on each vertex of the sketch. Internal external: Like for global mode, the fillet is applied on each vertex of the sketch, but with different values for internal and external radii.

Example of fillets on each vertex, on the left with the Global mode, on the right with the Internal External mod

2. Enter the radius of the fillet. In case of using the Internal External mode, enter both internal and external radii. 3. Select a vertex of one element of the sketch. (With local mode) 4. Check Keep Vertex to keep the selected point. Fillet with vertex kept

Fillet with vertex not kept

5. With Global and Internal External modes, it is possible to modify the angular tolerance. It is the minimum angle from which the fillet will be created. Under this value, there will be no fillet on this vertex. 6. Validate by clicking .

Additional Information / Modifications: A fillet is considered as a circle arc, from the popup menu you can: Constrain the center of the circle arc on an element with the Define center... command. When the center point no longer exists, recreate the circle arc's center point with the command Create center.

The Internal external mode only works with a closed sketch.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Extension Links / Videos:

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This command allows you to extend a profile.

Creation Stages / Use: Click the icon or select the 2D sketch > Operations > Extension.. command from the drop-down menu. 1. Select the profile to extend. 2. Select whether it is the start or the end of the profile that is to be extended. 3. Validate with the button.

The Tolerance contextual command allows to modify this app

Available Types:

Curvature:

The curvature radius of the curve is constant.

Tangent:

The segment is tangent to the curve.

Exact :

The extension follows the probable evolution of the curve based on its last points (takes into account the curvature and the

Fitting Links / Videos :

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This command is used to fit and sew the selected profiles between them, if their distance is within the specified tolerance.

Creation stages / Use: Click the menu.

icon or select the 2D sketch > Operations > Fitting... command from the drop-down

1. Select the profiles to adjust. 2. Enter the adjustment tolerance. It is the distance in which must be extremities points of profiles to fit. 3. Validate with the button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Trim

This command allows a profile to be cut or shared at the intersection with another entity (profile point, face, plane, or at a certain distance).

Use: Click the icon or select 2D Sketch > Operations > Trim... from the drop-down menu. 1. Select the profile to trim or share. 2. Choose the trimming entity: Point Profile Length

Face Plane

Select the point that will trim the profile. The point must be on the profile. Select the profile that will trim the profile. The two profiles must intersect at a point. Enter the length at which the profile will be trimmed or shared. The length is the distance from the profile's point of origin. Select the face from a shape that will trim the profile. The profile must cross this face. Select the plane that will trim the profile. The plane is considered to be infinite.

3. Check Invert if necessary. The preview represents the kept portion. 4. Check Share if necessary. The profile will be cut in two, but the two parts will remain available.

5. If the trimming must be done on both sides of the profile (the profile will be segmented into three parts), check Second trimming. 6. Choose the second trimming entity: Point Profile Length

Face Plane

7. Validate by clicking

Select the point that will trim the profile. The point must be on the profile. Select the profile that will trim the profile. The two profiles must intersect at a point. Enter the length at which the profile will be trimmed or shared. The length is the distance from the profile's point of origin. Select the face from a shape that will trim the profile. The profile must cross this face. Select the plane that will trim the profile. The plane is considered to be infinite.

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The point, profile, or trimming face must intersect the profile. The preview represents the kept portion. If the portion to save is on the bad side, use the Invert option.

Continuity adjustment

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This command allows to force the tangency on the extremities of an open curve. The operation consists in modifying the second (or next to last) control point of the curve by projecting it on the direction imposed. This function is used to adjust the tangency between two almost tangent curves.

Creation stages / Use: Select the 2D sketch or 3D sketch > Operations > Continuity adjustment... command from the dropdown menu. 1. 2. 3. 4.

Select the profile near the extremity to modify. Select the type of modification to be applied to the profile. Select the type of influence. Select the curve of reference.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation. If the curve is not a Spline, it is converted.

Available Options: Type: Position: The extremity of the curve to modify is superposed to the reference curve. Tangency: The extremity of the curve to modify is not moved, but it is bent to be tangent with the extremity of the reference curve. Position and tangency: Both modifications are applied.

Influence: Local: allows to confine the modifications near the considered extremity. Distributed: allows to modify several control points, on a sliding scale way. This method is recommended when there is a large number of control points, in order to avoid a too strong variation of the curve. The influence length is measured on the control polygon in order to know which points will be modified.

Segments removing Links / Videos:

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This command allows segments to be deleted both in a sketch and in sketch operations. This command is more advanced than the Deletion command (DEL key on the keyboard).

Creation Stages / Use: Click the icon or select the 2D sketch > Operations > Segments Removing... command from the drop-down menu. For a Unfolding document, select the Unfolding > Segments Removing on Unfolding... command from the drop-down menu. 1. Select the segments to be deleted. 2. Select a type of heal based on the options defined below. 3. Validate.

Available heal types:

The red crosses denote segments to be deleted.

Heal type: None The segments are deleted.

Heal type: Join The segments are deleted and replaced by a segment that connects the two end points.

Heal type: Extend/Limit The segments are deleted, and the remaining segments are extended.

Additional options for Extend/Limit healing type: These additional options are effective only for extending circular segments. By tangency:

Deleted segments are replaced by lines that run tangent to the circular segments having a common point with the deleted segments. (the segment to delete in blue and the preview of the result in orange).

By Curvature: Deleted segments are replaced by the extended circular segments that had a common point with the deleted segments. (the segment to delete in blue and the preview of the result in orange).

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Arcs lines conversion Links/Videos:

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This command allows to transform as arcs and lines, complex curves like ellipses, splines,... to allow some machining software to be able to import our unfolding and machining trajectory exports.

Creation stages / Use: Click the icon or select the 2D sketch or 3D sketch > Operations > Lines Arcs Conversion... command from the drop-down menu. 1. Edit the sketch and select the profile or segment to convert. 2. Enter linear and angular tolerances. 3. Validate by clicking .

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Available Options: Tolerances: Linear tolerance: It indicates the maximum gap value authorized with simplified curves. Angular tolerance: It indicates the maximum angle value authorized at the angle of tangency between two successive segments.

Large radii polygonization: When it is checked, this option allows to replace by polygons, built arcs when the radius is higher than the entered value, to avoid error messages on the punch, cut and machining programs.

Modifications / Additional information: The modification of the conversion is done from the operations tree, select the sketch, then right click on your conversion and select the Edit command from the contextual menu.

Split Segment

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This command allows to divide a segment in two segments.

Creation stages / Use: Select the 2D Sketch > Operations > Split Segment... command from the drop-down menu. Select the segment to split and give the division point.

When the point is outside the segment, it is projected perpendicularly on the segment. A command with the same name is also available in the 3D Sketch > Operations menu.

Profile Origin and Orientation

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This command allows to modify the origin and the direction of a profile.

Creation stages / Use: Select the 2D Sketch > Operations > Profile Origin and Orientation... command from the drop-down menu. Three selection modes are suggested: All profiles: all the profiles of the sketch are selected. In this case, orientation of the profiles can be modified only. List of profiles: this mode allows you to select several profiles one by one. In this case, orientation of the profiles can be modified only. One profile: this mode allows you to select one profile only. In this case, origin and orientation of the profile can be modified. When the profile has been selected, TopSolid displays a circle at the origin of the profile and also a blue arrow which shows the direction of the profile. Then you can: double-click on the arrow or check the Orientation option in order to revert the direction of the profile(s).

choose the Orientation for all the selectionned profile, choose a direction (reverse, clockwise or anti-clockwise).

This modification is an operation, it is not visible in the sketch edition. A command with the same name is also available in the 3D Sketch > Operations menu.

Available options: With the One profile mode and if this profile is closed, the Origin option allows you to locate the new origin of the profile. For this, three modes are available: Point: this option allows you to define the new origin by selecting a point. Middle point: this option allows you to define the new origin from a middle point of one segment of the profile. Ratio point: this option allows you to define the new origin from a point positionned along a segment (the 0 ratio correspond to the origin of the segment, the 0,5 ratio correspond to the middle of the segment and the 1 ratio correspond to the end of the segment). In these 3 modes, when the point is not on the profile, it is automatically projected according to the perpendicular direction on the nearest segment.

The Offset field allows you to move the origin with the given value according to the arrow direction.

Middle Links/Videos:

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This command allows to create a middle profile between two profiles.

Creation stages / Use: Click the menu. 1. 2. 3. 4. 5.

icon or select the 2D sketch > Operations > Middle... command from the drop-down

Select the first profile. Select the second profile. Select the type of synchronization. Select the matching. Validate with the button.

Example of a middle profile in orange with its reference curves in blue and magenta.

To calculate the middle curve, TopSolid matches together a succession of points on each curve the calculate the middles points of each pairs and then draw a curve through these middle points.

Different types of synchronization: Sweep synchronization corresponds to how TopSolid corresponds sections together. Arc Length: When you use curvilinear synchronization for the sweep, this means that when the shape is c in done in proportion to the length of each one.

Parametering: When you use parametric synchronisation for the sweep, this means that when the shape correspond to the nature settings of the sections. Example: The parametric extension of a line is [0;1] (length) The parametric extension of a circle is [0;360] (angle)

a: Line: parametric extension [0;1]

b: Arc: Parametric Extension [0;54]

Different types of matching: Different types of matching are below: Profile to profile: During the middle profile creation, TopSolid tries to match overall profiles regarding their built settings. The result is only a profile. It is the default mode, it gives generally good results. Segment to segment: During the middle profile creation, TopSolid try to match segments of each profile two by two. The result gives a profile for each couple of segments. This option can only be used if profiles have the same number of segments.

Modifications / Additional information:

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Section

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This command allows you to create a section between different profiles. This section can be used in the Extrusion command to extrude the profiles included in the section without taking into account other possible sketch profiles.

Creation stages / Use: Click the menu.

icon or select the 2D sketch > Operations > Section... command from the drop-down

1. Select the different profiles. 2. Select the hatch type. 3. Select the spacing of the hatches, as well as the orientation and the offset according to X and Y.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch elem The Tolerance contextual command allows to modify this approximation.

Modifications / Additional information: You can change the sketch or section using the corresponding popup command.

The hatch type has no effect on using the sketch.

Profile

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If a sketch is created with the sewing manual mode (option available in 2D or 3D sketch > Options...), this command allows to transform a batch of segments to profile. This can be used in an extrusion, trim, etc.

Creation stages / Use: Click the menu.

icon or select the 2D sketch > Operations > Profile... command from the drop-down

1. Select the different segments. 2. Validate by clicking .

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch elemen The Tolerance contextual command allows to modify this approximation.

If this command is grayed, it is because the sewing mode is set to automatic (available option in 2D or 3D sketch > Options...).

Selected segments are highlighted.

Seedling

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This command allows to create a batch of points randomly inside a closed profile.

Creation stages / Use: Select the 2D Sketch > Operations > Profiles Batch > Seedling... command from the drop-down menu. 1. Select the section. 2. Enter the points count you want inside this section. 3. Validate.

Distribution of 40 points without minimum distance

Distribution of 40 Since minimum distance is a pri

Once points are created you can move them. Select a point and drag it to another position (because dynamic is not managed, the point will change position as you release the cursor). Possibility to change the random position of points. Right click on one point then under the Seedling title select the Force update command.

Available options: Minimum distance: Possibility to ask for a minimum distance between each point. Distance between points will greater than or equal to the enter value.

Modifications / Additional information: The element thus created is an operation, its updating is carried out after solving the sketch.

This element is not therefore visible during editing the sketch and cannot be limited by a sketch element nor used as a limitation to the sketch element.

Seedling on profile

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This command allows to randomly distribute points on a profile.

Creation stages / Use: Select the 2D Sketch > Operations > Profiles Batch > Seedling on profile... command from the drop-down menu. 1. Select the profile on which points will be created. 2. Enter the points count you want to create. 3. Validate.

Once points are created you can move them. Select a point and drag it to another position (because dynamic is not managed, the point will change position as you release the cursor). Possibility to change the random position of points. Right click on one point then under the Seedling title select the Force update command.

Available options: No minimum distance:

The points are randomly placed on the profile.

Minimum distance: The points are randomly placed on the profile by maintaining a minimum distance between each point.

Distribution of 5 points with a minimum distance of 10mm

Distance along a direction: The points are randomly placed on the profile by maintaining a minimum distance between each point according to a direction.

Distribution of 5 points with a minimum distance of 10mm on X axis

Modifications / Additional information: The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element nor used as a limitation to the sketch element.

Triangulation

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This command allows to create a Voronoï diagram or a Delaunay triangulation from a batch of points

Creation stages / Use: Select the 2D Sketch > Operations > Profiles Batch > Triangulation... command from the dropdown menu. 1. Select the triangulation type to create. 2. Select points to use. Seedling points Explicit points Serial points 3. Validate.

Voronoï diagram A cell is created around each point

Delaunay triangulation Triangles are created using points as vertex

Each triangle (Delaunay) or each cell (Voronoï) are closed profiles. When a point is moved the triangle/cell will be updated.

Available options: Margin: Option available with Voronoï diagram only. This triangulation will create a rectangle parallel to X and Y axes of the sketch frame and passing through extreme points on X-/X+ and Y-/Y+ (see first image above).

The margin value is the gap from these extreme points and the rectangle curves.

Make result convex: Option available with Delaunay triangulaton only. This option adds triangle to make the result convex.

Delaunay without Make result convex option

Delaunay with Make result convex option Red curves have been added to create new triangles

Modifications / Additional information: The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element nor used as a limitation to the sketch element.

Interior offsets

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This command allows to create closed profiles parallel to a batch of closed profiles.

Creation stages / Use: Select the 2D Sketch > Operations > Profiles Batch > Interior offsets... command from the drop-down menu. 1. Select profiles to use. Triangulation profiles Explicit profiles Serial profiles 2. Enter the distance value. 3. Validate.

Interior offsets example (in green) from a triangulation of type Voronoï diagram

Modifications / Additional information: The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element nor used as a limitation to the sketch element.

Interior Bsplines

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This command allows to create interior Bsplines of closed profiles.

Creation stages / Use: Select the 2D Sketch > Operations > Profiles Batch > Interior Bsplines... command from the drop-down menu. 1. Select profiles to use. Triangulation profiles Explicit profiles Serial profiles 2. Enter the distance value. 3. Validate

Interior Bsplines example (in green) from a

triangulation of type Voronoï diagram

Modifications / Additional information: The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element nor used as a limitation to the sketch element.

Cells

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This command allows to create closed profiles from a batch of intersecting open profiles.

Creation stages / Use: Select the 2D Sketch > Operations > Profiles Batch > Cells... command from the drop-down menu. 1. 2. 3. 4.

Select the first batch of open profiles. Select the second batch of open profiles. Enter the offset value. Validate.

Example of cells creation (in green) from blue batch and red batch

In each open profiles batch, the selection order influences the cells creation: First cell is created between profiles 1 and 2 of first profiles batch and second profiles batch. A second cell is created between profiles 2 and 3 of first profiles batch and second profiles batch. Etc... The same if profiles come from a repetition in which pattern uses Alternated numbering mode.

First created between 1-2 et 1-2

Second cell created between 2-3 et 1-2

Last cell created between 3-4 et 1-2 (orange cell). This cell is superimposed to previous cells

Available options: Batch of open profiles: In Special inputs of open profiles batch field, possibility to use: Explicit profiles Serial profile

Modifications / Additional information: The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element nor used as a limitation to the sketch element.

View sketch from top

This command orients the current view of the sketch to a top view in relation to the sketch frame.

Creation Stages / Use: Click on the icon or choose the command 2D Sketch > Visualization > View sketch from top... from the drop down menu. There is no validation. When using this command, the current view is immediately oriented.

If your document is splitted in several views, only the current view will be modified.

View sketch in perspective

This command orients the current view of the sketch in perspective in relation to the sketch frame.

Creation Stages / Use: Click on the icon or choose the command 2D Sketch > Visualization > View sketch in perspective... from the drop down menu. There is no validation. When using this command, the current view is immediately oriented.

If your document is splitted in several views, only the current view will be modified.

Zoom in on sketch

This command allows you to zoom to fit the sketch in the current view.

Creation Stages / Use: Click on the icon or choose the command 2D Sketch > Visualization > Zoom on Sketch... from the drop down menu. There is no validation. When using this command, the current view is immediately oriented.

If your document is splitted in several views, only the current view will be modified.

Orient front of cut Links / Videos:

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This command allows the camera in front of the active graphic cut to be oriented.

Creation Stages / Use: Select the 2D sketch > Visualization > Orientate front of cut... command from the drop-down menu. Launching the command automatically orients the camera perpendicularly to the active cut plane.

Modifications / Additional information: A graphic cut is created using the Cut command of the Visualization menu.

Final attributes Links/Videos:

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This mode allows to visualize a 2D or 3D sketch with its final attributes (segment style and color), also during sketch edition.

Creation stages / Use: Select the 2D or 3D sketch > Modes > Final attributes or click the icon in the right part of the 2D or 3D sketch tab. (Index 1. on the screenshot below).

1. Final attributes (Mode activated)

2. Current type

3. Current attributes

When a new style and/or color is chosen, its representation (index 3. on the picture above) is modified. To delete the style or the color, click the icon.

Attributes will only be applied during a new profile creation. To modify attributes of an existing profile, use the Attributes

contextual menu. This mode must be activated to be able to modify current attributes. When this mode is activated, constraint colors (blue, magenta, ...) of the sketch are no more visible.

Construction

This mode allows the construction mode for the new sketch entities to be enabled or disabled. The sketch entities in construction mode are useable in the sketch, but cannot be used for shapes. It is not possible to extrude them, rotate them, make embossments or pockets with construction entities.

Use: Click the icon or select the 2D sketch or 3D sketch > Modes > Construction command from the drop-down menu. When this mode is enabled, the new entities created in the sketch are in construction mode. When this mode is disabled, the new entities created in the sketch are in normal mode

Modifications: The popup menu allows the construction entities to be transformed into normal entities by selecting No construction, and normal sketch entities into construction entities by selecting Construction.

Additional Information: By default, the construction entities are inside the sketch. This mode is enabled when the icon is pressed (the background remains colored).

Dynamic Symmetry

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This command allows to symmetrize sketch entities during their creation.

Creation stages / Use: Click the icon or select the 2D Sketch > Modes > Dynamic Symmetry... command from the drop-down menu. 1. Select the type of symmetry. The symmetry is not active. the mode is deactivated. Simple symmetry. Select: Sketch OX axis to symmetrize regarding the OX axis. Sketch OY axis to symmetrize regarding the OY axis. Specified axis to select the symmetry axis. Double symmetry. Select: Sketch OX and OY axes to double symmetrize regarding the two sketch axes. Specified axis to select the two symmetry axes.

2. Validate. As long as the mode is active (orange background), the symmetry is done.

This mode is only used during the creation. To symmetrize sketch entities after their creation, use 2D sketch > Other modifications > Symmetry or 2D sketch > Operations > Repetition. The created entities by dynamic symmetry are displayed with small arrows oriented towards the symmetry axis. By clicking one of these arrows, both symmetrized entities are highlighted.

Only creation of basic entities commands (line, circle, arc, rectangle, ellipse, spline, ....) are taken in account during the symmetry. Entities that refers to other entities (as symbol, standard curves, edge copy commands) are not symmetrized Commands which modify the geometry (fillet, chamfer, extent, offset, ....) are not symmetrized.

Magnetic grid

In sketch mode, this mode allows hooking on the grid to be enabled or disabled.

Steps of use: Click the icon or select the 2D sketch or 3D sketch > Modes > Magnetic grid command from the drop-down menu. In a draft document, use the Sketch > Modes > Magnetic grid command. When this mode is enabled, the pitch and number of grid intervals attracts the selection point. The pitch and number of grid intervals can be defined by using the function Modify grid.

Additional information: This mode is enabled when the icon is pressed down (the background stays in color).

Projection

This mode allows the sketch's projection mode to be enabled or disabled

Use: Click the icon or select the 2D sketch or 3D sketch > Modes > Projection command from the drop-down menu. When the projection mode is enabled, hooking of the point clicked is projected in the support plane of the current sketch. When the projection mode is disabled, only hooking of the point clicked in the support plane of the current sketch is possible.

Example: When the mode is activated, the green points selection is possible. If the mode is deactivated, only the red points selection is possible.

Additional information: This mode is enabled when the icon is pressed down. (background stays in color).

Automatic dimensions

This mode enables automatic dimensioning of sketches to be enabled or disabled.

Use: Click the icon or select the 2D sketch or 3D sketch > Modes > Automatic dimensions command from the drop-down menu. In a draft document, use the Sketch > Modes > Automatic dimensions command. When this mode is enabled, simple closed sketches (rectangles, circles, etc...) are automatically dimensioned. When this mode is disabled, simple closed sketches (rectangles, circles, etc...) will have to be dimensioned manually.

Additional information: This mode is enabled when the icon is pressed (the background remains colored).

Ask dimension value

This mode allows asking for the dimension value to be enabled or disabled.

Use: Click the icon or select the 2D sketch or 3D sketch > Modes > Ask dimension value... command from the drop-down menu. In a draft document, use the Sketch > Modes > Ask dimension value command. When this mode is enabled, the value of the dimension put in is proposed, all you need to do is validate or modify it. When this mode is disabled, the dimension is put in without its value being asked for.

Modifications: The modification of the value of a dimension is made by doubleclicking on the dimension text when no command is launched (neutral mode).

Additional information: This mode is enabled when the icon is pressed (the background remains colored).

Automatic alignments

This mode allows the automatic creation of alignment constraints to be enabled or disabled between the sketch elements.

Use: Click the icon or select the 2D sketch or 3D sketch > Modes > Automatic alignments command from the drop-down menu. In a draft document, use the Sketch > Modes > Automatic alignments command. When this mode is enabled, the alignment relations are created automatically. When this mode is disabled, the alignment relations are not created.

This mode is additional to the mode Automatic relations which creates the constraints of the element being created.

Additional information: This mode is enabled when the icon is pressed (the background remains colored).

Automatic relations

This mode allows the automatic creation of relations between the sketch entities to be enabled or disabled.

Use: Click the icon or select the 2D sketch or 3D sketch > Modes > Automatic relations command from the drop-down menu. In a draft document, use the Sketch > Modes > Automatic relations command. When this mode is enabled, the relations (alignment, horizontal, vertical, tangency, coincidence, etc..) are created automatically. When this mode is disabled, the relations are not created.

Activation of this mode may over-constrain the sketch. In this case, the relations of no use must be deleted manually.

Additional information: This mode is enabled when the icon is pressed (the background remains colored).

Show relations This mode allows the display of relations to be enabled or disabled.

Use: Click the icon or select the 2D sketch or 3D sketch > Modes > Show relations command from the drop-down menu. In a draft document, use the Sketch > Modes > Show relations command. When this mode is enabled, the relations (alignment, horizontal, vertical, tangency, coincidence, etc..) are visible. When this mode is disabled, the relations are not displayed.

Additional information: This mode is enabled when the icon is pressed (the background remains colored).

Show internal elements

This mode allows the elements inside the sketch to be shown or hidden.

Use: Click the icon or select the 2D or 3D sketch > Modes > Show internal elements command from the drop-down menu. In a draft document, use the Sketch > Modes > Show internal elements command. When this mode is enabled, the elements inside the sketch (construction lines, etc..) are visible. When this mode is disabled, the internal elements are not displayed.

Additional information: This mode is enabled when the icon is pressed down. (background stays in color).

Show orientations

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This command shows by an arrow the orientation of each entity of the sketch.

Creation Stages / Use: Click the icon or select the 2D or 3D sketch > Modes > Show orientations... mode from the drop-down menu.

This mode is useful to check if segments of an angle are in the same direction, which is better in case of equations or symmetries. It is not possible to reverse an entity. Only a variable can be reversed by using the Reverse contextual command.

Show extremities Links / Videos:

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This command shows the extremities of the sketch if they are not closed.

Creation Stages / Use: Click the icon or select the 2D sketch > Modes > Show extremities... command from the drop-down menu.

If the sketch is closed, there are no extremities. This mode allows you to quickly locate where the sketch is open.

Available Options: You can change the color and diameter of the representation in the sketch options.

Show superpositions

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This command shows if segments are superposed.

Creation Stages / Use: Click the icon or select the 2D sketch or 3D sketch > Modes > Show ends... mode from the drop-down menu.

3 segments are superposed between A and B: one for each rectangle and one line.

Each grey circle represents a superposed segment (between A and B).. This mode allows you to quickly locate where are superpositions.

Available Options:

You can change the color and diameter of the representation in the sketch options.

Automatic Hatching

This command allows to automatically create hatching on closed profiles. This allows to quickly recognize them.

Use: Click the icon or select the 2D Sketch or 3D Sketch > Modes > Automatic Hatching... command from the drop-down menu. When this mode is activated, a hatching is displayed on all the closed profiles. When this mode is not activated, no hatching is displayed..

The hatching angle and spacing cannot be modified, nor configured.

Example:

Show Tool Diameter

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This mode allows to create an obround corresponding to the machining tool diameter. This mode will be mainly used for a mouse facing in TopSolid4cam

Use: Click the icon or select the 2D Sketch > Modes > Show Tool Diameter... command from the drop-down menu. Choose the tool diameter and validate with the

.

Then, an obround corresponding to the tool diameter is displayed on all the segments of the sketch. This obround will be displayed on new segments as well.

Filter external geometries Links / Videos :

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This mode allows external geometries (faces, edges, others sketches) to be taken or not to be taken into account during the creation of relations between the sketch's elements. See also: Filter faces.

Creation stages / Use: Click the icon or select the 2D Sketches > Modes > Filter External Geometries... command from the drop-down menu. When this mode is enabled, no external geometry is taken into account during the creation of relations between the sketch's elements. When this mode is disabled, external geometries are taken into account during the creation of relations between the sketch's elements.

When this mode is not enabled, during the creation of a sketch element, passing over a cylindrical face or edge will automatically set off the creation of a coincidence constraint with these elements, which can be annoying in some cases. It is then preferable to disable this mode.

Additional information: This mode is enabled when the icon is pressed (the background remains colored).

Filter faces

This mode allows the faces to be taken or not to be taken into account during the creation of relations between the sketch's elements. See also: Filter external geometries.

Creation Stages / Use: Click the icon or select the 2D sketch > Modes > Filter Faces command from the drop-down menu. When this mode is enabled, the faces are not taken into account during the creation of relations between the sketch's elements. When this mode is disabled, the faces are taken into account during the creation of relations between the sketch's elements.

When this mode is not enabled, during the creation of a sketch element, passing over a cylindrical face will automatically set off the creation of a coincidence constraint with the cylinder's axis, which can be very annoying, in this case it is preferable to disable it.

Additional information: This mode is enabled when the icon is pressed (the background remains colored).

Cross section Links / Videos:

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This command allows to activate the graphic cross section in the plane of the editing sketch.

Creation Stages / Use: Click the icon or select the 2D sketch > Modes > Cut... command from the drop-down menu.

Modifications / Additional information: The color of the cut plane can be configured in Tools > Options > Sketch section. A graphic cross section is created using the Cross section command of the Visualization menu.

Filter Links / Videos:

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This command makes it possible to filter (mask) the elements of an imported sketch (Dxf, Dwg, Iges, etc.) by color, line type, or element type.

Creation Stages / Use: Select the 2D sketch > Healing > Filter... command from the dropdown menu. TopSolid proposes colors and lines types used in the imported sketch. 1. Select a color or line type to mask it. 2. Validate the creation of constraints with the button.

This command can only be used with an imported sketch. It cannot be launched when a sketch is being edited.

Available Options: The All option makes it possible to display all of the sketch's elements, while the Segment option masks dimensions, text, and notes from the imported sketch. The Reset button displays again all of the filtered elements.

Clean Links / Videos:

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This command makes it possible to delete superimposed circles and lines from an imported sketch (Dxf, Dwg, Iges,...).

Creation Stages / Use: Select the 2D sketch > Healing > Clean... command from the dropdown menu. 1. 2. 3. 4.

Select the sketch or elements to clean. Enter linear and angular tolerances values. Move to the result viewing stage with the button. Validate the cleanup with the button.

This command can only be used with an imported sketch. It cannot be launched when a sketch is being edited.

Available Options: The Verify Color and Verify Line Type options make it possible to consider only the elements with the same line type and color. For example, if you uncheck the Verify Color option, you can clear two segments with different colors.

Modifications / Additional information: When the distance between two elements is less than the specified tolerances, the two elements are considered to be superimposed and are replaced by a single element.

Rebuild Links / Videos:

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This command rebuilds a circle arc from a multitude of small segments.

Creation Stages / Use: Select the 2D sketch > Healing > Rebuild... command from the drop-down menu. 1. 2. 3. 4.

Select the segments to rebuild. Enter the linear tolerance value. Move to the result viewing stage with the Validate the cleanup with the button.

button.

This command can only be used with an imported sketch, it can't be used during the sketch edition.

Available Options: If profiles are not continuous and if the distance between their extremities is smaller than the tolerance, the Adjust profiles option allows to link them.

Sketch options Links / Videos:

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This command allows to modify the sketch behavior by sewing or not profiles together, by verifying or cleaning automatically the sketch, by managing the splines extension of the editing sketch.

Creation stages / Use: Select the 2D sketch > Options... command from the drop-down menu.

Profiles. Allows to manage the profiles sewing. Automatic: Different entities (lines, arcs, splines, ...) are automatically sewed together to create a profile. The result can be extruded. Semi-automatic: Several closed profiles can be sideby-side. The extrusion will always be possible. (see the example below). Manual: Different entities (lines, arcs, splines, ...) are not sewed together to create a profile. This sew operation has to be done manually by using the Profile command. Non sewed profiles are displayed with thin lines, they can be extruded. None: It will not be possible to sew different entities (lines, arcs, splines, ...) to create a profile.

Automatic mode:

Semi-automatic mode:

The profile on the left has The profile on the left has been been added. Its incompatible added. Segments are not dotted. segments with an extrusion The extrusion is not possible. are dotted. The extrusion result will be a surfacic square and a flat surface (extrusion of the line).

Check. Advanced options.

The Large radius value is a step at which a circle will be deformed differently during its resolution by the solver. Below this threshold, for a rather short radius, it will not be able to change the sign of curvature and will always remain on the same side of the chord. This curvature sign change can be seen using the deformation command. Otherwise, if the radius becomes to large, it could cross its chord and reverse its curvature.

The large radius option has only to be use for uncommon cases like a radius of several kilometers for railway rails. The default threshold is set to R = 1m which correspond to a diameter of 2m. We highly recommend that you do not change this numerical threshold.

3D Sketch Links / Videos:

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The sketch creation is done by clicking the icon. A sketch is an element composed of geometric and constrained elements.

Creation Stages: Choose the command 3D Sketch > Sketch.. from the drop down menu. Spatial sketch may contain constrained planes as well as other geometries. When creating a spatial sketch, 3 orthogonal planes corresponding to XY, XZ and YZ of sketch frame are created. Infinite construction lines corresponding to axes are also created like in a planer sketch. These geometrical entities are not modifiable. The absolute frame is automatically displayed with perspective. When the sketch is created, all commands from Spatial sketch are available. This mode is symbolized by the button containing the name of the sketch displayed in the top center of the graphic area, this button also allows you to exit the Sketch mode by validating it by clicking near the blue check. By clicking the red cross, you will quit the sketch edition and will cancel all what you have done during this edition.

When an element is being created, you can use the Ctrl + Space keys to change input automatically positioned on the last input point.

Additional Information: This command is automatically used when using an entity creation command like Point, Line, Rectangle,...

Position sketch Links / Videos:

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This command allows you to fix the origin and the axes of your sketch on a particular point of your part. A sketch is positioned by selecting a support plane, an origin and a direction (horizontal or vertical).

Creation Stages: You must first create a sketch. When a sketch has been created, click the icon or select the 3D sketch > Position sketch.. command from the drop-down menu. 1. 2. 3. 4. 5.

Select the sketch's support plane. Select the point defining the origin of the sketch. Choose the direction you wish to define (X or Y). Select the direction defining the X or Y axis. Validate by clicking .

This command also allows to move a sketch from a frame to another. It will stay orientated according to the new reference point and new X and Y axes.

Position entry plane

This command defines the temporary input plane of the elements of your 3D sketch. As for the positioning of a planar sketch, the input plane is positioned by selecting a support plane, an origin and a direction (horizontal or vertical).

Creation Stages: When a sketch has been created, click the icon or select the 3D sketch > Position sketch plane... command from the drop-down menu. 1. 2. 3. 4.

Select the sketch's support plane. Select the point defining the origin of the sketch. Choose the direction you wish to define (X or Y). Select the direction defining the X or Y axis.

This input plane is temporary, the definition of a new input plane causes the previous plane to be deleted.

When an element is being created, you can use the Ctrl + Space keys to change input planes (toggle XZ then automatically positioned on the last input point.

Contour Links / Videos:

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The Contour command automatically allows a succession of lines and arcs to be created with coincidence relations.

Creation Stages: Click on the

icon or choose the command 3D Sketch > Contour.... from the drop down menu.

1. Chose a creation mode of the segment, the Line mode is chosen by default. Line

Creation of a line by two points. : The cursor can move freely in the sketch plane : The cursor can move horizontally or vertically. : The cursor can move horizontally only.

Arc Tangent arc

: The cursor can move vertically only. Creation of a circle arc by three points. Creation of an arc tangent to the last element of the contour. Creation of an arc perpendicular to the last element of the contour.

Perpendicular arc Plane

Creation of a segment from the last created point to the selected plane. Extended: The previous segment is extended up to the plane. Distance: The created segment will have the requested distance that corresponds to the start point and the destination plane point.

2. Enter the coordinates of the segment's passing points.

If you wish to create a closed contour, finish your contour by clicking the start point of the contour again or click the last segment of the contour. Otherwise, click the icon or press the Esc key to exit the command and create an open contour. The creation mode chosen is used just once, then it switches to the Line mode, except if Lock the mode option is checked.

When an element is being created, you can use the Ctrl + Space keys to change input planes (toggle XZ then YZ), then the input pla automatically positioned on the last input point.

Available Options: The Lock mode allows to lock the interactive mode to stay permuted. For example, when with the Interactive mode, you move the cursor on the last vertex of the contour, TopSolid automatically switches to tangent arc. When the arc is created, it automatically switches back to line. By checking this mode before creating the arc, it will be active after positioning the arc and another arc will be proposed. Interactive mode allows to switch between different Line mode, Tangent Arc and Perpendicular Arc by moving cursor on the last edge of under construction contour. By default, in the circle, tangent circle or perpendicular circle mode, the circle arc is created in the trigonometric direction (counter-clockwise), check the Additional Arc option to change to clockwise.

Additional Information / Modifications: When a contour vertex is re selected, the construction mode is automatically enabled. When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element

Point Links / Videos:

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A point is created either by entering the coordinates in the dialog panel, or directly from the graphics zone by locating a point or selecting an element.

Creation Stages: Click on the icon or choose the command 3D Sketch > Point... from the drop down menu. Creation by the dialog panel: Enter the point coordinates. Creation from graphic area: Locate a point on the grid or select an element.

When an element is being created, you can use the Ctrl + Space keys to cha automatically positioned on the last input point.

Modifications / Additional Information: Click on a point and move your mouse while holding down the left button to modify the position of the point.

When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are

Point on shape Links/Videos:

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This command allows to create a point constrained on a shape.

Creation stages / Use: Choose the command 3D Sketch > Point on Shape... from the drop down menu. 1. Select the location of the point by clicking a face or edge of a shape.

The point is constrained onto the selected face and can be move freely through all tangent neighboring faces of the shape. The point cannot be moved beyond sharp edge of the face.

Modifications / Additional information: You can directly move the point without editing the sketch.

Line Links / Videos:

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A line is created either by entering the coordinates of the start point and end point in the dialog panel, or directly from the graphics zone by locating two points on the grid or on elements.

Creation Stages: Click on the icon or choose the 3D Sketch > Line... command from the drop down menu. Creation by the dialog panel: Enter the coordinates of two line points. Creation from graphic area: Locate two points on the grid or on elements. It is of course possible to mix the creation modes by indicating for example the coordinates of the line's start point in the dialog panel and describing an element to indicate the end point.

When an element is being created, you can use the Ctrl + Space keys to change input automatically positioned on the last input point.

Modifications / Additional Information:

Displacement of an end: Click the end of a line and move your mouse while holding down the left button to modify the position of this end. Displacement of the line: Click the line and move your mouse while holding down the left button to modify the position of the line.

Available Options: Infinite: This checked option allows to create an infinite line and using the construction mode. In this case, the line is represented like an axis line of the sketch. It is defined by two passing points.

When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are

Circle Links / Videos:

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A circle is created either by entering the coordinates in the dialog panel, or directly from the graphics zone by locating a point or selecting an element.

Creation Stages: Click on the icon or choose the command 3D Sketch > Circle.... from the drop down menu. Creation by Center and passing point: 1. In the Size topic, select Free Size mode. 2. Check Given Center. 3. Enter the coordinates of the center point and the passing point of the circle.

Creation by 3 passing points: 1. In the Size topic, select Free Size mode. 2. Uncheck the box Given center. 3. Enter the coordinates of the passing points of the circle.

Creation by Center and Diameter or Radius: 1. 2. 3. 4.

In the Size topic, select Diameter or radius mode. Enter the value of the diameter or the radius. Check Given Center. Enter the coordinates of the center point of the circle.

Creation by Diameter or Radius and 2 passing points: 1. In the Size topic, select Diameter or radius mode. 2. Enter the value of the diameter or the radius.

3. Uncheck the box Given center. 4. Enter the coordinates of the 2 passing points of the circle.

No matter which creation mode is chosen, the circle is created with its center point.

When an element is being created, you can use the Ctrl + Space keys to change input automatically positioned on the last input point.

Additional Information / Modifications: Click the circle or its center point and move your mouse while holding down the left button to modify the position of the circle. From the popup menu you can: Constrain the center of the circle on an element with the Define center... command. When the center point no longer exists, recreate the center point of the circle with the command Create center. When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are

Rectangle Links / Videos:

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A rectangle is created either by entering the coordinates of the rectangle diagonal points in the dialog panel, or directly from the graphics zone by locating two points on the grid or on elements.

Creation Stages: Click on the icon down menu.

or choose the command 3D Sketch > Other curves > Rectangle... from the drop

Creation by the dialog panel: Enter the coordinates of the two points of the diagonal of the rectangle. Creation from graphic area: Locate two points on the grid or on elements.

Naturally, you can mix creation modes by indicating, for example, the coordinates of the 1st point of the diagonal in the dialog panel and describing an element to indicate the 2nd point of the diagonal.

After indicating the 1st point of the diagonal, the rectangle appears in dynamic mode with its dimensions and the coordinates of the 2nd point of the diagonal.

When an element is being created, you can use the Ctrl + Space keys to change input planes (toggle XZ then YZ), then the input plan automatically positioned on the last input point.

Modifications / Additional Information: A rectangle is composed of 4 segments. Each segment can be independently removed or modified independently. Click a segment or a rectangle vertex and move your mouse while holding down the left button to modify the size, position or shape of the rectangle, depending on the constraints that are applied to it: If a rectangle is constrained by 2 dimensional constraints, it will not be possible to move it. If the rectangle is constrained by 4 alignment constraints, it will be possible to modify its size or to move it. If the rectangle is not constrained, it will be possible to modify its size or to transform it into a quadrilateral.

When the mode Automatic dimensions is enabled, the dimensional constraints (driving dimensions) are also t d When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the element is created. The dimensions of the rectangle must be parallel to the axis X and Y of the current input plan of the sketch.

To create a rectangle centered on an axis or the origin of your sketch, you can indicate the first point of your rectangle then move the cursor on the opposite side in relation to the axis or origin, when the centering is detected TopSolid will frame the value of the side with the sign =.

Arc Links / Videos:

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A circle arc is created either by entering the coordinates in the dialog panel, or directly from the graphics zone by locating a point or selecting an element.

Creation Stages: Click the icon or select the 3D sketch > Other curves > Arc... command from the drop-down menu. Creation by Center and 2 passing points: 1. In the Size topic, select Free Size mode. 2. Check Given Center. 3. Enter the coordinates of the center point and the 2 passing points of the circle arc.

Creation by 3 passing points: 1. In the Size topic, select Free Size mode. 2. Uncheck the box Given center. 3. Enter the coordinates of the passing points of the circle arc

Creation by Center and Diameter or Radius: 1. 2. 3. 4.

In the Size topic, select Diameter or radius mode. Enter the value from the diameter or radius of the circle arc. Check Given Center. Enter the coordinates of the center point of the circle arc.

Creation by Diameter or Radius and 2 passing points:

1. 2. 3. 4.

In the Size topic, select Diameter or radius mode. Enter the value from the diameter or radius of the circle arc. Uncheck the box Given center. Enter the coordinates of the 2 passing points of the circle arc.

No matter which creation mode is chosen, the circle arc is created with its center point and its extremity points.

When an element is being created, you can use the Ctrl + Space keys to change input automatically positioned on the last input point.

Available Options: During an arc creation, it is created between the selected points. By checking Complementary it is the complementary arc (to close the circle) which will be created. For example, if the arc is with an angle of 60°, its complementary will be 300°.

Additional Information / Modifications: Displacement of an extremity: Click the end of a circle arc and move your mouse while holding down the left button to modify the opening angle of the circle arc. Displacement of the circle arc: Click the circle arc or its center point and move your mouse while holding down the left button to modify the position of the circle. From the popup menu you can:

Constrain the center of the circle arc on an element with the Define center... command. When the center point no longer exists, recreate it with the command Create center. Create the complimentary arc with the command Complimentary. When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the element is created

Spline Links / Videos:

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The creation of a spline curve is done by indicating the curve's passing points.

Creation Stages / Use: Click on the icon or choose the command 3D Sketch > Other curves > Spline.... from the drop down menu. 1. Select the spline type between Passing points, Control points or Blend: Passing points: The spline passes by each selected point. Control points: The spline is constrained by the selected points.

Passing points

Control point

Blend: allows to create a tangent curve to the two others. By default, the tangents length is equal to 1/3 of the distance between the vertices of the 2 curves. This constraint can be modified with 2 constraints. 2. Position or enter the coordinates of the spline points, or for the blend, select the 2 entities to blend. 3. Validate the spline creation by clicking on .

Options available for the Spline with clearance points: Tense:

A tense spline will be less malleable when it or its interpolation points are moved. There is a popup menu option on a non-tense curve for making it tense. This can cause a change to the geometry of the curve in order to create a more constant curvature.

Closed: Check Closed to create a closed spline curve.

Zero curvature: When this option is checked, it causes a null curvature at the two ends of the spline. These constraints, symbolized by a black circle, can be separately enabled/disabled by a popup menu option near one of the curve.

Options available for the Spline with control points: Closed: Check Closed to create a closed spline curve.

Zero curvature: When this option is checked, it causes a null curvature at the two ends of the spline. These constraints, symbolized by a black circle, can be separately enabled/disabled by a popup menu option near one of the curve.

Options available for the blend: Tense: A tense spline will be less malleable when it or its interpolation points are moved. There is a popup menu option on a non-tense curve for making it tense. This can cause a change to the geometry of the curve in order to create a more constant curvature.

Zero curvature: When this option is checked, it causes a null curvature at the two ends of the spline. These constraints, symbolized by a black circle, can be separately enabled/disabled by a popup menu option near one of the curve.

Additional Information / Modifications: Tangents: Tangents at points of interpolation can be constraints.

To define tangency: Handles (yellow spheres) at the ends of the curve allow tangencies to be defined through the popup menu when creating the curve. After activating the command, select the start or end tangent (line, axis, etc.). When the spline is

validated, constraints between the tangent and referent element will automatically be created.

Show curvature: A popup menu option on a spline makes it possible to view its curvature. The circle symbolizes the area with the greatest curvature.

Curvature circle: A popup menu option on a point of interpolation allows the curvature circle at the point to be displayed and constrained.

Global scaling: Global scaling is triggered when modifying a constraint between two points of interpolation on a large-dimension spline. Displacement By default, the dynamic movement on tangency constraints and interpolation points are local. But using the Alt key on the keyboard during movement

triggers a global modification. (It may sometimes be necessary to authorize such a movement in order to achieve the desired result.)

When an element is being created, you can use the Ctrl + Space keys to change input planes (togg automatically positioned on the last input point.

Spline on shape Links/Videos:

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This command allows to create a spline by using a shape as reference for the points location or as well create a spline by giving the points coordinates.

Creation stages / Use: Click on the icon or choose the command 3D Sketch > Other Curves > Spline On Shape... from the drop down menu. 1. Position or enter passing points coordinates of the spline. It is possible to hook a shape (vertex, plane, face, ...) 2. Validate the creation of the spline curve with the button.

When an element is being created, you can use the Ctrl + Space keys to change input automatically positioned on the last input point.

Available Options: Closed: Check Closed to create a closed spline curve.

The accuracy of the projection of the spline on faces can be set in Options command of the sketch.

Helix Links/Videos:

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This command allows to create a cylindrical or conical helix without created a sketch operation.

Creation stages / Use: Click the icon or select the 3D sketch > Other curves > Helix... command from the drop-down menu. 1. 2. 3. 4. 5. 6. 7. 8. 9. 10.

Select the helix type. (Cylindrical or conical). Enter the cylinder radius or the start radius for a conical helix. Enter the quarter of radial pitch for a conical helix.. For a conical helix, indicate if the cone go inside according to the start radius.(If the end radius is smaller than the start radius, ckeck Go inside). Enter the longitudinal pitch. Indicated if the helix is left handled. Enter the starting angle. Enter the ending angle. Enter the different points in the Frame section. Validate by clicking .

The ending angle must be higher than the starting angle.

Available Options: Frame: By default, the helix is created with the start radius center on the sketch frame. By using this option, select the origin point, a point following the Z direction and a point following the X direction.

Advanced options: Extension: The entered value adds virtual turns on both extremities of the helix. They will allows to drag one of the extremity points to extend the helix. For example, if the entered value is 2 tr, it will be possible to drag one extremity point to add 2 turns and then it will be blocked. The extension is done on both sides.

If the entered value is 2 tr, the dragged extremity point will be blocked after 2 turns. You just have to release it and select it again to be able to drag it two more turns.

Modifications / Additional information: The helix can be edited by a contextual menu, in the graphic area or in the Sketches folder of the entities tree. Its extension can also be modified. The Split contextual command allows to detach the starting point of the helix if it has been merged with the X frame point. The Create frame command allows to create again deleted axes of the helix.

Fillet Links / Videos:

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A fillet is created by entering its radius value and selecting the vertex of a sketch element.

Creation Stages: Click the icon or select the 3D sketch > Fillet... command from the dropdown menu. 1. Enter the radius of the fillet. 2. Select the vertex of a sketch element. Check Keep Vertex to keep the selected point. Fillet with vertex kept

Fillet with vertex not kept

Additional Information / Modifications: A fillet is considered as a circle arc, from the popup menu you can: Constrain the center of the circle arc on an element with the Define center... command.

When the center point no longer exists, recreate the circle arc's center point with the command Create center.

Trim

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The command Trim... allows one or more segments to be cut at the intersection of one or more other segments or sketch planes.

Use: Click the

icon or select the 3D sketch > Trim... command from the drop-down menu.

1. Choose the type of geometry to be modified: Segment Profile

Only the selected segment will be modified. All the sketch elements joined to the selected segment will be modified.

2. Choose the limitation mode: Keep Delete Split

The part of the segment selected is kept, this part is temporarily drawn in a thick full orange line. The part of the segment deleted, this part is temporarily drawn in a thick orange and green dotted line. The segment is split at the intersection point with the intersecting segment.

3. Select the element to be limited.

It is not possible to use the sketch's X, Y and Z axes to limit an element. This command does not allow a sketch segment to be extended.

Available Options: Geometries to be ignored: You can limit this command's field of action by checking the options Construction segments and/or Internal segments, in this case the segments of construction and/or internal type are not taken into account in the limitation calculation. The Isolated vertices option allows not taking into account the points which are on the geometry to be limited and which are not connected to any other geometry. The Planes option allows not taking into account the sketch planes.

Segments removing

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This command allows to remove some segments in a 3D sketch.

Creation Stages / Use: Click the icon or select the 3D sketch > Segment removing... command from the drop-down menu. 1. Select the segments to be deleted. 2. Select a type of heal based on the options defined below. 3. Validate.

Available heal types:

Segments to be deleted are in cyan.

Heal type: None The segments are deleted.

Heal type: Join The segments are deleted and replaced by a segment that connects the two end points.

Heal type: Extend/Limit The segments are deleted, and the remaining segments are extended.

Additional Options for Extend/Limit Healing: These additional options are effective only for extending circular segments. By tangency: Deleted segments are replaced by lines that run tangent to the circular segments having a common point with the deleted segments. (the segment to delete in blue and the preview of the result in orange).

By Curvature: Deleted segments are replaced by the extended circular segments that had a common point with the deleted segments. (the segment to delete in blue and the preview of the result in orange).

The DEL keyboard can also be used to remove selected segments. In this case, the type of heal is None.

Edge copy Links / Videos:

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This command copies a curve, edge, profile, loop, border edges of a surface shape, or all edges of a shape.

Creation Stages / Use: Click on the icon or choose the command 3D Sketch > Edges Copy... from the drop down menu. 1. Select the type from the drop-down list. (description below). 2. Select the entities to group together. 3. Validate the edge copy with the button.

If the copied edge is based on a geometry that has minor discontinuities, the copy will automatically generate a sewn sketch to fill the holes. The same is true for edges with near tangencies; the copy will automatically create a tangency constraint between them. It results in a possible geometry difference between the reference edge and the resulting sketch. This automatic cleaning may sometimes take time. You can interrupt the copy with the Esc key.

Available Types: All Border Edges: Allows border edges to be copied. The edges that delimit a surface

are its border edges. A volume shape does not have any border edges.

All Shape Edges: Allows you to copy all edges of a shape.

Edges or curves: Allows edges from a shape or curves to be copied.

Path between two edges: Allows to copy an edge path by selecting a start and end edge. Angle mode: all tangent edges (or inside the given angle tolerance limit) between the two selected edges will be copied. Border mode: all bounder edges between the two selected edges will be copied. The is not tangency criterion in this mode.

Path around faces: Allows to get the contour of several faces The selected faces (in blue)

The resulting contour (in black)

Profiles or loops: Allows sketches or loops (contour of a surface of the shape) to be copied.

Intersect Links / Videos :

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This command allows to produce the intersection curve between faces and a sketch plane

Creation stages / Use: Click the icon or select the 3D Sketch > Intersect... command from the drop-down menu. 1. Select the plane. 2. Select faces. 3. Validate by clicking

.

An intersection constraint is created between the plane, the face and the segment.

3D sketch - Profile Links/Videos:

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If a sketch is created with the sewing manual mode (option available in 2D or 3D sketch > Options...), this command allows to transform a batch of segments to profile. This can be used in an extrusion, trim, etc.

Creation stages / Use: Click the icon or select the 3D sketch > Profile... command from the drop-down menu. 1. Select the different segments. 2. Validate by clicking .

Selected segments are highlighted.

If the command is grayed, the sewing mode is set to automatic (option is available in 2D or 3D sketch > Options...).

Block Links/Videos:

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This command allows you to create a block-based construction support. This command is very useful for creating a piping line for example.

Creation Stages / Use: Click on the icon or choose the command 3D Sketch > Block... from the drop down menu. 1. Click or enter the X, Y, Z coordinates of the first point. 2. Click or enter the X, Y, Z coordinates of the second point. 3. Validate by clicking

The lines created are construction lines. They are only used as support. Block dimensions can be centered on a point or a plan by using contextual menu.

Example of a block for a piping line creation.(1. starting point - 2. ending point).

Deformation Links / Videos:

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This command allows a segment to be transformed into a circle arc.

Creation Stages / Use: Click on the icon or choose the command 3D Sketch > Deformation... from the drop down menu. This command does not have a dialog panel, select the line to be transformed into a circle and move the cursor keeping the left mouse button pressed down then release the button when the desired circle arc is obtained.

This command does not allow the reverse transformation to be made (transformation of an arc into a line). Depending on the constraints applied on the segment, deformation is not always possible, for example, it is not possible to deform a segment with an alignment constraint.

3D sketch - Constraint

The Constraint... command creates dimensional constraints (driving dimensions) or relations between the elements of the document.

Creation Stages / Use: Click the icon or select the 3D sketch > Constraint... command from the drop-down menu. This command does not have a dialog panel, TopSolid will propose different types of possible dimensioning (linear, angular, radial or diametral) depending on the element(s) selected.

To create a dimension centered on an axis, before putting in your dimension, choose the command Centered Dimension from the popup menu that displays by right-clicking, then select an axis.

Modifications / Additional information: The value of a dimension is modified by double-clicking on the text of the dimension when no command has been launched (neutral mode) or when the command Constraint is launched. The type of extremity of a dimension depends on the selected element: the selection of an extremity of an element creates a dimension with a point type extremity and the selecting of an element creates a dimension with an arrow type extremity.

As the dimensions and constraints are created, TopSolid changes the color of the sketch elements in order to indicate whether they are fully constrained. An under constrained element is displayed in magenta, a completely constrained element is displayed in blue. The same is true for the dimensions. When an over-constrained dimension is detected, TopSolid automatically disables the dimension being created and displays it in gray. The commands Enable and Disable in the popup menu of a dimension allow the types of dimensions to be modified. In case of over-constraint, the dimensions or relations in question are displayed in red. Ask dimension value mode allows you to modify the dimension value just after having created it.

Perpendicularity relation Links / Videos:

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This relation allows an element to be positioned perpendicularly to another.

Creation Stages / Use: Click the icon or select the 3D sketch > Relations > Perpendicularity... command from the drop-down menu. Select the two elements to be made perpendicular: the two elements are moved and the Perpendicularity symbol is displayed between the two elements.

To delete the Perpendicularity relation, you must select the Perpendicularity symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the

Tangency relation Links / Videos:

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This relation allows an element to be positioned in tangency on another.

Creation Stages / Use: Click the icon or select the 3D sketch > Relations > Tangency... command from the drop-down menu.

1. Select the two elements to be made tangent: the two elements are moved and the Tangency symbol is displayed between the two elements. 2. In some cases, it is also needed to select a tangency point. For example to add a tangency between two splines. In this case, the filed is automatically ungrayed. In the common case of a tangency between a line and an arc, it isn't needed and stays grayed.

To delete the Tangency relation, you must select the Tangency symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the selection of a sketch element or as the You can quickly create a tangency constraint between a line and an arc by selecting the line or arc close to the tangency point then displacing it until the display of the tangency symbol is obtained.

Orientation along an axis relation Links / Videos:

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This relation renders a line horizontal or vertical along the closest X, Y, or Z axis.

Creation Stages / Use: Click the icon or select the 3D sketch > Relations > Orientation along an axis... command from the drop-down menu. Select a line to render horizontal or vertical: The line is pivoted towards the horizontal or the vertical of the closest X, Y or Z axis and the Orientation along an axis symbol is displayed in its middle.

To delete the Orientation relation, you must select the Orientation symbol and then press the Delete key on your keyboard or choose the Delete command from the popup menu displayed by rightclicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are A 45° or -45° line will be pivoted vertically whereas a 135° or -135°

line will be pivoted horizontally. The first creation point of a line is used as the pivot center except if another constraint prevents movement of the other extremity of the line.

Orientation along a plane relation Links / Videos:

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This relation constrains an element in the closest XY, XZ, or YZ plane.

Click thee icon or select the 3D sketch > Relations > Orientation along a plane... command from the drop-down menu. Select the element to constrain: the element is moved in the closest XY, XZ or YZ and the Orientation along a plane symbol is displayed in its middle.

To delete the Orientation relation, you must select the Orientation symbol and then press the Delete key on your keyboard or choose the Delete command from the popup menu displayed by rightclicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are

Alignment Relation Links / Videos:

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This relation allows two points to be aligned horizontally or vertically.

Creation Stages / Use: Click on the icon or choose the command 3D Sketch > Relations > Alignment.... from the drop down menu. Select the two points to align: the two points are moved towards the closest horizontal or vertical and the Alignment symbol is displayed in the middle of the two points.

To delete the Alignment relation, you must select the Alignment symbol, then press the Del key on your keyboard or choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the

Align Links / Videos:

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This relation allows a batch of points to be aligned horizontally or vertically.

Creation Stages / Use: This command is available in contextual menu only. At the neutral point, during the sketch edition, select a batch of vertices and using a right-click to display the contextual menu select the Align command. Points are moved to the nearest horizontal or vertical and Alignment symbol are displayed between these points. If n vertices are selected, the command creates at most n-1 alignment relation.

To delete the Alignment relation, you must select the Alignment symbol, then press the Del key on your keyboard or choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the

Coincidence relation Links / Videos:

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This relation allows an element to be positioned on another.

Creation Stages / Use: Click on the icon or choose the command 3D Sketch > Relations > Coincidence... from the drop down menu. Select the two elements to be made to coincide: the two elements are moved and the Coincidence symbol is displayed between the two elements. Elements selected Two points A point and a line, an arc, a circle or an edge. Two lines

Result The points are superposed. The point is placed on the element or in its extension. The lines are placed collinearly.

To delete the Coincidence relation, you must select the Coincidence symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information:

When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the

Centering relation Links / Videos:

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This relationship can center two elements with respect to a point or a plane.

Creation Stages / Use: Click the icon or select the 3D sketch > Relations > Centering... command from the drop-down menu. Select the two elements to center, the centering point or plane, and place the Centering symbol. The two elements are moved at equal distances in relation to the centering point or plane and the Centering symbol displays between the two elements.

To delete the Centering relation, you must select the Centering symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Parallelism relation Links / Videos:

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This relation allows two lines to be made parallel.

Creation Stages / Use: Click the icon or select the 3D sketch > Relations > Parallelism... command from the drop-down menu. Select the two lines to make parallel and then place the Parallelism symbol: the two lines are moved and the Parallelism symbol is displayed between the two lines.

To delete the Parallelism relation, you must select the Parallelism symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional information: When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are automatically created during the

3D sketch - Intersection Links / Videos:

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This relation allows you to constraint an edge on the intersection of 2 curves.

Creation Stages / Use: Click on the icon or choose the command 3D Sketch > Relations > Intersection.... from the drop down menu. 1. Select the first curve. 2. Select the second curve. 3. Select an edge on the first curve. The first curve will be constraint on the intersection of the second curve on this edge. 4. Validate.

The intersection function creates a sketch operation. The point is moved at the intersection of the two elements and the Intersection symbol is also displayed at the intersection of the two elements. To delete the Intersection relation, you must select the Intersection symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Modifications / Additional Information:

When the mode Automatic relations is enable, the tangency and coincidence alignment constraints are

Equality Links / Videos:

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This relation allows the length of several lines to be made equal.

Creation Stages / Use: Click the icon or select the 3D sketch > Relations > Equality... command from the drop-down menu. 1. Select the line to be made equal. 2. Validate the Equality relation with the

button.

The lengths of the lines are modified and an Equality symbol is displayed in the middle of each line.

To delete the Equality relation, you must select the Equality symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by right-clicking.

Fixity relation Links / Videos:

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This relationship allows a sketch entity to be fixed.

Creation Stages / Use: Click the icon or select the 3D sketch > Relations > Fixed... command from the drop-down menu. Select the sketch entity to be fixed. The entity will change to black and will no longer be able to move.

To delete the fixity relation, you must select the Fixity symbol then press the Del key on your keyboard and choose the command Delete from the popup menu displayed by rightclicking. It is also possible to use the Remove fixity popup command. In order to clarify the entities tree, fixity constraint symbols are not displayed in the sketch constraints folder.

Contact with shape relation Links/Videos:

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This command allows to add a contact relation between a point from a 3D sketch and a shape. Thus you can create a point into a 3D sketch, and add this relation so the point always remains in contact with all the face of a shape.

Creation stages / Use: Click on the icon or choose the command 3D Sketch > Relation > Contact with shape... from the drop down menu. 1. Select the geometry (the point). 2. Select the shape. 3. Validate by clicking .

When the point is constrained, it is circled in black.

If you need to move dynamically this point on the shape, it is best to swap to 4 views display so you can visualize and control better the displacement. When a Spline is created by selecting points on faces, this relation is automatically created on each point, and the spline is as well automatically projected onto the faces of the shape. If relations are deleted (deletion of the black circle around the point), it is possible to create again this contact on shape, but it will have to be made point by point. Moreover, in this case, the spline will not be

projected anymore on the face of the shape, so the result may not be exactly the needed one. In the case it is necessary to constrain again some points of the spline, you should first select the spline then select the point. Thus the spline tangency on this point will fits with the point tangency with the face.

Point Links / Videos:

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This command allows you to create an offset point from a point of the sketch.

Creation Stages / Use: Choose the command 3D Sketch > Operations > Point... from the drop down menu. 1. Select the reference point. 2. Enter the offset values in X, Y and in Z.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Line Links / Videos:

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This command allows you to create a line from two points (vertices) of the sketch. It will be in particular used to complete (close) the elements created by sketch operations so as for example to obtain a closed contour allowing a solid to be built during an extrusion.

Creation stages / Use: Choose the command 3D Sketch > Operations > Line... from the drop down menu then select the start and end points.

1. Select the start and the end point. 2. Validate.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Edge copy Links / Videos:

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This command copies a curve, edge, profile, loop, border edges of a surface shape or all edge of a shape. It is especially useful for completing (closing) elements created by sketch operations.

Creation Stages / Use: Click on the icon or choose the command 3D Sketch > Operations > Edges copy... from the drop down menu. 1. Select the type from the drop-down list. (description below). 2. Select the entities to group together. 3. Validate the edge copy with the button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element nor used as a limitation to the sketch element.

Available Types: All Border Edges: Allows border edges to be copied. The edges that delimit a surface are its border edges. A volume shape does not have any border edges.

All Shape Edges: Allows you to copy all edges of a shape.

Edges or curves: Allows edges from a shape or curves to be copied.

Path between two edges: Allows to copy an edge path by selecting a start and end edge. Angle mode: all tangent edges (or inside the given angle tolerance limit) between the two selected edges will be copied. Border mode: all bounder edges between the two selected edges will be copied. The is not tangency criterion in this mode.

Path around faces:

Allows to get the contour of several faces The selected faces (in blue)

The resulting contour (in black)

Profiles or loops: Allows sketches or loops (contour of a surface of the shape) to be copied.

Available Options:

Adjustment: During the operation, the resulting curves may be separate. They are automatically adjusted and sewed together is their tolerance match with the given tolerance. Check this option to modify the adjustment tolerance.

Isocline Links/Videos:

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This command allows to create curves that define the isoclines of a shape or several faces along a given direction.

Creation stages / Use: Click the menu.

icon or select the 3D sketch > Operations > Isocline... command from the drop-down

1. Select the direction. 2. Enter the angle with the normal.

Influence of the angle on the isoclines curves. The arrows shows the direction. The angle is given according to the 90°between the normal and the direction.

3. Choose if you want to get the isoclines from a shape or from a selection of faces. Shape. All the shape is selected. Faces: You can manually select the faces to take in consideration.

4. Validate the isoclines creation with

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element n The planar faces do not generate isoclines.

Available Options:

Adjustment: During the operation, the resulting curves may be separate. They are automatically adjusted and sewed together is their tolerance match with the given tolerance. Check this option to modify the adjustment tolerance.

Silhouette Links / Videos:

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This command allows to create curves that define the silhouette of a shape along a specific direction

Creation Stages / Use: Click on the icon down menu.

or choose the command 3D Sketch > Operations > Silhouette... from the drop

1. Select the shape. 2. Select the direction. 3. Validate the silhouette with the

button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch elemen The Tolerance contextual command allows to modify this approximation. The planar faces do not generate silhouette.

Additional information: Preview: When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Projection

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This command projects a curve, edge, profile, or loop onto a face or all faces in a shape.

Creation Stages / Use: Click on the icon menu.

or choose the command 3D Sketch > Operations > Project... from the drop down

1. Select the element type to project, choose to project curves/edges or to project profiles/loops. 2. Select the elements to project. 3. Choose the projection direction. Either normal to the destination faces or specified. 4. Select the projection type. Choose For projection onto a shape for projection onto faces. If the type is Shape, the projection will be done on all faces of the shape in the given direction. If the type is Faces, the projection will be done only onto the selected faces. 5. Validate creation of the projected elements with the button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch elemen The Tolerance contextual command allows to modify this approximation. Invisible coincidence constraints are created between the selected elements and the created elements.

Available Options:

Adjustment: During the operation, the resulting curves may be separate. They are automatically adjusted and sewed together is their tolerance match with the given tolerance. Check this option to modify the adjustment tolerance.

Intersection Links / Videos:

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This command allows you to create intersection curves between shapes and sets of faces.

Creation Stages / Use: Choose the command 3D Sketch > Operations > Intersection... from the drop down menu. 1. Select the first shape, batch of faces or profiles to intersect : Allows to select a shape. The intersection can be calculated between this shape and another one or a batch of faces. Allows to select a batch of faces. The intersection can be calculated between this batch of faces and another one or a shape. Allows to create an intersection profile between two extruded profiles following entered directions.(the extrusion is hidden). 1. Select the first profile. 2. Select the first direction of projection. 3. Select the second profile. 4. Select the second direction of projection.

2. Then select the second shape or batch of faces to intersect (except if projected profile has been selected): Allows you to select a shape. Allows you to select a batch of faces.

3. Validate creation of the projected elements with the

button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element n The Tolerance contextual command allows to modify this approximation.

Available Options:

Adjustment: During the operation, the resulting curves may be separate. They are automatically adjusted and sewed together is their tolerance match with the given tolerance. Check this option to modify the adjustment tolerance.

Isoparametric Links / Videos:

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This command allows you to create isoparametric curves in a face's U and V directions.

Creation Stages / Use: Choose the command 3D Sketch > Operations > Isoparametric... from the drop down menu. 1. Select the face on which you would like to create isoparametric curves. 2. Select the calculation mode for the isoparametric curves: By parameter : allows to create U or V isoparametric curves by entering parameters following u or V direction of the surface. Values are between 0 and 1. Also enter the total number of isoparametrics following this direction. By point : allows to create U and V isoparametric curves from a point on the face. This point can also be projected on this face by checking the Projection direction option and by selecting this direction.

3. Validate the creation of isoparametric curves with the

button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Available Options: Restrained mode limits isoparametric curves to restriction curves on the exterior of the surface.

Restrained mode unchecked

Restrained mode checked

Offset on shape Links/Videos:

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This command allows you to create the offset of a profile along a surface.

Creation stages / Use: Click the icon or select the 3D sketch > Operations > Offset on shape... command from the dropdown menu. 1. 2. 3. 4. 5.

Select the profile. Select the shape. Enter the plane's offset distance. Check Reverse or click the arrow, if necessary. Validate by clicking .

You can select profiles or profiles on path. The distance indicated corresponds to the distance of the section from the selected profile to the calculated parallel profile. The command can produce the parallel profile even if the carrier faces contain holes as long as the profile only affects one face.

The profile must be continuous in tangency.

Available Options:

Adjustment: During the operation, the resulting curves may be separate. They are automatically adjusted and sewed together is their tolerance match with the given tolerance. Check this option to modify the adjustment tolerance.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element n The Tolerance contextual command allows to modify this approximation.

Offset Normal to Shape Links / Videos :

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This command allows to create an offset profile along the face normal according to given distance and angle.

Creation stages / Use: Click the icon or select the 3D Sketch > Operations > Offset Normal to Shape... command from the drop-down menu. 1. 2. 3. 4.

Select the profile to offset. Select the face to use for the normal direction. Enter the distance. Validate by clicking .

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element n The Tolerance contextual command allows to modify this approximation.

Example of offset profile normal to shape

Available options:

Extend to tangent faces: This options allows to use tangent neighboring faces of selected face.

Angle: This options allows to give an angle in addition to the distance to create the offset profile.

Offset with 0°

Offset with 45°

Middle curve

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This command allows to create the middle curve of two other curves or edges into a 3D sketch through a sketch operation.

Creation stages / Use: Click the icon or select the 3D sketch > Operations > Middle... command from the drop-down menu. 1. 2. 3. 4. 5.

Select the first profile or edge. Select the second profile or edge. Select the type of synchronization. Select the correspondence. Validate.

To Calculate the middle curve, TopSolid match together a succession of points on each curve the calculate the middles points of each pairs and then draw a curve through these middle points.

Available Options: Synchronization: The synchronization allows to define the way TopSolid make the curves match each other. You can choose 3 modes: Free Arc Length: When you use the arc length synchronization, the correspondence between the curves is made proportionally to their length. Local: When using this mode, TopSolid tries to make in correspondence the natural curve parameters.

Offset Links / Videos :

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This command allows to create an offset from a 3D profile.

Creation stages / Use: Click the icon or select the 3D Sketch > Operations > Offset... command from the drop-down menu. 1. 2. 3. 4.

Select the profile. Specify the vertical direction. Enter the offset distance. Validate with the button.

Offset profile with Z as vertical direction

Helix

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This command allows you to create a helix or a spiral.

Creation Stages / Use: Select the 3D sketch > Operations > Helix... command from the drop-down menu. 1. Select the Frame for creating the helix/spiral. 2. Enter the value of the start radius of the helix/spiral. 3. Enter the value of the radial pitch of the helix/spiral (this value must be null in the case of a right helix). 4. Enter the value of the longitudinal pitch of the helix/spiral (this value must be null in the case of a flat spiral). 5. Enter the minimum number of turns of the helix/spiral. 6. Enter the maximum number of turns of the helix/spiral. 7. Validate the creation of the helix/spiral with the button.

Available Options: Invert Z: By default, the helix is created along the Z + axis of the selected frame, this option allows you to create the helix along the Z- axis. Invert Z option unchecked

Invert Z option checked

Go inside: In the case of a spiral, the radial pitch is applied by default towards the exterior of the spiral, this option allows you to apply the pitch towards the interior of the spiral so that the spiral is re-centered toward its creation axis. Left handled: This option inverts the direction of travel of the sketch (right pitch or left pitch).

Additional Information / Modifications:

Click the yellow handles to quickly and dynamically modify the radius and pitches of the helix/spiral or double-click the labels to enter the values of the radius and pitches of your helix/spiral: 1. longitudinal pitch 2. radial pitch 3. starting radius

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Rolling up

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This command rolls patterns around cylindrical or conical faces.

Creation Stages / Use: Click on the icon down menu.

or choose the command 3D Sketch > Operations > Rolling Up... from the drop

1. 2. 3. 4. 5.

Select the profiles to roll. Choose the profile's point of origin. Select the Y axis of the profile. Select the axial frame on the cylindrical or conical face to position the rolled up profile. Select Cylindrical or conical face to roll up around this face and select Radius to enter the rolling up radius. 6. Select a rolling up mode on cone. Sketch (text as profile mode) to roll up.

Projected conical rolling up Keeps lengths and angles, corresponds to a real rolling up. This is a real rolling operation. If you want to have a “proper” rolled result, you have to draw your planar profile as it would be unrolled.

Circular conical rolling up

Keeps only lengths. With this option, if you want to have a “proper” rolled result, you have to draw your planar profile as consider that the unrolling area is a triangle.

In each cases, the sketch is positioned according to the cone radius, at the center of the selected axial frame.

7. Validate by clicking the

button.

TopSolid considers again the profile to roll up regarding the selected origin point which will become the center of the sketch's frame according to the y axis of the profile. Then this profile, positioned in its new frame (according to the chosen center and the y axis), will be positioned on the axial frame at the intersection of the x axis of the frame and the cylinder or cone, in tangency with it, the y axis in the direction of the z axis of the frame.

Available Options: Adjustment: During the operation, the resulting curves may be separate. They will be automatically adjusted and sewed together if their distance is in the entered tolerance. Check this option to modify the adjustment tolerance.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element no

The Tolerance contextual command allows to modify this approximation.

Curve by formula

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This command allows you to create a 3D curve by providing its Cartesian equations.

Creation Stages / Use: Choose the command 3D Sketch > Operation > Curve by formula... from the drop down menu. 1. Enter the formulas along the X, Y and Z axes of your curve. 2. Enter the minimum and maximum intervals of parameter t.

It is important to systematically specify the unit of the values entered in the expressions. Whereas the parameter t does not have to have a unit

This command does not manage the curves that are not continuous in tangency. So it is necessary to check that the provided formulas properly generate a G1 type curve within the given interval.

Available Options: Tolerance: The curve obtained is an approximation of the true curve by a B-spline curve generated at the tolerance given this option allows you to refine the curve obtained

Examples : Helix Equations X(t) : 120mm*sin(360°*t) Y(t) : 120mm*cos(360°*t) Z(t) : 20mm*t Minimum : 0 Maximum : 5

Curve

Helix with changing pitch Equations X(t) : 120mm*sin(360°*t) Y(t) : 120mm*cos(360°*t) Z(t) : 20mm*t*t Minimum : 0 Maximum : 5

Curve

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Repetition Links / Videos:

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This command allows the repeat (duplicate with associativity) an element from a 3D sketch according to a given pattern.

Creation stages / Use: Choose the command 3D Sketch > Operations > Repetition... from the drop down menu. 1. Select the profile to repeat. 2. Define the pattern to be applied and its parametering.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Available Options: Join methods: This option allows you to choose the type of join between the instances of the pattern: Type None

Straight

Definition The repetition's elements are not joined.

Example

The repetition's elements are joined by a line.

Additional Information / Modifications: Modify the repetition from the operations tree, select your sketch, then right-click on the repetition and choose Edit from the popup menu.

Fillet

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This command allows you to create a fillet on the vertex of a sketch.

Creation Stages: Choose the command 3D Sketch > Operation > Fillet... from the drop down menu. 1. Enter the radius of the fillet. 2. Select the vertex of a sketch element.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Extension Links / Videos:

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This command allows you to extend a profile.

Creation Stages / Use: Click the icon or select the 3D sketch > Operations > Extension... command from the drop-down menu. 1. Select the profile to extend. 2. Select whether it is the start or the end of the profile that is to be extended. 3. Validate with the button.

The Tolerance contextual command allows to modify this app

Available Types:

Curvature:

The curvature radius of the curve is constant.

Tangent:

The segment is tangent to the curve.

Exact :

The extension follows the probable evolution of the curve based on its last points (takes into account the curvature and the

Trim

This command allows a profile to be cut or shared at the intersection with another entity (profile point, face, plane, or at a certain distance).

Use: Click on the icon or choose the command 3D Sketch > Operations > Trimming... from the drop down menu. 1. Select the profile to trim or share. 2. Choose the trimming entity: Point Profile Length Face Plane

Select the point that will trim the profile. The point must be on the profile. Select the profile that will trim the profile. The two profiles must intersect at a point. Enter the length at which the profile will be trimmed or shared. The length is the distance from the profile's point of origin. Select the face from a shape that will trim the profile. The profile must cross this face. Select the plane that will trim the profile. The plane is considered to be infinite.

3. Check Invert if necessary. The preview represents the kept portion. 4. Check Share if necessary. The profile will be cut in two, but the two parts will remain available. 5. If the trimming must be done on both sides of the profile (the profile will be segmented into three parts), check Second trimming. 6. Choose the second trimming entity: Point Profile Length Face

Select the point that will trim the profile. The point must be on the profile. Select the profile that will trim the profile. The two profiles must intersect at a point. Enter the length at which the profile will be trimmed or shared. The length is the distance from the profile's point of origin. Select the face from a shape that will trim the profile. The profile

Plane

7. Validate by clicking

must cross this face. Select the plane that will trim the profile. The plane is considered to be infinite.

.

The point, profile, or trimming face must intersect the profile. The preview represents the kept portion. If the portion to save is on the bad side, use the Invert option.

Fitting Links / Videos:

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This command is used to fit and sew the selected profiles between them, if their distance is within the specified tolerance.

Creation Stages / Use: Click the menu.

icon or select the 3D sketch > Operations > Fitting... command from the drop-down

1. Select the profiles to adjust. 2. Enter the adjustment tolerance. It is the distance in which must be extremities points of profiles to fit. 3. Validate with the button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

Blend Links / Videos:

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This command can join two segments by a fillet or a spline.

Creation Stages / Use: Click on the icon menu.

or choose the command 3D Sketch > Operations > Blend... from the drop down

1. Select the first element. 2. Select the second element. 3. Select the blend type.. Fillet: Creates a radius between the two segments, based on the entered value. The two segments must be contiguous. The fillet is tangent to the two segments. Enter the radius.

Link Creates a connective curve between the two discontinuous segments. The curve starts and ends at the segments end points. The tangent value influences the connection curvature. Enter the tangency values. Click Reverse or on the yellow arrow to reverse the tangency side.

4. Validate the creation of the blend with the

button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch eleme The Tolerance contextual command allows to modify this approximation.

Available Options: First reference point: The reference point indicates the side of the first segment where the join will be.

Second reference point: The reference point indicates the side of the second segment where the join will be.

Smoothing Links / Videos:

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This command is used to obtain a smooth curve by creating point on the curve and rebuilding by passing over the points to get a continuous curve in tangent.

Creation Stages / Use: Click on the icon drop down menu.

or choose the command 2D or 3D Sketch > Operations > Smoothing... from the

1. Select the profiles to smooth. 2. Select the smooth type.. Local: The smoothing will be done segment by segment, based on the entered angular tolerance. If the angle between the two profiles is less than the entered value, the two profiles will be rounded at their intersection. If the angle between the two profiles is greater, the sharp angle will be preserved. Global: The smoothing will be global for the entire sketch. The more interpolation points there are, the closer the curve will be to the initial sketch. There will no longer be sharp angle between the segments. By tolerances: The smoothing of a Bspline will be done regarding the entered linear and angular tolerances. The linear tolerance is the maximum distance between a point of the Bspline to smooth and its equivalent on the smoothed curve. The angular tolerance is the maximum angle between the tangent of a point of the Bspline to smooth and the tangent of its equivalent on the smoothed curve.

3. Validate with the

button.

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch elemen The Tolerance contextual command allows to modify this approximation.

Available Options: Local : Angular tolerance: The curve is smoothed by created points on the curve and rebuilding by going back over the points according to a specified angular tolerance in order to get a continuous curve in tangent. If the angle between the two profiles is less than the entered value, the two profiles will be rounded at their intersection. If the angle between the two profiles is greater, the sharp angle will be preserved. Select Point Influence or Distributed Influence. These options, which are to be used on poor quality curves, can soften the curvature. With Point Influence, the point closes to the

intersection can be moved. With Distributed Influence, the entered distance will indicate the distance on which the control points will be able to be moved to gradually soften the curvature.

In black: Two splines are not smooth. In green: The result of the smoothing with point influence. In orange: The result of the smoothing with distributed influence Note: The angular tolerance has been increased (80°) so that no sharp angles remain.

Global : Number of interpolation points: Number of passage points defining the smooth curve. The higher this number, the closer the curve will be to the initial curve. However, the processing time may be much longer.

Sketch without smoothing

Number of interpolations: 20

Number of interpolations: 100

Segments removing Links / Videos:

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This command allows to remove some segments in a 3D sketch with a sketch operation.

Creation Stages / Use: Click the icon or select the 3D sketch > Operations > Segment removing... command from the drop-down menu. 1. Select the segments to be deleted. 2. Select a type of heal based on the options defined below. 3. Validate.

Available heal types:

Segments to be deleted are in cyan.

Heal type: None The segments are deleted.

Heal type: Join The segments are deleted and replaced by a segment that connects the two end points.

Heal type: Extend/Limit The segments are deleted, and the remaining segments are extended.

Additional Options for Extend/Limit Healing: These additional options are effective only for extending circular segments. By tangency: Deleted segments are replaced by lines that run tangent to the circular segments having a common point with the deleted segments. (the segment to delete in blue and the preview of the result in orange).

By Curvature: Deleted segments are replaced by the extended circular segments that had a common point with the deleted segments. (the segment to delete in blue and the preview of the result in orange).

Split Segment

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This command allows to divide a segment in two segments.

Creation stages / Use: Select the 3D Sketch > Operations > Split Segment... command from the drop-down menu. Select the segment to split and give the division point.

When the point is outside the segment, it is projected perpendicularly on the segment. A command with the same name is also available in the 3D Sketch > Operations menu.

Profile Origin and Orientation

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This command allows to modify the origin and the direction of a profile.

Creation stages / Use: Select the 3D Sketch > Operations > Profile Origin and Orientation... command from the drop-down menu. When the profile has been selected, TopSolid displays a circle at the origin of the profile and also a blue arrow which shows the direction of the profile. Then you can: check the Origin option and give the new origin of the profile. check the Reverse option in order to revert the direction of the profile. double-click on the arrow in order to revert the direction of the profile.

The new origin point must belong to the profile. If needed, a point can be added by spliting a segment. This modification is an operation, it is not visible in the sketch edition. A command with the same name is also available in the 3D Sketch > Operations menu.

Profile Links/Videos:

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If a sketch is created with the sewing manual mode (option available in 2D or 3D sketch > Options...), this command allows to transform a batch of segments to profile.This can be used in an extrusion, trim, etc.

Creation stages / Use: Click the menu.

icon or select the 3D sketch > Operations > Profile... command from the drop-down

1. Select the different segments. 2. Validate by clicking .

The element thus created is an operation, its updating is carried out after solving the sketch. This element is not therefore visible during editing the sketch and cannot be limited by a sketch element The Tolerance contextual command allows to modify this approximation.

If the command is grayed, it is because the sewing mode is set to automatic (available option in 2D or 3D sketch > Options...).

Selected segments are highlighted.

Rolling Up Wizard Links / Videos :

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This command allows to unroll a profile or a face on a plane, modify it and then roll it up at the same location. It combines the unrolling and rolling up commands.

Creation stages / Use: Click the icon or select the 3D Sketch > Operations > Rolling Up Wizard... command from the drop-down menu. 1. Choose a mode: Profile: Allows to unroll a profil rolled up on a cylindrical face in order to modify it and roll it up again o cylindrical face. Face: Allows to get the unrolled borders of a cylindrical face in order to modify it and roll it up again on cylindrical face. Free: Allows to create a sketch on the bulk of a unrolled cylindrical face (virtual or existing) and roll it o cylindrical face.

2. Select the profile or the reference face. 3. Select the revolution axis 4. Confirm with the

Exemple: Face mode:

Free mode:

Step 1: Selection of the face to unroll and the reference point

Step 1: Selection of the face which represent the bulk of the face to unroll and the reference point.

Step 2: The modification sketch is automatically created with the border of the selected face. When this sketch is modified, the segments before modification will be displayed Step 2: Creation of segments in the unrolled sketch. in dashed linetype. In our example, a parallel is created and the border of the unrolled face are switched as construction lines.

Step 3: Result after validation of the modification sketch.

Step 3: Result after validation of the unrolled sketch.

Available options: Reference point: The selected reference point allows to define the origin of the modification sketch (unrolled sketch), the unrolled sketch plan will be tangent to the cylindrical face at the selected point. It must be on the cylindrical face.

Advanced options: Tolerances: Cylindricity: Check the cylindricity of the selected geometries. The curve must be inside 2 theorical cylinders of the same axis with radii different of the given tolerance. Arcs rebuild: Allows to recognize the arcs during the creation of the result. If the curve is inside 2 arcs whose the radius is distant of the given tolerance then the curve is rebuilt as an arc.

Modifications / Additional information: The sketches generated by the operation (unrolled sketch, modification sketch or rolling up sketch) can be directly modified. They can also be modified using the contextual edition commands (Edit, Edit unrolled shetch, Edit preparation sketch).

View sketch from top

This command orients the current view of the sketch to a top view in relation to the sketch frame.

Creation Stages / Use: Click the icon or select the 3D sketch > Visualization > View from top command from the drop-down menu. There is no validation. When using this command, the current view is immediately oriented.

If your document is splitted in several views, only the current view will be modified.

View sketch in perspective

This command orients the current view of the sketch in perspective in relation to the sketch frame.

Creation Stages / Use: Click the icon or select the 3D sketch > Visualization > View sketch in perspective command from the drop-down menu. There is no validation. When using this command, the current view is immediately oriented.

If your document is splitted in several views, only the current view will be modified.

Zoom on sketch

This command allows you to zoom to fit the sketch in the current view.

Creation Stages / Use: Click the icon or select the 3D sketch > Visualization > Zoom on sketch command from the drop-down menu. There is no validation. When using this command, the current view is immediately zoomed.

If your document is splitted in several views, only the current view will be modified.

Show extremities

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This command shows the extremities of the sketch if they are not closed.

Creation Stages / Use: Click the icon or select the 3D sketch > Modes > Show extremities... mode from the drop-down menu.

If the sketch is closed, there is no extremity. This mode allows you to quickly locate where the sketch is open.

Available Options: You can change the color and diameter of the representation in the sketch options.

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This mode allows external geometries (faces, edges, others sketches) to be taken or not to be taken into account during the creation of relations between the sketch's elements.

Creation stages / Use: Click the icon or select the 3D Sketches > Modes > Filter External Geometries... command from the drop-down menu. When this mode is enabled, no external geometry is taken into account during the creation of relations between the sketch's elements. When this mode is disabled, external geometries are taken into account during the creation of relations between the sketch's elements.

When this mode is not enabled, during the creation of a sketch element, passing over a cylindrical face or edge will automatically set off the creation of a coincidence constraint with these elements, which can be annoying in some cases. It is then preferable to disable this mode.

Additional information: This mode is enabled when the icon is pressed (the background remains colored).

3D Sketch options Links / Videos:

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This command allows to modify the sketch behavior by sewing or not profiles together, by verifying or cleaning automatically the sketch, by managing the splines extension of the editing sketch.

Creation stages / Use: Select the 3D sketch > Options... command from the drop-down menu.

Profiles. Allows to manage the profiles sewing. Automatic: Different entities (lines, arcs, splines, ...) are automatically sewed together to create a profile. The result can be extruded. Semi-automatic: Several closed profiles can be sideby-side. The extrusion will always be possible. (see the example below). Manual: Different entities (lines, arcs, splines, ...) are not sewed together to create a profile. This sew operation has to be done manually by using the Profile command. Non sewed profiles are displayed with thin lines, they can be extruded. None: It will not be possible to sew different entities (lines, arcs, splines, ...) to create a profile.

Automatic mode:

Semi-automatic mode:

The profile on the left has The profile on the left has been been added. Its incompatible added. Segments are not dotted. segments with an extrusion The extrusion is not possible. are dotted. The extrusion result will be a surfacic square and a flat surface (extrusion of the line).

Check. Projection.

Allows to specify the accuracy of the curve projection on surface. The more the value is small, the more the result is accurate. This option is only used by the command Spline on Shape.

Planes. Allows to set the size of the planes that could be created selecting a point of a 3D sketch by right click.

Advanced options. The Large radius value is a step at which a circle will be deformed differently during its resolution by the solver. Below this threshold, for a rather short radius, it will not be able to change the sign of curvature and will always remain on the same side of the chord. This curvature sign change can be seen using the deformation command. Otherwise, if the radius becomes to large, it could cross its chord and reverse its curvature.

The large radius option has only to be use for uncommon cases like a radius of several kilometers for railway rails. The default threshold is set to R = 1m which correspond to a diameter of 2m. We highly recommend that you do not change this numerical threshold.

Block

This command allows you to create a rectangle parallelepiped by defining its three lengths and its orientation frame.

Creation Stages / Use: Click the icon or select Shape > Primitives > Block... from the drop-down menu. 1. Enter the values for the lengths X, Y and Z of the block. 2. Define the origin point of the block. 3. Define the reference frame for the orientation of the X, Y and Z axes of the block. 4. Validate by clicking .

The block creation only accepts positive values. A block can't be created following X- Y- and Z- directions

Additional information: You can center the different lengths of the block in relation to the origin point by checking the corresponding check box: Center on X , Center on Y, Center on Z .

Enclosing block

This command allows you to create a block enclosing a selection of entities (points, profiles, shapes, frames, etc.) with the possibility to define margins.

Creation Stages / Use: Click the icon or select Shape > Primitives > Enclosing Block... from the drop-down menu. Select the different elements to enclose.

Available Options: Orientation frame: This command allows you to define the frame used to orient the enclosing block. If this option is unchecked, then the enclosing block is oriented according to the global bulk of the selected elements.

Enclosing block with orientation frame.

Enclosing block without orientation frame. The block is created according to the global bulk of the selected elements to have a block closest to the minimum.

Margins: You have the possibility of adding margins on each side of the enclosing block. If you check the Single margin check box, then the value provided is applied to all the faces.

Although no orientation frame the enclosing block is created to the nearest minimum, it is not possible to guarantee that this block is the smallest possible.

Cylinder

This command allows you to create a cylinder by defining its diameter and its length.

Creation Stages / Use: Click the icon or select Shape > Primitives > Cylinder... from the drop-down menu. 1. Enter the values for the diameter and the length. 2. Select the cylinder origin. 3. Select the cylinder axis direction.

The cylinder creation only accepts positive values. The cylinder may be created following one of the X- Y- or Z- direction by clicking the tilt arrow in front of the selected direction.

Additional information: It is possible to center the cylinder length with its origin by checking Center.

Cylinder 2 points

This command allows you to create a cylinder by defining its diameter and its two extremities.

Creation Stages / Use: Click the icon or select Shape > Primitives > Cylinder 2 points... from the drop-down menu. 1. Enter the value for the diameter. 2. Define the start point of the cylinder. 3. Define the end point.

You are able to create a point "on the fly" by clicking the "+".This point is created in the running command. It will be deleted if the command is canceled.

Enclosing cylinder

This command allows you to create a cylinder enclosing a shape with the possibility to define margins.

Creation Stages / Use: Click the icon or select Shape > Primitives > Enclosing Cylinder... from the drop-down menu. 1. Select the shape to enclose. 2. Define the axis of the enclosing cylinder (orient and position the cylinder along this axis).

This function is very handy for obtaining a rough shape from a revolved shape.

Available Options: Tubes: This option allows to create an enclosing tube. Automatic: the tube is automatically defined regarding the selected shape and axis. Diameter: the tube is defined by manually entering the inner diameter. Thickness: the tube is defined by manually entering the thickness.

Of course, to be able to define an enclosing tube, the shape must have a through all hole on the cylinder axis.

Margins: Margins can be added on the diameter and on each side of the enclosing cylinder. If the tube option is selected, a margin can also be defined on the inner diameter. The Single margin option allows to apply the same value everywhere.

Cone

This command allows you to create a pointed or truncated cone along an axis and an origin point.

Creation Stages / Use: Click the icon or select Shape > Primitives > Cone... from the drop-down menu. 1. Choose the type of cone you wish to create: Truncated 2. 3. 4. 5.

or

Pointed Fill in the different parameters of the cone. Check Center if the height should be centered on the origin. Define the origin point of the cone. Define the axis of the cone.

Available Options: Constraint This option allows you to choose which parameters (in addition to the base diameter) you wish to use to build the cone. For a truncated cone: - Second diameter / Height - Second diameter / Angle - Height / Angle For a pointed cone: - Height - Angle

Modifications: By double-clicking the cone, you can make the driving dimensions appear.

The cone creation only accepts positive values. The cone may be created following one of the X- Y- or Z- direction by clicking the tilt arrow in front of the selected direction.

Additional information: It is possible to center the cone with its origin by checking Center.

2 points cone

This command allows you to create a pointed or truncated cone between two points.

Creation Stages / Use: Click the icon or select Shape > Primitives > 2 Point Cone... from the drop-down menu. 1. Choose the type of cone you wish to create. Truncated

or

Pointed 2. Fill in the different parameters of the cone. 3. Define the starting point of the cone. 4. Define the end point of the cone.

You are able to create a point "on the fly" by clicking the "+".This point is created in the running command. It will be deleted if the command is canceled.

Available Options: Constraint: This option allows you to choose which parameters (in addition to the base diameter) you wish to use to build for the truncated cone: - Second diameter - Angle

Modifications: By double-clicking the cone, you can make the driving dimensions appear.

Sphere

This command allows you to create a sphere by defining its diameter and its center.

Creation Stages / Use: Click the icon or select Shape > Primitives > Sphere... from the drop-down menu. 1. Enter the value for the diameter of the sphere. 2. Define its center point.

Extruded

This command allows to extrude a shape from a planar section.

Creation Stages / Use: Click the icon or select Shape > Extruded... from the drop-down menu (or Modeling > Local Shapes > Extruded in the assembly document). 1. Select the section to be extruded. 2. Define, if need be, the extrusion direction (normal to the profile by default) 3. Define the extrusion limit (see below the available options for the different modes)

The extrusion of a closed section automatically forms a solid extruded shape. If your section is open, you must use the Offset option for a solid extruded shape.

Click on yellow handles to rapidly and dynamically modify the height and draft of your extruded shape. Double-click the labels to enter values for the height and draft of your extruded shape. You are able to create a new sketch "on the fly" by clicking the "+" in the field.

Available Options: Limit: You can define the extrusion limit in several ways: Length: Enter the value for the extrusion height Point: Define a point for the extrusion limit. Plane: Select a trimming plane for the extrusion Center: By checking this option, the operation is mode symmetrically on both side of the section. If you enable this option then the operation limit can only be defined by a length Draft: By checking this box, you will be able to add a draft on all lateral faces of the extruded shape. Offset limit: For limits like Point, Plane, Surface, Face set, Shape, it is possible to add an offset.

Example of an offset limit regarding the surface.

Surface: By checking this box, the result of the extrusion is systematically a surface, even if the profile is planar and closed. Offset: Using this option, you can offset the start of the extrusion by a distance given in relation to the section. The check box Negate allows you to apply the offset in the opposite direction of the extrusion Second Side: This option allows you to extrude at the same time the section in the opposite direction with the trimming mode that you want (see Trim option). You can also apply a separate draft and offset limit to the second side. The result of this double extrusion is one single and same solid. This option is not compatible with the Center option. Offset: This option allows you to obtain a hollow extruded shape open at its extremities. To do this, you can provide a thickness by using one of the following modes: Centered

The entered value is distributed symmetrically to the section.

Outwards

The extruded shape is thickened from the value provided towards the exterior.

Inwards

the extruded shape is thickened from the value provided towards the interior.

On both sides

You can provide two different values for the thickening towards the interior and towards the exterior.

The Rounded joints check box allows you to add fillets on vertical edges of the extruded shape using, as the radius value, the outer thickening value.

Offset:

Fast

Check result

In this mode the profiles are grouped before being extruded. When the sketch to extrude contains a lot of profiles as a grid with holes for example, it allows to get the extruded shape almost instantaneously. In this mode, there shouldn't be any intersection between profiles. This option allows to check whether the profiles to extrude are intersecting, in such case, the extrusion will be forbidden.

Modifications: By double-clicking the extruded shape, you can make the driving dimensions appear.

Extruded Faces

Links / Videos :

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This command allows you to extrude a selection of faces along a direction.

Creation stages / Use: Select the Shape > Extruded Faces... command from the dropdown menu. 1. Choose the faces to extrude. 2. Choose the extrusion direction 3. Enter the extrusion length

The faces should belong to the same shape and must be connected as well. The faces should not be parallele to the extrusion direction.

Example:

Revolved

This command generates a shape by turning a profile about a revolution axis.

Creation Stages / Use: Click the icon or select Shape > Revolved... from the drop-down menu (or Modeling > Local Shapes > Revolved in the assembly document). 1. Select the section to revolve. 2. Select the axis of rotation (by default it is the X axis of the sketch)

Rotating a closed section can automatically result in a solid rotated shape. If your section is open, you must use the Offset option to get a solid rotated shape.

It is possible to create a new section "on the fly" by clicking the "+".

Available Options: Surface: By checking this box, the result of the extrusion is systematically surfacic, even if the profile is planar and closed. Bound: This option allows you to define a partial revolution. You also have the following possibilities: Open: enter here the angular value of revolution Center: By checking this check box, the extrusion is made symmetrically on both sides of the section. Offset: this option offsets the start of the revolution of a given angle in relation to the section. Invert: inverts the revolution direction.

Click on yellow handles to quickly and dynamically modify the revolved shape. Double click on handles to enter a new bounds angle.

Parallelize: This option allows you to obtain a hollow revolved shape open on its extremities. To do this, you can provide a thickness by using the following modes: Centered

the entered value is distributed on both sides of the section.

Outwards

the section is thickened outwards with the entered value.

Inwards

the section is thickened inwards with the entered value.

On both sides

you can enter 2 different values for the outwards and inwards thickening.

The Rounded joins check box allows you to add fillets on the outer circular edges of the revolved shape with, as the radius value, the exterior value thickness.

Pocket

This command allows you to create a pocket on the part having the same shape as the profile used.

Creation Stages / Use: Click the icon or select Shape > Pocket... from the drop-down menu (or Modeling > Local Shapes > Pocket in the assembly document). 1. Select the shape to modify. 2. Select the section to use to generate the pocket. A sketch can be created on the fly by using the "+". 3. Define, if need be, the recess direction of the pocket (normal to the section by default) 4. Define the bound of the bottom of the pocket (see available options for the different available modes)

If the section is opened, you should first use the Offset command before using this command.

Click on yellow handles to dynamically and quickly modify heights and the draft of the pocket. Double click on a handle to enter heights or the draft angle. Click on "+" to be able to create a sketch "on the fly".

Available Options:

Limit: You can define the bottom of the pocket in several ways: Depth: Enter the value for the depth of the pocket, measured in relation to the section. Point: define a point for the bound of the bottom of the pocket. Plane: select a trimming plane of the bottom of the pocket. Surface: select a surface (flat or curve) to trim the pocket bottom. Face set: select a face of the shape to trim the pocket with this face and all its adjacent faces. Shape: Select a shape against which the pocket must be trimmed Through: the pocket traverses through a first thickness of the part in the defined direction. Through all: the pocket traverses the part in its entirety in the defined direction, even if it countersinks a first time in the area without material. Though all on both directions: the pocket traverses the entirety of the part on both sides of the section In place: The section defines the bottom of the pocket that countersinks on the exterior of the part in the defined direction.

Draft: By checking this box, you will be able to add a draft on all lateral faces of the pocket.

Offset limit: For limits like Point, Plane, Surface, Face set, Shape, it is possible to add an offset.

Example of an offset limit regarding the surface.

Through over: This option allows you to make the pocket countersink on the material of the part located above the section. This option should be active when the pocket section is mounted on a portion of the part and the area above it must be removed. By activating this option, TopSolid removes the material found directly above and in contact with the section, until it falls off.

Blends and fillets: Blend: Allows to add a fillet or a chamfer on the upper edge of the pocket. It is the edge between the reference face and the pocket. None: The upper edge has no fillet or chamfer. Chamfer: Enter the value for the both sides of the chamfer.

Fillet: Fillet: Enter the value of the radius. The "rounded corners" check box allows you to obtain a rounded connection between the fillets arriving at a sharp angle.

Fillets: Allows you to add fillets. Bottom Radius: On the edges of the bottom of the pocket. Vertical radius: on the lateral edges of the pocket.

Reference plane: This option allows you to make the pocket on the other planar face, this face must be parallel to the definition plane of the sketch. The depth of the pocket is therefore calculated in relation to the reference plane and not in relation to the sketch. Sketch Pocket Reference plane

Advanced Options:

Fast : When the sketch contains many profiles, the fast mode allows to generate operation almost immediately. This allows for example to produce easily a plate with many holes (one Machining process: This option allows to assign a machining process to the operation. This machining process is recognized by TopSolid'Cam. It can also assign a color to the operation. Entry point : Once the machining process defined, it is possible to activate this option in order to defined entry points positions for this machining. Give the diameter value and select the points to define as entry point positions. The entry points can be displayed/hidden into the graphic area by using the display mode Create MF available in the Edition menu or on the Home Tab icon bar.

Boss

This command allows a boss having the same shape as the profile used to be created on a part.

Creation Stages / Use: Click the

icon or select Shape > Boss... from the drop-down menu.

1. Select the shape to modify. 2. Select the section to use for generating the boss. 3. Define, if need be, the elevation direction of the boss (normal to the section by default) 4. Define the limit of the vertex of the boss (see the available options for the different available modes).

If the profile is open, you should Thicken it to use this command.

Click the yellow handles to rapidly and dynamically modify the height and draft of the boss. Double click the labels to enter the heights and draft values. To create a new sketch "on the fly", click the "+".

Available Options: Limit: You can define the limit of the boss in several ways: Height: enter the value for the height of the boss, measured in relation to the section. Point: define a point for the bound of the bottom of the pocket. Plane: select a trimming plane for the vertex of the boss.

Surface: select a surface (plane or curve) in order to trim the vertex of the boss. Face set: select a face of the shape in order to trim the elevation on this face and all of the faces adjacent to it. Shape: Select a shape against which the boss must be trimmed Through: the boss rises up to the first face of the shape that completely intersects the section of the boss. Through all: the boss rises up to the last face of the shape that completely intersects the section of the boss. Through all in both directions: the boss rises on both sides of the section up to the last face of the shape that completely intersects the section of the boss. In place: The section defines the vertex of the boss.

Center: By checking this option, the operation is mode symmetrically on both side of the section. Draft: By checking this box, you will be able to add a draft on all lateral faces of the boss.

Offset limit: For limits like Point, Plane, Surface, Face set, Shape, it is possible to add an offset.

Example of an offset limit regarding the surface.

Extends below: This option allows you to extend the boss in the opposite direction of the rising of the boss. This option is useful for example when the section of the

boss is not in contact with the start face but is located slightly above.

Blends and fillets: Blend: Blend: Allows you to add a fillet or a chamfer at the base of the boss. None: There is no blend. Chamfer: Enter the value for the two lengths of the chamfer. Fillet: Enter the value of the radius. The "rounded corners" checkbox allows you to obtain a rounded connection between the fillets arriving at a sharp angle.

Fillet blend without rounded corners

Fillet blend with rounded corners

Fillets: Allows you to add fillets. Upper radius: on the edges of the vertex of the boss. Vertical radius: on the lateral edges of the boss.

Reference plane: This option allows to create the boss regarding another plane face of the part. This face must be parallel to the sketch plane. The boss height is calculated regarding the reference plane and not the sketch. In the example below, the Extend option must be checked Sketch Pocket Reference plane

Advanced Options:

Fast : When the sketch contains many profiles, the fast mode allows to generate operation almost immediately. This allows for example to produce easily a plate with many holes (one sketch containing over

Boolean

This function performs Boolean operations among several shapes: union, subtraction, and intersection.

Creation Stages / Use: Click the icon or select Shape> Boolean... from the drop-down menu (or Modeling > Local Shapes > Boolean in the assembly document). 1. Select the shape to modify. 2. Select the type of Boolean operation to perform on this shape:

Original shapes

Union:

Union of the 2 shapes Subtraction:

Substraction of the cylinder Intersection:

Intersection of the 2 shapes

3. Select tool shapes for boolean operation 4. Validate by clicking .

Available Options: Hide: This option allows to hide the selected elements (it can helps to the selection of other shapes that could be hidden by the shapes already selected).

Clearance: When you choose the subtraction mode, you can define a clearance value that will be applied on all the faces of th tool shape. In such case, the tool shape is parallelized with the clearance value in all the direction and this shape subtracted to the shape to modify.

Example of subtraction with

clearance

The Direction to through option allows you to extend the tool according to the given direction:

Example of subtraction with clearance and direction to through along the X axis

Example of subtraction with clearance and direction to through along the Y axis

Example of subtraction with clearance and direction to thro along the Z axis

Fillets: This option allows you to add, on final result, a fillet on every intersection edges between the shape and tools.

Local operation: This option allows you to use only some shape or tool areas. Shape faces: In some case, it is necessary to select some shape to define a boolean operation limitation. In the example below, union of the cylinder with the U will be made regarding U upper face (in green). By including, or excluding a face, edge or vertex from tool (magenta) , result will be different.

Selected shape face (in green) and selected tool edge (in yellow)

Result with mode: Include

Result with mode: Exclude

Tool faces: In some case, it is necessary to select some shape to define a boolean operation limitation. In the example below, the shape is the cylinder (in cyan), the tool is the U (in magenta) and the 2 faces from selected tool are in pink.

Faces from selected tool (in pink)

Result

Faces, edges or vertex from tool to include or exclude: Select tool faces, edges or vertex and choose if they must be included or excluded from boolean operation.

Slot to create on the blue angle by using yellow shape.

Select yellow edge to include to be able to remove the complete tool section on the other side of the angle.

Result with include mode

Advanced options: Check this option to check faces. If this option is not checked, calculation will be faster, but can generated some invalidities. The Optimize coincidences option allows to better resolve tangency (coincidence) problems between faces of the part to modify and the tool. A tolerance value can be given, it will influence the search for the tangent faces to optimize.

Trim

This command trims a shape using a surface, face or plane.

Creation Stages / Use: Click the icon or select Shape > Trim... from the drop-down menu (or Modeling > Local Shapes > Trim in the assembly document). 1. Select the shape to trim. 2. Define the type of trim element. 3. Select the trim element corresponding to the type chosen.

Available Options: Type of item: Plane: the trim element must be a plane or a planar face. The trimming extends to infinity (a plane does not have borders). Surface: you must select a surface or a single face of a shape. If the surface is planar, then the trim is infinite. If the surface is not planar, then it must go completely through the shape to trim. Shape: trimming occurs using all of the faces of the shape. Faces: this mode allows you to select a set of faces of a shape. The set of faces selected must go completely through the shape to trim.

Reverse: This option allows you to choose the side that will be removed. It can also be reversed by double clicking on the

yellow arrow in the graphic. Offset: This option allows you to add an offset on the trimming in relation to the trimming element. You can enter a negative value to apply to the offset in the opposite direction. The offset is computed by offsetting of the trimming element. Trimming using a surface with a negative offset.

Advanced options: Hide tools: This option allows to hide tools used for this trimming. If this option is unchecked, the tools are visible and can be used with another operation. Keep trimmed side: If unchecked, the trimmed side is hidden. If checked, the trimmed side is visible and can be used.

Additional information:

When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Fillet

Links / Videos:

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This command allows you to create fillets on shapes.

Creation Stages / Use: Click the icon or select Shape > Fillet.... from the drop-down menu (or Modeling > Local Shapes > Fillet in the assembly document). 1. Choose the fillets building mode: Identical or different radii (see details in the available options) 2. Enter the fillet value. 3. Select edges and/or faces on which to apply the fillet with the entered value.

Available Options: Radii: Identical : in this mode, all of the edges/faces selected will use the same radius value. If the radius value is modified while in use, then the edges/faces already selected (and those selected thereafter) will use this same new radius. Different : in this mode, it is possible to assign different radius values to the edges/faces selected. Thus, when you change the value of the radius, the edges/faces already selected will still use the value of the radius which was entered when they were selected. The new edges/faces selected will use the new value. This mode also allows you to create fillets of which the radius is variable (described in detail below)

Edges: The edges/faces selected will be appear in this list To delete elements from this list, it is possible to select them again in the graphic area or to select them from the list and use the "Delete" key on your keyboard. If the selection contains multiple invalidities, the contextual command Delete Invalid Selections allows to remove them quickly. By checking Shape edges, all edges of the shape are selected. If the Radii option is set on "different", then two new columns are displayed in this list: Radius: this column displays the value of the radius applied if the radius is constant. Mode: this column allows you to choose the type of fillet (constant, linear variable, changing variable). Constant

Variable linear

Variable smooth

To modify the fillet type on an edge/face, click the corresponding cell and select the desired type from the drop-down list by using the contextual menu. For variable type fillets, it is therefore possible to modify the start and end values of the fillet using the labels. To do this, double-click the numeric value on the label. Labels for linear variable fillet

To add intermediate radius values on a variable fillet, right-click the affected fillet labels and select the "Add Radius" function. A new value point then appears with a label as illustrated below. It is then possible to move the point along the edge by dragging it with the mouse or by modifying the coefficient displayed under the value of the radius (0=start of the edge and 1=end of the edge)

Of course you can modify the radius value of the point by double-clicking on the value of the radius on the label.

Corners: This option allows you to create a "ball corner" at the connection of 3 edges on which a fillet is applied. Without corner

With corner

You can modify the amount of the roundness along each edge by modifying the offset value corresponding to each edge or by dragging each point along the edge:

Constraints: This option allows you to specify the edges to follow. In this case, a variable fillet is created at the fillet's ends. Without constraints

With constraints

Limits: By default, the fillet is applied on the complete selected edges. This option allows to define limits. Points: allows to select 2 points by segment or loop to limit the fillet. These points can also be created on the fly by clicking "+". Limits: allows to select 2 planes,surfaces or faces of the shape by segment or loop to limit the fillet. These planes can also be created on the fly by clicking "+".

The pink arrows allow to invert the side of the limit.

Overflows: This option allows you to define how to create the fillet when it extends onto neighboring faces.

You can define this behavior independently for an extension on smooth edges and on square edges. An image in the dialog illustrates the principle of the selected option.

Overlaps: This option defines how overlapping fillets will be created. An image in the dialog illustrates the principle of the selected option.

Advanced Options: Dynamic preview : If this option is checked, then the preview of the fillet is updated dynamically by dragging on an offset point of a ball corner or on a value point of a variable fillet. Keep overlapped faces : When this option is checked, TopSolid stores in the memory the topology of the faces which disappeared after creation of the fillet. This keeps you from losing operations that use these faces as references. Below is a shape with a boss operation made on the upper face. The fillet makes this face disappear. Here the behavior difference is observed. Initial shape

Deactivated option

Activated option

Repair self-intersecting : This option allows you to automatically repair the autointersection area of a fillet. This option allows in some cases certain fillets to be able to be created despite the fact that the surface of the fillet self-intersects. Vertex blending : This option allows you to round off corners between two consecutive fillets. Option Disabled

Option Enabled

Variable fillet on edge : This option allows to smooth the junction between 2 edges. Option Disabled

Option Enabled

Tight curvature of adjacent faces: "Tight curvature" means here that the curvature radius of the face is smaller than the fillet radius. This option allows to modify the construction method of the fillet on lateral faces that have a curvature radius smaller than the fillet radius. it is possible to choose among 3 types of situation: Blends : the adjacent faces with tight curvature are fillet type faces. The green face is a fillet type face.

So it is possible to use the Blend type method (the simplest method).

Faces : the whole face has a tight curvature. The green face is not a fillet type face and has a tight curvature.

The "fillet" type method is not able to manage this case. So it is necessary to use the Face type (or the next one).

Partial : only a section of the face has a tight curvature. The green face has a tight curvature on a portion only.

Only this last mode is able to manage this case.

In general terms, the "Partial" type is the one that will work in all cases. But its computation is more complex and will be longer. So it is recommended to use the type that fits the best with the situation in order to make the operation calculation shorter.

Modifications: Double-click the fillet to display and modify the values of the radii.

Additional information: When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Chamfer

This command allows you to create chamfers on the edges of a shape.

Creation Stages / Use: Click the icon or select Shape > Chamfer... from the drop-down menu (or Modeling > Local Shapes > Chamfer in the assembly document). 1. Choose the chamfer creation type: Identical or different values (see details in the available options) 2. Choose the chamfer creation mode 3. Fill in the parameters corresponding to the mode chosen 4. Select the edges and/or faces on which to apply a chamfer with the value provided

Available Options: Value: Identical: in this mode, all of the edges/face selected will use the same values as the chamfer parameters. If the values are modified while in use, then the edges/sides already selected (and those selected thereafter) will use this same radius. Different: in this mode, it is possible to assign different values to the edges/faces selected. Thus, when you change the value of a parameter, the edges/faces already selected will still use the value of this parameter which was entered when they were selected. The new edges/faces selected will use the new value. This mode applies the different values to the chamfer, but it is not possible to change the creation mode.

Mode: You can choose here the way in which the chamfer is parameterized: Offsets

Distance Angle

Distances

Offsets: Offsets: This mode creates chamfers that are even, this being the case even on non-planar faces or those faces that do not have an constant angle amongst each other. It is therefore indispensable when a chamfer is made on non-planar faces.

Angle Distance: This mode only supports planar, cylindrical or conical faces. The chamfer will not function if the faces are complex (curves). Distance: This mode only supports planar, cylindrical or conical faces. The chamfer will not function if the faces are complex (curves).

Distances and Angle Distance: Supported edges must have neighboring faces type: - Plane - Plane, - Plane - Cylinder - Plane - Cylinder/Cone - Plane - Cylinder/Sphere

Edges: The edges/faces selected will be appear in this list. To delete elements from this list, it is possible to select them again in the graphic area or to select them from the list and then use the "Delete" key on your keyboard. If the selection contains multiple invalidities, the contextual command Delete Invalid Selections allows to remove them quickly. You can invert the direction of the chamfer by clicking on the last column "Invert" If the Values option is set on "different", then two new columns are displayed in this list. These two columns correspond to the value of the two parameters of the chamfer for the corresponding edge. You can modify the value of the parameters by clicking in the cell.

Limits: By default, the chamfer is applied on the complete selected edges. This option allows to define limits. Points: allows to select 2 points by segment or loop to limit the chamfer. These points can also be created on the fly by clicking "+". Limits: allows to select 2 planes,surfaces or faces of the shape by segment or loop to limit the chamfer. These planes can also be created on the fly by clicking "+".

The pink arrows allow to invert the side of the limit.

Advanced Options: Keep the faces covered: When this option is checked, TopSolid stores in the memory the topology of the faces which disappeared after creation of the chamfer. This keeps you from losing operations that use these faces as a reference. Below is an example illustrating the occurrence with a fillet. The principle is the same for a chamfer. Here is a shape with a boss operation made on the upper face. The fillet makes this face disappear. Here the behavior difference is observed. The behavior is similar with a chamfer. Initial shape

Option Disabled

Option Enabled

Modifications: Double-click the chamfer to display and modify parameter values.

Draft

This command allows you to create drafts on the faces of a shape.

Creation Stages / Use: Click the

icon or select Shape > Draft... from the drop-down menu.

1. Enter the draft angle. 2. Choose the creation mode of the draft. With the reference plane With the parting line On isoclines With step

3. Depending on the chosen creation mode, you must define: either the reference plane and faces to draft. either the reference direction and edges of the parting line. or the draft direction and faces to draft.

Available Options: Draft in Reference Plane Mode: Plane: this option allows you to define in relation to which plane the draft is applied. The blue arrow indicates the reference direction of the angle.

Face: this option allows you to define on which faces the draft is applied.

Draft in Parting Line Mode: Direction: This is the reference direction for the measurement of the draft angle. In other words, this can represent the mold opening direction of the part. Parting lines: add to this list the edges around which the faces will "pivot" in order to generate the draft. By clicking the small icon in the "invert" column, the face of the other side of the edge will be treated.

Draft on isoclines mode: With this mode, fillets are between the fixed face (indicating the direction) and faces to draft are to be selected. Direction: This is the reference direction for the measurement of the draft angle. In other words, this can represent the mold opening direction of the part. Faces: Select faces to which the draft is applied.

Initial part

In blue: the direction, in pink : selected faces, in transparent orange: the preview

Rebuild blends: This option has to be checked if faces to draft have fillets.

Draft with step: This mode allows you to apply draft on faces with a step following edges. the drafted face will not be divided acco reference edges, but a step will appear on the edges. Faces: Select faces to which the draft is applied. Step edges: Select all the fix edges of the face.

Tapered step (surfaces are generated the same way as the face to draft)

Special Faces:

Normal step (surfaces are ruled surfaces perpendicularly to the face to draft)

Step with sheet (surfaces ba geometry of the parting s

Option specific to the mode This option allows you to assign specific draft angles for certain faces. Select the faces in order to add them to the list and to modify the draft angle in the list.

Advanced Options: Smooth boundary edge: If the drafted faces have smooth lateral edges (tangency with another face), then created to allow the draft to be created.

Smooth edge: In the case of two drafted tangent faces with different angles, this option creates a lateral fac edge. Initial shape

Option disabled

Option Enab

Extend mode: This mode allows to select how the draft should react regarding a close geometry like for ex Automatic or drafted faces

Additional information:

Fixed faces

None

When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Drilling

This command allows you to perform different types of drilling operations on a part.

Creation stages / Use: Select Shape > Drilling... from the drop-down menu (or Modeling > Local Shapes > Drilling in the assembly document). 1. 2. 3. 4.

Select and/or create a drilling template. Select (or create by clicking on "+") the drilling frame. Select the shape to drill. Validate the command with the button

To be able to create tapped holes, you need to reference a library containing the standard you wish to use for the tapping.

Available Options: Lightweight: This option allows you to not create the boolean operation, it is available for holes only. The drilling is then displayed with a circle but the operation gets all the manufacturing information for Top Create Features option must be checked as well. The drilling created this way can be repeated, it allows to design a flat part with a huge number of holes. displayed in the drafting document as well.

Inoperative: This option allows you to create a drilling without making the corresponding boolean operation. It is main drilling from an imported geometry. This option concerns blind holes only. A through hole must be defined as a blind hole with a depth equal When the Home > Create MF option is checked, the drilling operation gets all the manufacturing informa

Templates and types of drilling:

With these options you can:

Current Fast Drillings: These three buttons allow you to create a spot faced hole, tapped hole or smooth bore without opening the drilling templates.

Explore Templates: By clicking on this option, you access the list of drilling templates where you can select the one you want to use.

Frame: With this option, you define the frame on which the drilling will be carried out. Each drilling operation requires a frame which defines the position of the drilling and its direction. The drilling is done based on the Z- of the frame. The Z- axis must therefore be directed toward the inside of the part so that the drilling can be carried out. If there is no drilling frame, it can be created in a dynamic way on certain types of faces by moving the mouse over this face: Plane face: the frame created is a is a constrained frame on the nearest edges of the face.

Cylindrical face: a radial frame is created.

Face with circular edges: a frame on face and center point which is created.

Reference frame: Possibility to use a reference frame on which be based axes of the constraint frame. Regarding the constraint frame, the reference frame can be used with automatic mode only.

The constraint frame of the drilling uses axes of the reference frame.

Shape to drill: Select the shape on which the drillings will be done.

A group of drillings can only be done on one shape. Several shapes cannot be selected for the same operation.

In/Out counter sinking:

Allow to apply different-sized countersinkings (length and angle) to each type of drilling.

In/Out counter sinking: Allow to activate the counter sinking. A boolean parameter can be used to condition the counter sinking creation. Length: Value of the countersinking length. Pitch factor: If the drilling primitive is a tapping hole, you can use a counter sinking length whose the value is function of the pitch and a factor defined by the user. Advanced options: Origin: This option allows you to define the measurement origin of the drilling depth: Frame: The depth is measured in relation to the origin of the frame. Face: The depth is measured in relation to a face specified by the user. Extension process of Countersink: This option defines the countersink drilling process at the entry face. In fact, drilling starts in the origin of the frame. However, in the event of an inclined face or the presence of a shoulder next to the drilling, TopSolid needs to "extend" the drilling above the origin point to achieve a good result. These are the two possible modes: Extend surfaces

Add a cylindrical face

Machining process:

Machining process: This option allows to assign a machining process to the operation. This machining process is recognized by TopSolid'Cam. It can also assign a color to the operation. Drilling processes: Below the main options, a list of icons is displayed which allows you to modify the parameters of the different procedures of the drilling template used.

By default, the values are those of the drilling template. It is therefore not required to access this if the values of the template are those you wish to use. See here for the detailed description of the different procedures.

Threading

This command creates a threading on the cylindrical faces

Creation stages / Use: Click the icon or select Shape > Threading... from the dropdown menu. 1. 2. 3. 4.

Select the cylindrical face to thread. Select the original plane to determine the start of the threading. Determine the different threading parameters Validate the command with the button

To be able to create threadings, you must reference a library containing the standard you wish to use for the threading.

Available Options: Complete threading: This option allows to create the threading along the entire length of the selected face.

Length: This option specifies the length of tapping (measured in relation to the original plane). If the Complete tapping is set to True, the length is grayed.

General:

Standard: This option allows you to select the threading standard to use from those found in the project or references. The threading dimension is automatically selected from the dimensions available in the standard based on the diameter of the cylindrical face selected. If this option is deactivated, you have to fill every tapping values (Description, nominal diameter, pitch, internal diameter, but also in the advanced tab, if the tapping is left hand or not). Strict: If this option is checked, the diameter of the selected cylinder must be strictly the same than the diameter of the selected standard.

Advanced: Thread start number: Allows to define the tread start number. This value is generally set to 1. Left hand: Allows to define the thread direction. This value is generally set to False.

Groove or shoulder Links/Videos:

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This command creates grooves or shoulders on cylindrical or tapered shapes. The geometry achieved is linked to the choice of a groove/shoulder template from the referenced library Before being able to use this function, your project references must have a library containing grooves/shoulder templates. The "TopSolid Mechanical Library" contains a selection.

Creation stages / Use: Click the icon or select Shape > Other Operations > Groove or Shoulder... command from the drop-down menu. 1. Select the type of operation you wish to carry out. Groove:

Shoulder:

2. Select the desired groove/shoulder template. 3. Enter dimensions of your groove/shoulder or select a code. 4. Define the positioning of the operation.

Available Options: Template:

The drop down list proposes the groove/shoulder templates available in the referenced libraries. If the template selected features pre-defined dimensions due to a catalogue, you can select the desired dimension code.

Drivers: Here, you can define the dimensions of your groove/shoulder. Offset: this value refers to the depth/overthickness of the groove/shoulder. Width: this value refers to the width of the groove/shoulder.

Position: This option determines the position of the operation. Axial frame: if the mouse is rolled over a cylindrical face, an axial frame is displayed dynamically. Click here to create the frame. Reference plane: this option changes the reference plane/face for measuring the positioning distance of the operation. Once the frame is created, the distance of the frame in relation to the reference face can be modified by pulling on the point of the arrow or by double-clicking on the label to modify the value. Face mode: Operated face: defines on which face the operation is to be carried out on. A coincidence constraint will be added between the selected face and the surface silhouette axis define in the groove/shoulder template. This option is useful in the event of a hollow cylinder, for example, to select the inner face. Diameter mode:

Diameter: value use to position the surface silhouette axis define in the groove/shoulder template (with revolution dimension from the X axis of the groove/shoulder frame). This mode is the only one compatible with the use of a groove as operator in a Process document. Shape to modify: shape on which the groove/shoulder operation will be applied. Reverse: This option reverses the direction of the groove/shoulder in the event the operation is not symmetrical (a fillet on only one side, for example).

Modifications: Once the function has been validated, a sketch is created with the dimensions of the groove/shoulder in place. Therefore, to modify the geometrical dimensions of the operation, you need to edit the sketch. If you wish to modify the positioning of the operation, you can either edit the axial frame or edit the operation itself. In the event you edit the operation, a check box called "Replace the template" allows you to fully redefine the template of the groove/shoulder.

Additional information: Personal groove/shoulder templates can be created. The Diameter mode is the only one compatible with the use of a groove as operator in a Process document.

Slot or Tongue

Links/Videos:

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This command creates a slot or a tongue on a shape by running a section along a path.

Creation stages / Use: Select Shape > Other Operations > Slot or Tongue... command from the drop-down menu. 1. Select the type of operation you wish to carry out. Slot:

Tongue:

2. Select the path of the slot/tongue 3. Select desired slot/tongue template or the sketch created for this purpose in the document to define the section. 4. Enter dimensions of your slot/torque or select a code.

Available Options: Slot or tongue: Here, select the type of operation to be carried out and select the shape to modify.

Path: The path represents the route following by the slot/tongue. It can be open or closed. By clicking the "+" it is possible to create an edge profile "on the fly". Planar path:

The sketch tool is always oriented based on the plane of the path sketch. It is therefore important to correctly orient the plane of the path sketch in order to obtain the desired slot/tab. Generally, the plane of the sketch must be parallel or tangent to the operated face. Misoriented Sketch Plane

Correct Sketch Plane

When using an edge profile, if only a linear edge is selected, the boundary will be invalid. A line does not define a plane. Path with tilted tool: When you use path on which you need to use a tilted tool, you need to specify a reference direction so the orientation of the tools remains correct all along the path. On the example bellow, the tool sketch is titlted according to the path. Without giving a reference direction, the sketch of the tool is reoriented according tho the plane of the path.

In this scenario, the reference direction (in yellow on the illustration) allows to keep a correct orientation of the tool.

Non planar path:

When the path is not planar, it is necessary to specify a direction that define the orientation of the toll along the path. In the example below, the direction is shown with the yellow arrow.

Sketch Tool: The sketch tool is actually the section of the semi-slot/tongue and runs along the path in the following way to generate the shape of the operation: The path is in green, the sketch tool in pink and the resulting geometry in orange.

User sketch: If you wish to use a sketch created in the document as a section of your slot/tongue, you need to define it with the following criteria: the sketch must only represent half of the slot/tongue. it may be drawn on any plane in any location in the document (not necessarily in place), but must have a colinear segment to the Y axis of the construction plane. Sketch for slot:

Sketch for tongue:

Double-usage sketch:

The same user sketch may be used to make several identical slots/tongues in the document.

Template sketch: By checking this option, you can use a sketch template. The drop down list offers you the available slot/tongue templates in the referenced libraries. If the selected template has pre-defined dimensions by virtue of a catalogue, you can select the desired dimension code.

Before being able to use a template sketch, your project must have a library containing slot/tongue templates in its references. The "TopSolid Mechanical Library" contains a selection.

Drivers: In the event of a sketch template, if the template has dimensional drivers, you can fill them in here.

The name of the drivers and their number may vary based on the template selected.

Advanced options: These options enable you to modify the geometry of corners and extremities: Sharp

Rounded

Normal

Extremities on the inside

Limit the extremities

Modifications: If a sketch template was used, once the function has been validated, a sketch is created with the dimensions of the slot/tongue in place. Therefore, to modify the geometrical dimensions of the operation, you need to edit the sketch.

Additional information: You can create customized slot/tongue templates.

Pattern union

This command allows a shape to be repeated (duplicated) according to a chosen pattern and then automatically gathers together all of the copies created in this way. In the end, one single shape is obtained.

Creation Stages / Use: Click the icon or select the Shape > Other Operations > Pattern Union... command from the drop-down menu. 1. Select the shape to use for the pattern. 2. Define the pattern to apply and its parameterization.

The result obtained is one single shape.

This command is very practical for shapes having axes of symmetry. This way, only some of the part is modeled and the modeling is completed by applying one pattern per symmetry. The design is therefore lighter and the file is smaller. Below is an example with a circular pattern:

Available Options: Pattern: This option allows you to choose the type of pattern that you wish to obtain: linear, circular, according to sketch, on frame, symmetric. You will find further details about the definition here.

Modifications: After creating the pattern union, you can modify the parameters of the pattern from the entities tree in the "Patterns" folder, which contains all of the patterns used in the document.

Additional information: When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Trim by profile

This command allows you to trim a shape by a profile.

Creation Stages / Use: Click the icon or select the Shape > Trim by profile... command from the drop-down menu (or Modeling > Local Shapes > Trim by profile in the assembly document). 1. 2. 3. 4. 5. 6.

Select the shape to trim. Select the trim type Select Extruded, Revolved, Imprinted or Round a point. Select sections regarding the selected type and a point on face if it is Round a point Check or uncheck Reverse to reverse the trim side. Select the direction for trimming by extruded profile, or the axis for the trimming by revolved profile. For imprinted and round a point, select if the direction is orthogonal or specify a direction.

Available Options: Type of element: Extruded: Trimming occurs by extrusion of the profile according to the chosen direction (by default, this is the normal direction to the plane of the profile). Revolved: Trimming occurs by rotation of the profile around an axis that you define Imprinted: The trimming is done by extruding the imprinted section in the chosen direction (by default, the normal direction of the section). Round a point: Trimming occurs by selecting a point on a face. A search will be automatically done to find the profiles near the selected point. It is possible to manually select profiles to use.

Extend profiles or extend until: Regarding the selected mode , you are able to extend profiles or extend until Extend profiles: (Only for extruded and revolved) When the section is shorter than the shape to trim, the trimming can only be done by checking this option.

Extend until: (only for imprinted and around a point). First edge: The trimming is done up to the first found edge. Boundary edge: the trimming is done on the complete shape, until the boundary edge.(only available for a surface shape, a solid has no boundary edge).

Before trimming

Extend until first edge

Reverse: This option allows you to invert the trim side. If this option is not checked, the shape generated by the extruded or revolved profile is removed from the part to modify. If this option is checked, then the intersection between the shape and the extruded or revolved profile remains. Trim by extruded profile without Reverse option.

Trim by extruded profile with Reverse option.

Trimming by revolved profile without reverse option.

Trimming by revolved profile with reverse option.

Partial trimming (for trimming by an extruded or revolved profile): This option defines the trimming distance in the 2 directions for trimming with extruded profile and the angle in the 2 directions in relation to the axis chosen for trimming with revolved profile. Partial trimming with extruded profile.

Partial trimming with revolved profile.

Extend until boundary edg

Hide tools: This option allows to hide tools used for this trimming. If this option is unchecked, the tools are visible and can be used with another operation.

Keep the trimmed side: If unchecked, the trimmed side is hidden. If checked, the trimmed side is visible and can be used.

Straighten lateral faces: This option allows to straighten lateral faces to make them normal to the trim faces. This option is only available for sheet metal parts and corresponds to the Straighten lateral faces from the sheet metal menu.

Modifications: The modification can be done from the operation tree or graphically in the popup menu from one of the faces resulting from the trim.

If the profile is open, then it should overlap the part or check Extend profiles or extend until options. Partial trimming is not possible if the profile is closed.

Additional information: When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Reciprocal trimming Links / Videos:

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This command trims a shape with respect to one another and inversely.

Creation Stages / Use: Click the icon or select the Shape > Reciprocal trim... command from the drop-down menu (or Modeling > Local Shapes > Reciprocal trimming in the assembly document). 1. Select the first batch of faces on the first surface shape. 2. Select the second batch of faces on the second surface shape. 3. Validate

When selecting faces, the entire shape is selected by default. To select only certain faces, use the rotative selection.

Available Options: Consider all shape: This option is automatically checked if the shape is a solid. All its faces will be taken in account.

Reverse:

This option allows you to determine the side that will be removed by the trimming. An arrow in the graphic zone indicates the side that will be removed. You can also double-click the arrow to enable or disable this option.

Mode: If the selected faces do not intersect completely (i.e. the intersection of the faces does not reach the border edges of the surfaces), this option is used for defining how the faces should be extended: Tangent: Tangent extension of the intersection between the batches of faces. Orthogonal: Extension following the intersection normal between the batches of faces. Reverse orthogonal: Extension in the direction opposite the intersection normal between the batches of faces.

Extend until: If the faces must be extended, you can also define where the faces should extend: First edge: The surface is extended to the first edge encountered on the other shape. Border edge: The surface is extended to the other shape's border edge.

Advanced Options: Keep the trimmed side from the first shape / Keep the trimmed side from the second shape Both of these options can save the part that is normally removed by the trimming. This trimmed side then becomes an independent entity of the main shape and can be found in the "Shape" folder in the entity tree.

Fillet Faces-Faces

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This command allows you to create a fillet between sets of faces.

Creation Stages / Use: Click the icon or select the Shape > Other operations > Fillet facesfaces... command from the drop-down menu. The command has two ways to create a fillet: Fillet between faces: allows to create a fillet between two batches of faces. 1. Select the batch of faces from the first side. 2. Reverse the direction, if necessary. 3. Select the batch of faces from the second side. 4. Reverse the direction, if necessary. The arrows indicate the side when creating the fillet. 5. Choose the radius type: Constant radius: The value entered is constrained for the entire fillet. Constant length: The length (shortest distance between the two fillet edges in contact with the set of faces) is constant for the fillet. Variable radius: The fillet radius will change between the input radius r11 and radius r12. r11 is the radius at the start of the intersection edge, and r12 is on the other side. Conical radius: The conical radius is created by entering two radius values for each side of the intersection edge. r11 will be the radius at the start of the edge on the side of the first batch of faces, and r12 will be the radius at the end of the edge on the same side. r21 and r22 will be the equivalents on the second batch of faces. 6. Validate by clicking .

Three face fillet allows to create a fillet passing by 3 batches of faces. 1. Select the batch of faces from the first side. 2. Reverse the direction, if necessary. 3. Select the batch of faces from the second side. 4. Reverse the direction, if necessary. 5. Select the batch of faces from the third side. 6. Reverse the direction, if necessary. The arrows indicate the side when creating the fillet. 7. Validate by clicking .

To select all of the tangent faces rather than selecting them one by one, use the rotative selection on one of the faces.

Available Options: Section:

Loop: The fillet between ball faces results from having the intersection of the faces form a sphere. The definition of normal to the section planes is not requested for a ball fillet. For a ball fillet with a curvature section shape, you must enter a curvature value. A value of 1 is equivalent to the conical section shape. The closer the value is to 0, the more the curvature will move to the right.

Section Shape: Conical

Section Shape: Curvature

Section Shape: Chamfer

Disk: The disk fillet between faces is created by making the intersection of the faces a disk. For this type of fillet, you must define the guide profile (spine profile) for the disk. The disk's normal is defined by the tangent to a given profile. This profile must be able to define a normal for each point of the fillet. The green profile or edge defines normal for the section plans. The geometry of the fillet is directly influenced by this normal.

The spine profile "follows" the intersection.

The spine is linear

The spine profile is linear and oriented

Spine profile origin: When the variable or conical fillet type is chosen and when the spine profile is closed, you can select a point on the spine profil that will be used as the origin of the spine profile. The value of the r11 radius will ba applied on this origin. When no point is given, the value of the r11 radius is applied on the spine profile origin.

Constraints: (only for the fillet between faces)

Constraints must be given by the edges of the element. It is therefore necessary to print the constraint profile(s) to the face(s). The radius defines the maximum radius of the constrained fillet. It must therefore be larger than the greatest distance between the intersection of the two faces and the constraint edge. Otherwise, the constrained fillet will be constant for distances greater than the given radius. None: Imprinted profiles are not taken into account.

Symmetrical edges: The selected printed edge will be made symmetrical with the intersection edge.

Edges - Edges: Both imprinted edges will be taken into account for the fillet.

Edges - Radius: The fillet will have the entered radius and will be limited by the selected imprinted profile. The radius must be less than the greatest distance between the impression and the intersection edge for the various faces.

Advanced Options: Repair auto-intersections: Makes it possible to repair fillets that self-intersect. In

the example below, it is not possible to make the fillet without activating this option.

No option

With option

Overlap: (only for blend between faces) extends the fillet after an interruption in either face (pocket for example).

No option

With the option

Propagate to discontinuous edges: (only for fillet between faces).Makes the fillet, even if there is a sharp angle between faces of the same side. The input angle must be at least equal to the angle between the two faces. In the example below, just one vertical face was selected, and the entered angle was 15°. The Angular tolerance allows to enter the angular tolerance to respect during the discontinuous edges propagation. In this case, the fillet will be created only if the angle is under the tolerance limits.

No option

With the option

Point: In some cases, it could be several possibilities. The point allows to select on which side applying the fillet.

Without selecting a point

by selecting a point

Hollow

This command removes a full hollow shape and thus to obtain a hollow shape with a thickness.

Creation Stages / Use: Click the icon or select the Shape > Other Operations > Hollow... command from the drop-down menu. 1. Select the solid shape to hollow. 2. Provide the thickness of the hollowed shape. 3. The yellow arrow indicates the hollow side. The side can be reversed by double-clicking the arrow or by checking Reverse. 4. Select faces to remove if need be. 5. Validate the command with the button

Available Options: Thickness: With this option, you define the thickness of the hollowed shape. The "Invert" check box allows you to create the thickness towards the exterior of the initial part.

Faces to Remove: This option allows you to select faces of the shape that will be removed before hollowing the shape. Thus, an opening is obtained in place of the faces selected here. The faces can be removed from the list by selecting them again on the shape.

Special Faces: With this option, you can select faces to assign a specific thickness to them. Initial solid shape

Hollowed shape

The green face is the face on which a special thickness is defined. The orange face is the removed face.

Advanced Options:

Self-intersections: Trim: When faces to offset intersect together, this option allo to trim unnecessary parts. Repair: When faces to offset intersect together, this option allows to delete and replace them by faces like fill hole.

Surface to thicken

Additional information:

Thickening with the trim option In green the surface to thicken, in yellow the offset surface.

When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Thicken

This command applies a thickness to a surface shape.

Creation stages / Use: Click the icon or select the Shape > Other Operations > Thicken... command from the drop-down menu. 1. Select the surface shape to modify. 2. Enter the first thickness to apply. 3. Validate the command with the button.

Available Options: Center: By clicking this option, the thickness given is distributed equally on both sides of the surfacic shape. This option allows you to use the "Enable the thickness side 2" option.

Invert: By checking this option, the thickness changes its side.It is indicated by the yellow arrow. You can also change the side by double clicking on the arrow.

Enable the thickness side 2: This option allows you to provide a second thickness in order to define the thickening value on both sides of the surface shape.

By clicking on the different elements of the handle, you can act on the options of the function:

1 On the point: Enables or disables the second side. 2 On the arrow: Reverses the thickening direction

Special Faces: With this option, you can select faces in order to assign specific values to them for the thickness of each side of the initial surface. Initial surface

Thickened shape

The orange face is the face on which the special thickness is defined.

Advanced Options:

Self-intersections: Trim: When faces to offset intersect together, this option allows to trim unnecessary parts. Repair: When faces to offset intersect together, this option allows to delete and replace them by faces like fill hole.

Surface to thicken

Additional information:

Thickening with the trim option In green the surface to thicken, in yellow the offset surface.

When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Offset

This command allows to modify a shape dimensions by parallelizing its faces.

Creation Stages / Use: Select the Shape > Other Operations > Offset... command from the drop-down menu. 1. Select the shape to offset. 2. Enter the global offset distance in the Distance field. 3. Validate the command with the button.

If the shape to offset has some tapped holes, these tappings will be lost.

Available Options: The Invert option offsets the shape in the other direction. In fact, the shape can be offset towards the interior and towards the exterior. You can invert the direction by double-clicking on the handle (yellow arrow) in the graphic area

Special Faces: The Distance field allows to indicate an offset distance different than the global offset distance for all the faces whose no values is added.

It is then possible to individually add a distance value for some faces. The option allows to access to different faces selections : blend faces, faces along edge paths, faces by color, faces by tangency, root face. In the example below, the green face is the face on which a special distance has been defined at zero The initial shape is the shape viewed by transparency in the interior. The final result is the outer shape.

Advanced Options:

Self-intersections: Trim: When faces to offset intersect together, this option allow to trim unnecessary parts. Repair: When faces to offset intersect together, this option allows to delete and replace them by faces like fill hole.

Surface to thicken

Thickening with the trim option In green the surface to thicken, in yellow the offset surface.

Deformation Links/Videos:

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This commands allows to deform a shape or a surface. Available deformations are: Flexion Shape on Shape Profile on profile Torsion Traction

Creation stages / Use: Click on the icon or select the Shape > Other operations > Deformation... command from the drop-down menu. 1. Select the shape or surfaces to deform. 2. Select a deformation if it has been created before, if not click on "+" to create one. 3. If surfaces have to be deformed, select surfaces to deform. If we consider as example a sheet metal part to be unfold, the 2 faces on the bend (the inside and the outside of the bend) and the 2 lateral faces are all faces that have to be deformed. All the faces of the flange to unfold are faces to be transformed. In this kind of case, lateral surfaces have to be separated for each group of surfaces. You can use the Surface > Imprint command. 4. Validate by clicking .

The initial volume of the shape is not preserved after deformation.

Available Options: Face by face: This option allows to use another mechanism for calculating the deformation when the overall deformation fails. Detect faces to exclude: This button allows to automatically excludes the problematic faces. These faces will be added to the list of faces to exclude, this list can be completed manually. Unsew: Activating this option TopSolid will create as many surfacing shapes as faces composing the shape to deform. These surfaces are available in the Shapes folder of the entities tree. Without this option TopSolid will create a unique surfacing shape result of sewing of all faces at the given tolerance. Create boundary edges: Because this deformation mode allows a surfacing result, it is interesting to recover the boundary edges of exclude faces to help the construction of new surfaces. A sketch operation is then created in the operation tree.

Original shape with flexion deformation

Preview and result of the flexion deformation. The front cylindrical face face and 2 side faces have been automatically excluded to allow this de

Rebuild blends: If this option is not activated, the fillets of the part will be deformed as well. The deformation can generate a loss of tangency or a punctual change of the radius at some points. When checking this option, fillets are "removed" before deformation, then rebuilt after deformation.

Torsion without rebuilding blends option

Torsion with rebuilding blends option

Faces to deform: If you have chosen some faces with the Faces to deform option, this dialog allows you to select the faces that will not be deformed but moved only. This could increase performances on complex shapes.

Example of torsion with faces selection, the 2 yellow faces are moved only

:

Modifications: Each modification can be done using the popup menu from the operations tree.

Additional information: When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Pipe unbending Links / Videos :

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This command allows to unbend elbows of a shape. We can then find the geometry of the initial pipe used for the manufacture of bent pipes.

Creation stages / Use: Click the icon or select the Shape > Other Operations > Pipe Unbending... command from the drop-down menu. 1. Select the unbending mode (simple or complex). 2. Select the fixed edge. 3. Select faces to unbend.

Available options: Simple elbow: Allow to manage simple elbow with circular section (toric shape, hollow or full, without hole in faces). Selection of only one bent face is enough, the complementary face will be selected automatically. The All option allows to select all elbow of the shape.

Example of Pipe unbending with simple mode

Complex elbow: Allow to manage complex elbow bend per bend (non circular section, with deformation). With this mode, you have to select all faces of the elbow. These faces must be connected with the fixed part on side. Border edges on each side must be on a plane (see first image below). Fixed plane and mobile plane mu planes is managed unrolling selected faces. Surface result is authorized on complex deformations.

A : fixed part with fixed plane. B : mobile part with mobile plane.

unbending with deformation of complex pipe

Modifications / Additional information: With simple mode, length of unroll area is calculated from median radius of torus.

With complex mode, length of unroll area is calculated on median radius of fixed section.

Drilling group

This command allows you to carry out several identical drilling operations in one operation. The position and the number of drillings is defined by the points of the a reference sketch.

Creation stages / Use: Click the icon or select Shape > Other operations > Drilling group... command from the drop-down menu. 1. The first stage of this function is identical to the Drilling function and allows you to select and/or define a drilling template. 2. Select the sketch containing the position points of the drillings. 3. Select the mode : Allows you to drill sketch (not internal) points. Allows you to drill sketch circles. If this mode is activated, there are 2 possibilities: If all circles have the same diameter, TopSolid uses the measured value of the circle diameter as hole diameter. If circles have different diameters, TopSolid uses the default values for each kind of hole. Allows you to drill sketch points and circles.

4. Define the direction of the drilling. 5. Select the shape to drill. 6. Validate the operation with .

To be able to create tapped holes, you need to reference a library containing the standard you wish to use for the tapping.

To unselect one of the 2 modes, just click again on the corresponding icon. At least on of these modes has to be selected.

Advanced Options: Machining process: Machining process: This option allows to assign a machining process to the operation. This machining process is recognized by TopSolid'Cam. It can also assign a color to the operation.

Available Options: Templates and types of drilling: With these options you can:

Current Fast Drillings: These three buttons allow you to create a spot faced hole, tapped hole or smooth bore without opening the drilling templates.

Explore Templates: By clicking on this option, you access the list of drilling templates where you can select the one you want to use Sketch: Select the sketch here to use for defining the position of the drilling.

The drillings are created in all the points with the status non-internal in the sketch.

In other words, if no point of the sketch is visible outside the sketch's editing mode, then no drilling can be created. All the points used must intersect the shape following the defined direction. If one of the points is "in space" the operation cannot be run.

Direction: Define the direction of the drilling.

The defined direction represents the Z+ of the drilling frame. However, the drilling is done based on ZTherefore, take care to note the direction indicated by the arrow which must indicate the opposite direction of the drilling (towards the exterior of the material).

Shape to drill: Select the shape on which the drillings will be done.

Grouped drilling can only be done on one shape. Several shapes cannot be selected on the same operation.

Pattern: Possibility to select a reference point corresponding to the pattern origin. This origin and the drilling group repetition will be automatically proposed in an assembly using this part to repeat a component with the same pattern. If in the assembly, a component is positioned at this place and if it is repeated, by flying over the drilling group, you will have access to the pattern defined by the drilling group. Without this reference point, the drilling group pattern will not be proposed when repeating the component in the assembly.

Drilling processes: Below the main options, a list of icons is displayed which

allows you to modify the parameters of the different procedures of the drilling template used. By default, the values are those of the drilling template. It is therefore not required to access this if the values of the template are those you wish to use. See here for the detailed description of the different procedures.

Tapping

This command creates tappings on the cylindrical faces

Creation stages / Use: Click the icon or select Shape > Other Operations > Tapping... command from the drop-down menu. 1. 2. 3. 4.

Select the cylindrical face to tap. Select the original plane to determine the start of the tapping. Determine the different tapping parameters Validate the command with the button

To be able to create the tappings, you must reference a library containing the standard you wish to use for the tapping.

Available Options: Length of tapping: This option specifies the length of tapping (measured in relation to the original plane). The Complete tapping command creates the tapping along the entire length of the selected face. If the Complete tapping is set to True, the length is grayed.

Standard: This option allows you to select the tapping standard to use from

those found in the project or references. The tapping dimension is automatically selected from the dimensions available in the standard based on the diameter of the cylindrical face selected. If this option is deactivated, you have to fill every tapping values (Description, nominal diameter, pitch, internal diameter, but also in the advanced tab, if the tapping is left hand or not).

Knurling

This command allows you to create a strait or crossed knurling on a cylindrical face of a shape.

Creation stages / Use: Click the icon or select Shape > Other Operations > Knurling... command from the drop-down menu. 1. Select the cylindrical face to knurl. 2. Select the type of knurling you wish to create:

straight or

crossed. 3. Enter the pitch or the slots count and the angular orientation of the knurling. 4. Validate.

The created knurling is a single texture wrap. It does not physically modify the geometry of the part. As a result, knurling will only appear on shadowed views in the draft.

Available Options: Pitch/Slot count: This option allows you to control either the knurling pitch (distance between each slot) or the slot number to split on the face.

Angle:

You are able to specify the angular orientation of the knurling.

Coloring Links / Videos:

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This command applies a specific color on one or more sides of a shape.

Creation Stages / Use: Click the icon or select the Shape > Other Operations > Coloring... command from the drop-down menu. 1. Select the faces to colorize. 2. Choose the color to apply.

Available Options: Color: By clicking this option, you have access to the color palette which allows you to choose an existing color or to define your own personalized colors.

Modifications: The coloring operation can be modified from the operation tree.

Coating Links/Videos:

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This command applies a coating to the faces of a shape.

Creation stages / Use: Click the Coating icon or select Shape > Other operations > Coating... command from the drop-down menu. 1. Select the faces to which you wish to apply the coating. 2. Select the type (see below) 3. Select the category and the coating in the list of those available in your references. 4. Select the orientation frame for the coating. 5. Validate by clicking on .

Before being able to use this function, your project requires a library containing the coatings in its references. The "TopSolid Mechanic Library" contains a selection.

Available Options: Type: The Parameter option allows to drive the coating by a parameter which references a Coating document. See coating

parameter command for more details. The Document option allows to choose a coating defined by a coating document. Orientation frame: This option selects the frame which will be used as a reference to position the coating. This can be useful in the event the coating contains a texture which needs to be positioned with precision in relation to the face (like for wood).

Decal Links/Videos:

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This command allows you to apply a specific coating on top of the existing material of a shape, such as a sticker.

Creation stages / Use: Click the icon or select Shapes > Other Operations > Decal... from the drop-down menu. 1. Select the faces. 2. Select the decal texture.

A decal texture must be created.

Available Options: Projection: 1. Select the orientation frame of the texture. 2. Select its projection type (for projection onto a planar or cylindrical face). 3. Enter the horizontal and vertical offsets of the origin point projected onto the face, as well as the angle of the texture in relation to this frame.

Size: 1. Check the Keep Proportions box in order to not deform the texture. 2. Check the Adjust Width or Adjust Height box and enter the value. When the Keep Proportions option is checked, one side can be adjusted.

Rendering: 1. Set the specular brightness by sliding the cursor. This is the color's light reflection on the part generated by a light source. For plastic material, the specular color is the same as the diffused color; for metals, the specular color is white.

2. Set the specular spread by sliding the cursor. The brightness of the material is changed. The higher the brightness, the more the material reflects lights.

Example of a decal applied to an object.

Modifications / Additional information: You can modify using the popup menu or the operations tree.

Machining process

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This command allows to assign a machining process (name of a process and a color) to several faces. These processes are then known by TopSolid'Cam.

Creation stages / Use: Click the icon or select the Shape > Other operations > Machining process... command from the drop-down menu. 1. 2. 3. 4.

Select the different faces where a process has to be assigned. Select the Machining process document in the drop-down list. Select a process in the drop-down list. Validate.

A Machining process document must have been created.

The machining process can also be assigned directly from the advanced option of Drilling, Group of drillings and Pocket commands.

Available Options:

Entry points: Allows to define the entry points of the machining process. Give the diameter and direction of the entry points, then select their positions. These entry points could be projected in a drafting view. Attributes of these entities could be setting in the view style (Lines option). They could be used by a drilling note. They could be included into a drillings table (Identification tab of drillings table). The entry points can be displayed/hidden into the graphic area by using the display mode Create MF or on the Home Tab icon bar.

available in the Edition menu

Modifications / Additional information: The process color is not displayed when using the realist rendering.

Face modification Links / Videos:

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This command changes the faces by re sizing or moving them. It is useful, for example, to modify imported parts. For example, it is possible to re size a hold by changing its diameter and moving it.

Creation Stages / Use: Click the icon or select the Shape > Other operations > Faces modification... command from the drop-down menu. 1. 2. 3. 4.

Select the Re size or Move option. Select the faces to modify. Enter the values. Validate.

Modifying faces creates a problem in the operations tree. It is then possible to edit the command to change the value.

Available Options: Re size: For cylindrical and spherical faces, this option allows a spherical or cylindrical (or fillet) face's radius or diameter to be changed by entering either the desired radius/diameter by

clicking Parameter or offset with respect to the selected face by clicking offset. For conical faces, this option changes the angle or allows you to get an offset with respect to the selected face. The offset option lets you offset any type of face by providing an offset value.

Displace Drag: This option moves the translation face by "dragging" the material. You then have to select the direction and enter the value. Revolve: This option moves the face by rotating it, "turning" the material. You then have to select the axis of rotation and enter the angle. Draft: This option is for modifying a face by adding or modifying a draft. You must then select the reference plane and enter the draft angle.

Modifications / Additional information: Modifying, deleting, activating, deactivating, and color changing are possible from the operations tree or the popup menu from the graphic.

Repetition

This command repeats operations or faces.

Creation stages / Use: Click the icon or select Shape > Repetition... from the dropdown menu. 1. Select faces or operations to repeat depending on the type of elements chosen (operation or faces). 2. Choose the pattern to use. 3. Validate the command with the button

Available Options: Selection: You can choose to repeat operations (pockets, drillings, ...) or faces.

Some operations that require reference faces (such as chamfers, fillets, threadings, and tappings) cannot be repeated by themselves. They must be repeated with their support (boss, pocket, hold, etc., on which they are supported).

Replay operations:

If you have chosen to repeat this operation, this additional option will appear. If this option is checked, the operation is recalculated for each entity. If it is not checked, the geometry of the operation is repeated identically. For the example below, the operation to repeat is a boss of which the height is defined up to the plane of the chamfer (continuity of the chamfer plane). Replay operations

Without replaying operations

With the Replay operations option, the geometry is recalculated n times, which can cause increased computation time. However, if this option is not active, sets of faces for selected operations must all be adjacent (in contact). If some faces are not in contact with the rest of the section, the repetition cannot be carried out.

Fast repetition: This option allows for faster repetitions in simples cases, because there is no control. However, there are also more errors (ex. if the repetition is outside of the part).

Fast repetition copies faces. You have to choose sides to repeat. For example, for a boss with chamfer to repeat, you must select the boss AND the chamfer. To be able to use this option, there cannot be any "holes" in the faces. For example, if one of the repeated bosses is not on the same support face (the face is intersected by a groove and the boss must be on two sides), or if it is on the exterior of the part, using this option makes repetition invalid.

Advanced Options: The Verify the results option allows you to verify the consistency of the repetition of the result.

It is advised to keep the Verify the results option checked, even if the computation time is increased.

Attributes

This command, available only through the popup menu, allows you to change the color of an operation.

Creation Stages / Use: Select Attributes... from the popup menu from the operation in the operation tree or directly on the faces generated by the operation to change the color. 1. Select the color for the operation. 2. Validate.

When a color has been placed on an operation, it can be changed by selecting the function again. To remove the color from the operation, you must rerun this function and click the black cross. Otherwise, you can use the life color function, available from the popup menu, for operations that have an assigned color.

Compare

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This command is for geometrically comparing and imported shape with a new version of the shape.

Creation Stages / Use: Select Shape > Comparison > Compare... from the drop-down menu. 1. 2. 3. 4.

Select the shapes to be compared. Select the document containing the comparison shapes. Select the news shapes of this document. If the shapes are not positioned identically with respect to the absolute frame, define a transformation to replace them.

When the new shape is selected, TopSolid automatically divides the window into two panes to view the compared shape alongside the new shape. In the view of the background document of the new part, TopSolid displays all entities (frames, points, ...). They can be used to define the transformation. In the editing document, the cursor is automatically positioned before the first modification operation of the shape to compare. It allows to use a point or a frame for the transformation. The Face-Face transformation is for easy displacement. If faces on both shapes have the same definition (same support but

different restriction or symmetry), TopSolid could not be able to detect the wanted transformation.

Hide: The box allows to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Advanced options: Linear and angular tolerances: These values are used to refine the comparison of shapes.

Quick comparison of Bsplines: Option checked by default for faster processing of B-splines faces. By disabling this option, additional nodes will be included in the processing, which will take longer to obtain a result.

Verify the geometry type: Allows the geometry type to be taken into account when comparing shapes. In the example below, if this option is disabled, all of the faces will be considered to be similar. However, turning on geography verification makes it possible to differentiate the cylindrical face from the planar face and group them in the face folder of the verification result.

Similar faces: Allows similar faces to be considered. Advanced search: this mode searches for every types of correspondence to find at best a correspondence between faces of the 2 shapes corresponding to a part family and for example to topologically identify an operation displacement like a drilling, a boss or a pocket. Search faces with: More active loops: If the face to be compared has more loops than the new face, these faces will be considered to be similar. Less loops: If the face to be compared has fewer loops than the new face, these faces will be considered to be similar. Different loops: If the face to be compared has loops with a different geometry or position, the faces will be considered to be similar. No active option: This looks only for faces that are completely identical. No concept of similar faces.

5. Switch to the next stage to get the results of the comparison.

In the comparison result, TopSolid displays the faces lists with 3 categories.

Similar faces: lists faces for which TopSolid has found correspondence from on shape to the other. Different faces on shape to compare: lists faces of the shape to compare which TopSolid has not found correspondence with faces of the same shape. Different faces on new shape: lists faces of the new shape which TopSolid has not found correspondence with faces of the shape to compare. The Zoom contextual command is available by selecting a pair of faces. In the comparison result box, a new transformation can be defined. It is applied to faces which have not been associated to start again the comparison on these same faces. This may be useful if the same operation exists between two shapes with a different positioning (ex. a boss). The transformation allows them to be superimposed to thus consider the faces to be similar. After validation of the dialog, results can be retrieved in the Comparison s folder of the entities tree.

It is possible to compare a solid shape with another solid shape or several surfacic single-face shapes with several other surfacic single-face shapes (for the comparison of a non-sewed import). The comparison does not work if several solid shapes or with several faces are selected.

Replace

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This command makes it possible to compare and replace faces from a shape imported from a new version of the same shape.

Creation stages / Use: Select Shape > Comparison > Replace... from the drop-down menu. 1. Select the shape to drill. 2. Select the new shape. 3. If the shapes are not positioned identically with respect to the absolute frame, define a transformation to replace them.

When the new shape is selected, TopSolid automatically divides the window into two panes to view the shape to be replaced alongside the new shape. In the view of the background document of the new part, TopSolid displays all entities (frames, points, ...). They can be used to define the transformation. In the editing document, the cursor is automatically positioned before the first modification operation of the shape to replace. It allows to use a point or a frame for the transformation. The Face-Face transformation is for easy displacement. If faces on both shapes have the same definition (same support but

different restriction or symmetry), TopSolid could not be able to detect the wanted transformation.

Advanced Options: Verify the geometry type: Allows the geometry type to be taken into account when comparing shapes. In the example below, if this option is disabled, all of the faces will be considered to be similar. Turning on geography verification makes it possible to differentiate the cylindrical face from the planar face and group them in the face folder of the verification result. In this situation, the user must manually replace the faces and edges of faces that are considered to be different. Faces that are considered to be similar will automatically be replaced when validating the replacement box.

Linear and angular tolerances: These values are used to refine the comparison of shapes.

4. Switch to the next stage to open the results of the replacement. Transformation: In the result box, a new transformation can be defined. It can be

useful if a same operation exists between 2 shapes but differently positioned (eg. a boss), the transformation allows to superpose them and then consider their faces as identical.

5. Switch to the next stage to open the Replace dialog, and then replace the faces and edges. Document: If needed, select a document where the shape is used, a list of used faces and edges is displayed. Activate the filed of the geometry to replace (face or edge) and select the new corresponding geometry for the new part. To help to understand the geometry correspondence, TopSolid displays with dash, the face or edge to replace on the new part.

Preserve new colors: When the replacing part gets colored faces, this option allows you to keep them during the replacing.

Faces / Edges: When a face or an edge is selected on the shape to replace (from the graphic area) it is selected in the table. If needed a face or an edge can be selected on the new part. In tables where faces or edges are not found on the shape to replace, the Zoom contextual command is available on the topology. It is possible to manage the transparency of the part to replace, with a temporary effect during the replacement.

Associative: This check allows to create a replacement operation. When there are too many faces/edges, this mode allows to create a Replacement operation, which can be edited later to finish to reconnect topologies. It is recommend to basify the shape when the work is done while the operation needs to save the geometry as well as

lists needed for replacement. There is no need to keep these informations.

Shape to replace display: For faces: If the face is transparent, check the "Opaque" option to better distinguish faces. Their color can be changed. By unchecking the "Color rehooked faces" option, faces already rehooked will not be colored to better visualize remaining faces to process. For edges: The type of lien and also its color can be changed. By unchecking the "Color rehooked edges", edges already rehooked will not be colored to better visualize remaining faces to process.

6. Validate by clicking

.

Pipe

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This command allows you to create a surface shape or solid shape by making a selection (opened or closed) run along a trajectory.

Creation Stages / Use: Click on the icon or choose the command Surface > Pipe... or from the drop down menu (or Modeling > Local Shapes > Pipe in the assembly document). 1. Select the type of piped shape you wish to create. Wire shape:

Tube shape.

Swept section.

2. Select the path (or trajectory) 3. Then define the parameters according to the type of pipe chosen in stage 1

Available Options: Wire shape: This mode allows you to create a wire with the desired diameter along a path.

If you check the Surfacic check box, the shape obtained will be a hollow shape without thickness and will not be a full wire.

Tube shape: This mode allows you to create a tube with the desired diameter and thickness.

Swept section: This mode creates a shape by making a section run along a path.

The Invert path option inverts the direction of the course along the path. On an open path, the section must be positioned on one of the extremities. On a closed path, the Path origin option allows you to define the path origin which must be defined at the section in order to obtain a coherent result. Section: The section can be designed in place by clickng the "+". It can be opened or closed. Section position: This option allows to specify the section position on the path, even if it is opened. It allows to create a pipe without having to position the section on the origin. If the section is not planar, the user has to specify the position on the path to obtain the wanted result.

Alignment: This command allows you to define how the section travels along the path. Normal: The section moves while remaining normal to the path. Vertical: The section moves while keeping an orientation in relation to a defined direction.

Parallel: The sections moves in parallel to its original orientation. Faces: The section moves along the normal of selected faces.

To create a pipe normal to faces, you must have faces defined all along the profile. In the cas below, the cylinder must be longer than the spiral.

You will find more details about this option on the Section alignment page. Surface: By checking this option, the shape obtained will be a hollow surface without thickness and not a full shape.

Advanced Options:

Division of minimal faces. This mode allows you to smooth the section and the path in order to obtain the face minimum on the resulting form.

Division of the faces into columns, according to the segments of the section. Only the path is smoothed in order to obtain faces for each segment of the section.

Division of the faces into the grid, according to the segments of the section and of the path. No smoothing is performed, and a face grid is generated by the segments of the section and the path.

Corners type: If the path is not continue in tangency, corners can be sharp or rounded. Simplify the geometry: This option allows to convert to flat, cylindrical or conical faces, faces of the pipe which are similar. Repair self-intersections: This option deletes the self-intersections between faces of the shape. Create sections: This option allows to create different sections of the surface to create. The number of wanted sections has to be entered.

Limits: This option allows you to define pipe limits by adding a start and an end point on the path.

The start point can be the section origin.

Example of a pipe with a start and end limit.

With the Swept section mode, the start point can only be selected if the section is not on the origin of the path and this point will have to be before the section position. Start and End points can also be defined when using the Wire shape and Tube shape modes.

Twist (only for pipe on section): This option allows you to apply a rotation to the section when sweeping along the path. The Initial length and Final length options determine the length at the path start and end on which the section will not be turning. The rotation is therefore applied along the remaining length of the two. The Initial angle and Final angle options determine the angular orientation of the section at the path start and end.

You can provide a final angle greater than 360°. In this case, the section will make more than one turn around the path.

If the path is closed, the total rotation angle must be a multiple of 360°

Scale (only for pipe on section): This option allows you to apply a reduction or increase of the size of the section during the sweeping along the path. The Initial length and Final length options determine the length at the path start and end on which the section will not be changing. The reduction/increase of size is therefore applied on the length remaining between the two. The Initial factor and Final factor options determine the scale factor of the section at the path start and end.

If the path is closed, it is not possible to use the scale (the end section must be equal to the start section).

Swept Links / Videos:

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This command allows you to create a surface or solid shape by making one or more sections (open or closed) run along one or two trajectories.

Creation Stages / Use: Click the

icon or select the Surface > Swept... command from the drop-down menu.

1. Select the path or paths. 2. Then select the sections and their hooking points on the paths.

Available Options: Paths: This path corresponds to the trajectory followed by the sections in order to generate the surface. By checking the "Second path" check box, you can select a second trajectory. The shape is thus created by making the sections travel between two paths by applying a scale on the sections in order to follow the evolution of the paths. One path

Two Paths

An arrow is hooked to the start of each path and thus indicates the travel direction. When two paths are used, the travel directions must be the same on each path. To invert the direction, simply double-click the arrow of the path in question.

Sections: This option allows you to define the section(s) of the swept shape. The sections must be designed in place. They must be planar and all be open or all be closed For each section, it is necessary to define: - the profile to use as a section - its position and hooking point on each path.

The positioning point corresponds to the point that will act as a reference to calculate the movement of the section along the path. The "Automatic hooking" allows you to automatically use the intersection point, detected between the plane of the section and the path, as the positioning point.

Warning, if the plane of a section intersects the path several times (in the case of a closed path for example), the point chosen by the software might not be correct. Therefore you should verify which point has been chosen by using the list of sections in the dialog.

On each section an origin and a "drawing direction" of this profile represented by a point and arrow are defined.

The coefficient (variable from 0 to 1) determines the origin position of the profile (0: at the start; 1: at the end). Double-click the numeric value to modify it. By double-clicking the small symbol in front of the coefficient, you can change the definition mode of the origin position.

The "point" mode allows you to select a point on the profile as being the new origin rather than using a coefficient. In order for the swept shape to be created correctly and for it not to twist, the section origins must be aligned.

Alignment: This option allows you to define how the section travels along the path. Normal: The section moves while remaining normal to the path. Vertical: The section moves while keeping an orientation in relation to a defined direction. Parallel: This section moves in a manner parallel to its initial orientation. You will find more options on the Section alignment page.

Surface: By checking this option, the shape obtained will be a hollow surface without thickness and not a full shape.

Limits: This option allows to define limits of a swept surface by adding start and end points on each path.

Example of a swept surface with start and end limits.

Start points can only be selected if the first section is not on the origin of the path. These points have to be before or on the first section position. End points have to be on or after the last section position.

Advanced Options: Synchronization: The sections Synchronization define the way TopSolid make the sections corresponds with Free: This test mode adapts sweeping best between section using a combination of va Local: When you use local synchronization for the sweep, this means that when the sh length of each one. Arc length: When you use arc length synchronisation for the sweep, this means that w nature settings of the sections. Example: The parametric extension for a line is [0;1] (length) The parametric extension for a circle is [0;360] (angle)

Minimal division of faces. This mode allows you to smooth the section and the path in order to obtain the face minimum on the resulting form.

Division of the faces into columns, according to the segments of the section. . Only the path is smoothed in order to obtain faces for each section segment.

Division of the faces into the grid, according to the segments of the section and o the path. . No smoothing is performed, and a face grid is generated by the segments o the section and the path.

Mixing: This option allows you to determine the manner in which the shape changes from one section to another. Section mixing. Repair self-intersections: This option deletes auto-intersections between surfaces of the shape when this is the case. Create sections: This option allows to create different sections of the surface to create. The number of wanted sections has

Lofted shape

This command allows you to create a shape by selecting a profile, segment or face.

Creation Stages / Use: Click on the icon 1. 2. 3. 4.

or choose the command Surface > Lofted... from the drop down menu.

Choose the type of loft: closed or open (periodically or not). Select loft profiles. Choose the synchronization mode. Choose if you want the lofted shape to be surfacic or solid.

To define the sections of a loft, it is possible to select a sketch, a segment of a sketch, or a planar face (only for the extremities sections of the loft)

Available Options: Closed: This option creates a periodic loft, turning back on itself. TopSolid also links the first and the last section. No option

With the option

Surfacic: If you check this check box, then the lofted shape will be surfacic and open at its extremities

Guides: Guide profiles constrain the lofted shape to change along the profile between sections. No option

With the option

Options on section labels: On each section, there is an arrow and a label.

The arrow's hook point corresponds to the origin of the section, and the arrow indicates the profile's direction. All sections must be in the same direction. You can either edit the value in the label (Coefficient varying from 0 to 1), or dynamically move the point indicated by the label by dragging it with the mouse. Another way is to double click the symbol of the label to switch to point, double click again to edit the label and select a point.

The position of the origins on each section is very important and greatly influences the final result of the lofted shape.

Tangency and curvature constraints (popup menu on the section): To use this option, right-click the desired section and select "Add Constraint". This option allows you to apply a constraint to the lofted shape at this section. There are two types of constraints: Curve: The lofted shape is adjusted so as to be tangent to the reference face and so as to follow the curve of the latter. Tangency: The lofted shape is adjusted to be tangent to the selected data reference face or plane.

Double click on the plane or surface icon in the label to change from one to the other.

A coefficient defines the magnitude of the tangency. The higher the coefficient, the more the tangency is pronounced. Constraint = None

Constraint = Tangency

Constraint = Curvature

Guides synchronization: The synchronization represents the way TopSolid make the section correspond with each other. Free: This test mode adapts sweeping best between section using a combination of various methods. Curvilinear: When you use curvilinear synchronization for the sweep, this means that when the shape is created, the sweep on the curves in done in proportion to the length of each one. Parametering: When you use parametric synchronisation for the sweep, this means that when the shape is created, the software tries to correspond to the nature settings of the sections. Example: The parametric extension for a line is [0;1] (length) The parametric extension for a circle is [0;360] (angle)

a: Line : parametric extension [0;1]

b: Arc: Parametric Extension [0;54]

With the local and arc length modes, the edges of the obtained surface are created by approximation with some BSpline (curve), by following either the curvilinear abscissa either the reference profile arc length. With the free mode, TopSolid does not use the approximation with BSplines to ensure that the simplification (lofted advanced option) gives better results. Only exceptions where the approximation is used in free mode: In the profile/profile correspondence if the number of profiles segments is different. In the point/point correspondence if the number of segments between consecutive points is different.

Correspondence points: This option defines points of correspondence between sections in order to structure the change of the lofted

shape. You can: add a new set of correspondence points delete an existing correspondence insert a new correspondence. When you enable this option, a box appears, where you add all of the points (in order) for a set of correspondences. Once the set has been defined, validate it with . You can then select the next list of points. Once all correspondence point sets have been defined, click in the box to finish defining correspondences.

The set of correspondence points must be defined in order, depending on the profile direction. Each point in a set must also be selected in the same order as the sections.

Correspondence: Different types of correspondence are: Profile to profile: During the shape creation, TopSolid overall matches profiles regarding their built settings (example: a circle is parameterized by an angle). It is the default mode, it usually gives satisfying results. Segment to segment: During the shape creation, TopSolid tries to match two by two segments of each profiles. The result is a surface for each pair of segments. This option is only available when profiles have the same number of segments. Point to point: If this mode is selected, you have to select manually corresponding points two by two between profiles.

With the profile/profile correspondence, if you select guides curves, the synchronization will be applied by section (by intersection between guides curves and profiles defining correspondence points). With other correspondences (Segment to segment and Point to point) the user has to check that guides curves don't intersect the correspondence.

When adding a batch of points with the contextual menu, TopSolid updates the point position during the first profile selection. TopSolid also checks the consistency of other points during the correspondent point selection on the second profile. All correspondences in this dialog are saved. It allows to switch from points/points to profile/profile and switch back to points/points.

Division of faces: Minimal division of faces. This mode allows you to smooth the section and the path in order to obtain the face minimum on the resulting form.

Division of the faces into columns, according to the segments of the section. Only the path is smoothed in order to obtain faces for each segment of the section.

Division of the faces into the grid, according to the segments of the section and of the path. . No smoothing is performed, and a face grid is generated by the segments of the section and the path.

Derivation magnitude: This option allows to smooth or not the derivation magnitude between profiles. Single: the derivation magnitude is alone.

Smooth: the derivation magnitude is smoothed between profiles for a more aesthetic result.

Simplify Surfaces : This option simplifies the geometry of some surfaces. By default, surfaces from this command are b-spline surfaces. According to the reference profiles, some surfaces could be simplified into planar, cylindrical or conical surfaces.

Filled Links / Videos :

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This command allows to create a surface based on edges and/or profiles defining a closed path. It is also possible to specify inner constraints (points or profiles).

Creation stages / Use: Click the icon or select the Surface > Filled... command from the dropdown menu. 1. Choose the boundary edges continuity mode. 2. Select the boundaries constraints 3. Validate.

Available options: Boundary edges continuity: This option allows to specify the continuity mode between the filled surface and the neighboring faces. None: no tangency or curvature constraint is used on this edge. Tangency: the surface will be tangent with the neighboring face along this edge. Curvature: the curvature radius of the neighboring face is used to define the curvature of surface.

Boundary constraints: Cette option allows to define the limits of the surface. They must define a closed path. If you select a boundary edge, the face of this edge is automatically used as reference for the continuity. If you select an inner edge of a shape or a profile, the default continuity will not be applied (so none continuity defined on this selection). If required, the user will have to define a special constraint on this selection. If you select a closed edge or profile among others, it will be automatically trimmed with the neighboring selected boundary (the picking point will be used to define the part of the profile to keep). At the first selection,if the edge or profile is opened, two handles are displayed on the extremities. It is possible to drag them along the next required edges/profiles to keep up automatically thee selection.

Special constraints: This option allows to define a specific continuity constraint on some edges of the surface: Either by using the contextual menu on the edge, and selecting the required continuity in the "Selection" section of the menu. Or by selecting the edge as special edges in the dialog and editing the label to choose the required continuity. In the case of an inner boundary or a profile, it is also necessary to select the face to use as reference for the continuity constraint. To do this you need to double click on the label with the text "Select a face".

Inner constraints: Type : if you activate the inner constraints, you need to choose if you want to give profiles or points as inner constraints. Profiles: The selected profiles must respect one of these conditions:

- either they are guide profiles: the profiles must not intersect themselves. - or they define a meshing: all the profiles must intersect to get a netting. The user do not need to specify which mode to use (guide or meshing), it is automatically detected according to the selected profiles. Points: You can select one or several points.

Without inner constraints

With points as inner constraints

Constrained

This command allows you to create a surface constrained by boundary curves, constraining curves and constraining points.

Creation Stages / Use: Click on the icon or choose the command Surface > Constrained... from the drop down menu. 1. 2. 3. 4.

Check Initial surface if needed. Check the types of constraints that you wish to use. Select the profiles or points for each one of the constraints. Validate.

Available Options: Initial surface: The initial surface allows to define a parametrization by projection of points on the surface.

Curves: Check the type(s) of constraints that you wish to use for your surface. Constraining boundary curves: All selected profiles must define a closed bound. These curves determine the outer bounds of the surface.

If the selected cruves don't define a close bound, the Close boundaries allows to automatically create line or a bspline curve between the origin of the first selected curve and the extremity of the selected curve. In case of bspline curve, the graphical handles allow you to set the tangency (direction and ratio) according to the extremities. Constraining curves: The resulting surface will pass through all of the curves displayed in this list. Constraining points: The resulting surface will pass through all of the points displayed in this list.

You can remove elements from the list by selecting them and then by using the "Delete" key on your keyboard. To select several elements in the list and to delete them all at once: "Ctrl + Left-click": Each click on an element in the list adds it to the selection. "Alt + Right-click": selects all elements included between the element clicked and the previously current element in the list.

Advanced options: Fast mode: The constrained surface calculation is optimized for the performance (at the expense of quality).

Smooth mode: The constrained surface calculation is optimized to produce a better quality surface.

Modifications: It is not necessary to use all of the types of constraints in order to build a surface. You can use only one of the three if you so wish.

Additional information: When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Blend

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This command can create join surfaces between sets of faces

Creation Stages / Use: Click on the icon menu.

or choose the command Surface > Blend... from the drop down

The command has three ways to create a join: Join between faces: allows to create a blend surface between 2 batches of faces. 1. Select the batch of faces from the first side. 2. Reverse the direction, if necessary. 3. Select the batch of faces from the second side. 4. Reverse the direction, if necessary. The arrows indicate the side when creating the join. 5. Choose the radius type: Constant radius: The entered value is constant for the entire join. Constant length: The length (shortest distance between the two join edges in contact with the set of faces) is constant for the entire join. Variable radius: The fillet radius will change between r11 and r12 entered radii. r11is the radius at the start of the intersection edge, and r12 is on the other side. Conical radius: The conical radius is created by entering two radius values for each side of the intersection edge. r11 will be the radius at the start of the edge on the side of the first batch of faces, and r12 will be the radius at the end of the edge on the same side. r21 and r22 will be the equivalents on the second batch of faces. 6. Validate by clicking .

Three face join: allows to create a blend face passing by 3 batches of faces. 1. Select the batch of faces from the first side. 2. Reverse the direction, if necessary. 3. Select the batch of faces from the second side. 4. Reverse the direction, if necessary. 5. Select the batch of faces from the third side. 6. Reverse the direction, if necessary. The arrows indicate the side when creating the join. 7. Validate by clicking .

Face profile join: allows to create a fillet between a batch of faces and a profile. 1. Select the batch of faces from the first side. 2. Reverse the direction, if necessary. The arrows indicate the side when creating the join. 3. Select the profile. 4. Fillet: Enter the value of the radius. 5. Validate by clicking .

To select all of the tangent faces rather than selecting them one by one, use the rotative selection on one of the faces.

Available Options: Section: Loop: A join between ball faces is created by making the intersection of the faces a sphere. The definition of the normal for the section planes is not requested for a ball join. For a ball join with a curved section shape, you must enter a curvature value. A value of 1 is equivalent to the conical section shape. The closer the value is to 0, the more the curvature will move to the right.

Section Shape: Conical

Section Shape: Curvature

Section Shape: Chamfer

Disk: The join between disk faces results from making the intersection of faces a disk. This type of join must be defined as a guide profile for the disk. The disk's normal is defined by the tangent to a given profile. The profile must be able to define a normal at each point of the join. The green profile or edge defines normal for the section plans. The geometry of the join is directly influenced by this normal.

The guide profile "follows" the intersection.

The guide profile is whatever

Constraints: (only for the join between faces) Constraints must be given by the edges of the element. It is therefore necessary to print the constraint profile(s) to the face(s). The radius defines the maximum radius for the constrained join. It must therefore be larger than the greatest distance between the intersection of the two faces and the constraint edge. Otherwise, the constrained join will be constant for distances greater than the given radius. None: Imprinted profiles are not taken into account.

Symmetrical edges: The selected printed edge will be made symmetrical with the intersection edge.

Edges - Edges: The two imprinted sides will be taken into account for the join.

Edges - Radius: The join will have the radius entered, and it will be trimmed by the selected imprinted profile. The radius must be less than the greatest distance between the impression and the intersection edge for the various faces.

Advanced Options: Trimming type: (only for the join between faces) defines the trimming of the join.

None

Shortest

Longest

Surface

Repair auto-intersections: Makes it possible to repair self-intersecting joins. In the example below, it is not possible to make the join without activating this option.

No option

With option

Overlap: (only for blend between faces) allows to extend the blend after an interruption in either face (pocket for example).

No option

With the option

Propagate to discontinuous edges: (only for blend between faces). Allows you create the join, even if there is a square angle between faces on the same side. The input angle must be at least equal to the angle between the two faces. In the example below, just one vertical face was selected, and the entered angle was 15°. The Angular tolerance allows to enter the angular tolerance to respect during the discontinuous edges propagation.

In this case, the fillet will be created only if the angle is under the tolerance limits.

No option

With the option

Point: In some cases, it could be several possibilities. The point allows to select on which side applying the fillet.

Without selecting a point.

By selecting a point.

Normal

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This command allows you to create a perpendicular shape, a tangent shape, or a shape with a given angle with respect to the perpendicular of a face.

Creation Stages / Use: Click on the icon drop down menu.

or choose the command Surface > Normal... from the

1. Select the face creation mode: By Profile: The face is created using a profile (border edge, edge from an impression, projection of a sketch, etc.), located on the reference face. 1. Select reference faces. 2. Select the profile. By Isoparametric: The face is created using isoparametric curves from the reference face. 1. Select the face. 2. Select U or V and its factor (between 0 and 1).

2. Enter the length of the face to create. 3. Choose the type of surface to create: Tangent: The face is created on the profile or curve that is isoparametric and tangential to the reference face. Perpendicular: The face is created on the profile or curve that is isoparametric and perpendicular to the reference face. Angle: The face is created on the profile or isoparametric curve with a given angle with respect to the perpendicular to the reference face.

4. Validate with the

button.

The profile must absolutely be the reference face.

To select all tangent faces, use the rotative picking.

Available Options: The Reverse option allows to change the surface side or double click the yellow arrow.

Faces

This command copies one or more faces from a shape, in restricted or unrestricted mode.

Creation Stages / Use: Select the Surface > Faces... command from the drop-down menu. 3 copy modes are available: Face mode: This mode allows to rapidly create a copy with extended limits or identical to the original. Face with trimming path mode: This mode allows to copy a face by using edges as complement to define the limits of the copy. Complementary Face mode: This mode allows to create a surface from a hole's edges.

Advanced options: Layer: You can specify a layer to which faces will be copied.

To select all tangent faces, use the rotative picking.

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This command allows you to create the middle or the offset surface between 2 sets of faces.

Creation stages / Use: Click the icon or select the Surface > Middle... command from the drop-down menu. 1. Select the faces on the first side (shown as blue dashed lines in the images below). 2. Select the faces on the second side (shown as magenta dashed lines in the images below). 3. Choose the computing method: Middle surface: compute the exact middle surface (the number of selected faces should be the same on each side).

Offset surface: the surface is created by parallelization of the first set of faces.

In this case, the positioning value is computed from the minimum distance between the 2 sets of faces. 4. Give the position of the surface by entering a value between 0 and 1. 5. Confirm the creation of the middle surface with the button.

The rotative selection (or rotative picking) allows you to select all

the faces tangent to the selected face. Positioning coefficient: a value close to 0 allows you to locate the surface near the first set of faces, a value of 0.5 allows you to locate the surface at the middle and a value close to 1 allows you to locate the surface near the second set of faces.

This command doesn't allows to get the middle face between to sets of non parallel faces.

Available options: Pairs: This dialog allows to display the matching between selected faces. A right clic displays the Add new pair command which allows you to compute a middle surface from new sets of faces.

Advanced options: The Trimmed option allows you to get a surface with the same limits than the reference faces.

Flat

This command allows you to create a flat surface from a closed planar sketch.

Creation Stages / Use: Click on the icon or choose the command Surface > Flat... from the drop down menu. 1. Select the sketch.

It is possible to select only one profile of a sketch (in the case of a sketch with several concentric closed profiles for example).To do this, simply perform a rotating picking.

Available Options: Offset: This option allows you to obtain a "hollow" flat shape. To do this, you can provide a thickness/offset distance in relation to the sketch by using one of the following modes: Centered: The value given is distributed on both sides of the sketch. Outwards: the flat shape is created towards the exterior of the sketch. Inwards: the flat shape is created towards the interior of the sketch.

Both sides: you are able to enter a different value for each offset side. The Rounded joins check box allows you to add fillets using, as the radius value, the outer thickening value.

A few examples of results with regard to the "offset" option. Without the offset option.

Outwards

Centered

On both sides

Advanced Options: Fast : When the sketch contains many profiles, the fast mode allows to generate operation almost immediately. This allows for example to produce easily a plate with many holes (one

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This command allows to create an extruded shape with several draft angles and fillets on convex portions.

Creation stages / Use: Click the 1. 2. 3. 4.

icon or select the Surface > Matrix... command from the drop-down menu.

Select the profile to extrude. Select the vertical extrude direction. Enter the distance. Enter the draft angle.

Available options: Origin: Possibility to modify the origin and direction of the profile. This could be useful if draft constraint is added to the matrix in order to help segments selection.

Conical fitting: Using this option, a conical fitting will be added to all convex points of the profile.

Surfacic: Possibility to create a surfacic shape using this option.

Constraints: On segment :

Addition of a constant draft from a selected segment to the end of the profile. Addition of a variable draft with start angle and second angle (end angle).

The draft is applied from the first selected segment to the end of the profile (according to the origin and profile direction). Right click on a variable draft gives access to the Until command allowing to apply the draft between to selected segments. After the end segment, the final angle will be applied to the next segments until the end of the profile. Constraint available on arc only. The Isometric constraint apply the same radius from the top to the bottom of the matrix. Constraint available on arc only. The Forced constraint allows to specify the radius value at the opposite of the profile. On vertex :

If the Conical fitting option is not activated you will be able to apply a conical fitting on a selected vertex. A conical fitting cannot be applied with the following cases: Draft angle is not the same on the right and on the left of the vertex. Draft angle is null. The vertex is concave. If the Conical fitting option is activated you will be able to apply a sharp fitting on a selected vertex.

Modifications / Additional information: Labels are available on the matrix in the graphic area with constraints settings. Constraints can be modified using these labels by double-click and/or right click on them.

Surface by formula

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This command allows to create a surface with 3 formulas

Creation stages / Use: Click the 1. 2. 3. 4. 5. 6. 7.

icon or select the Surface > Surface by formula... command from the drop-down menu.

Enter formulas for X(u,v), Y(u,v) and Z(u,v). Enter Minimum and Maximum intervals of u and v. Check if intervals are Periodics. Reverse intervals if needed Select the positioning frame of the surface. Enter the modeling tolerance. Validate by clicking .

It is important to systematically specify the unit of entered values in expressions. Otherwise, u and v parameters have no unit.

Available Options: Periodic: If the edge following u or y has to be closed, you have to check periodic. For example, a torus (see below) the section (u) is closed therefore periodic , the trajectory is cylindric (also closed, therefore periodic).

Reverse: u and v are inside the interval [minimum value, maximum value]. By clicking the Reverse option, the interval taken into account is [maximum value, minimum value]. It is equivalent to replace u by u max - u + u min.

Tolerance: This option allows to modify the modeling tolerance. By default this modeling tolerance is set in the document options.

The more the tolerance is precise, the more the geometry will be precise. The default value is a good compromise between geometry accuracy and performance.

A finer tolerance (for example 0.01 instead of 0.1) needs more important calculation time. If the modeling tolerance is modified in the document options, manually modified tolerances with this command will not change.

Simplify: To measure the surface quality, TopSolid calculates the distance between points on the created Bspline surface and those calculated by the formula. If the tolerance is not reached for some points of the Bspline surface, TopSolid inserts parameters where the accuracy is not reached and calculates again the surface. TopSolid iterates several times to locally refine the surface and reach the accuracy. To guarantee a better surface quality, TopSolid measures several points per tile (a tile corresponds to u which varies between [ui ; ui+1] and v which varies between [vj ; vj+1]), so 9 points are positioned at ¼, ½ and ¾ of intervals The quality measures uses a lot of system resources. If the "Simplify" option is not checked, the precise mode is activated (measure of 9 points per tile). If it is checked, the approximative mode is activated (measure of 1 point per tile).

For below examples, the result is the same with or without the option checked (except for the "eggs box"), but the calculating time is faster with the option checked.

Examples: Torus: Formulas:

Values signification:

Result:

X(u,v) (30mm+5mm*cos(u*360°))*cos(v*360°) Y(u,v) (30mm+5mm*cos(u*360°))*sin(v*360°) Z(u,v) 5mm*sin(u*360°) u and v intervals u and v are periodics, their minimum value is 0, their maximum is 1 (without unit)

Helical: Formulas: X(u,v) 1mm*u*cos(v*360°) Y(u,v) 1mm*u*sin(v*360°) Z(u,v) 5mm*v (5mm is the pitch) u and v intervals u and v aren't periodics, u changes from 0 to 2 (which is the helicoid radius), v changes from 0 to 5 which is the number of turns.

Values signification:

Result:

4 is the diameter (the entered radius is 2) 5 is the pitch

Hyperboloid: Formulas: X(u,v)

Values signification:

Result:

3mm*sqrt(1+u*u)*cos(v*360°) Y(u,v) 3mm*sqrt(1+u*u)*sin(v*360°) Z(u,v) 5mm*u (5mm is the base height) u and v intervals v is periodic, u changes from 0 to 3 (which is the helicoid radius), v changes from 0 to 1 which is the number of turns.

6 is the diameter (the entered radius is 3 for X and for Y) 15 is the height (see Z)

Flattened sphere: Formulas:

Values signification:

Result:

X(u,v)

50mm*cos(v*360°)*cos(u*360°)+u*1mm Y(u,v)

50mm*sin(v*360°)*cos(u*360°)+u*1mm Z(u,v)

10mm*sin(u*360°) u and v intervals u changes from 0 to 0.25, v from 0 to 1.

50mm is the radius ( X and Y) 10mm is the height (following Z)

Hyperbolic paraboloid: Formulas: X(u,v)

50mm*u Y(u,v)

Values signification: 50mm is the biggest radius 20mm is the smallest radius

20mm*v Z(u,v)

20mm*(u*u-v*v) u and v intervals u and v change from -1 to 1.

Horopter: Formulas: X(u,v)

Result:

u*cos(v*360°)*50mm Y(u,v)

50mm*tan(v*360°) Z(u,v)

50mm*u*sin(v*360°) u and v intervals u changes from -1 to 1, v from -0.1 to 0.1

Part of a sphère: Formulas: X(u,v)

Result:

Result:

50mm*cos(u*360°)*cos(v*360°) Y(u,v)

50mm*sin(u*360°)*cos(v*360°) Z(u,v)

50mm*sin(v*360°) u and v intervals u changes from 0 to 0.5, v from -0.1 to 0.1 50mm is the sphere radius

Eggs box: Formulas:

Result with intervals [-1 ; 1] :

X(u,v)

1mm*u Y(u,v)

1mm*v Z(u,v)

0,5mm*cos(u*360°)*sin(v*360°) u and v intervals u and v change from -1 to 1, then from -5 to 5.

Other surfaces: Formulas: X(u,v) 10mm*u Y(u,v) 10mm*sin(v*90°)* (1+cos(u*360°)/5) Z(u,v) 10mm*cos(v*90°)* (1+cos(u*360°)/5) u and v intervals v is periodic, u changes from -5 to 5 (the number of pitches is centered with the frame ), v changes from -2 to 2 (4 x 1/4 of turn).

Result:

Formulas with parameters: X(u,v) F*sin((P*u+v)*1°) Y(u,v) (GF*cos((P*u+v)*1°))*cos(u*1°) Z(u,v) (GF*cos((P*u+v)*1°))*sin(u*1°)

Result:

Re

Intervals u Minimum : -1620 Maximum : 1260 Intervals v Minimum : 0.6 Maximum : 6.6

Modifications: The surface can be modified with the Edit.. contextual command from the surface of from the operations tree.

Additional information: When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Extension Surface Links / Videos :

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This command allows to create a shape by extending a part area, while locally keeping the tangents to the base faces.

Creation stages / Use: Click the 1. 2. 3. 4.

icon or select the Surface > Extension Surface... command from the drop-down menu.

Select edges to define edges path. Select neighbouring face to define tangent and sections. Enter length extension. Select extension mode. Extruded: Edge extrusion according to given direction. Lofted: Creation of a lofted shape on edges path. Sections are created automatically from edges path and base face. Swept: Creation of a swept shape on edges path. Sections are created automatically from edges path and base face. Extension: Surface created by edge extension keeping face curvature.

5. Complete options.

This is particularly useful in sheet metal for manual unstamping.

Surface extension example with Lofted mode and lateral extension at the start

Available options: Boundary type (for Extension mode): Exact : Boundary extensions represent an exact measure of the distance from origin boundaries. Approximate : Boundary extensions represent an approximate measure of the distance from origin boundaries. Only the lateral boundaries length is exact.

Exact

Approximate

Side edges: Following adjacent edge: The extension side edge is created following the adjacent edge and/or its e Orthogonal to base edge: The side edge is created orthogonal to the base edge.

Following adjacent edge

Orthogonal to base edge

Lateral extensions: This option allows to extend surface boundaries at the start and/or end.

Create sections: This option allows to create different sections of the surface to create. A sketch solving operation is created.

Repair self-intersections: This option deletes auto-intersections between surfaces of the shape when this is the case.

Tangent surfaces

This command allows to create a batch of tangent surfaces along an edge path.

Creation stages / Use: Select the Surface > Tangent surfaces... command from the dropdown menu. 1. 2. 3. 4.

Select edges to define edges path. Select neighbouring face to define tangent side. Enter length of the surfaces. Validate with

A surface is created for each edge of the path. If the path is made of tangent edges, TopSolid will try to create a single surface for these edges. Individual operations are created for each surface in the operation tree.

Available options: Create folders: When this option is activated, all the surface operations are gathered into a sub-folder in the operation tree and a sub-folder is also created in the entities tree to gather all the surfaces.

Sewing: When this option is activated, a sawing operation is also created in order to sew all the surfaces together. You can specify the sewing tolerance.

Advanced options: Repair self-intersections: In some cases, it may be necessary to activate this option to help TopSolid to repair surfaces that are self-intersecting

Modifications / Additional information: Once the command has been validated, it is possible to edit each surface individually in order to modify its creation settings. It is also possible to delete them individually.

Imprint

This command allows you to print one or more profiles on one or more sides of a shape. New edges corresponding to the projection of the profiles are created on the faces.

Creation Stages / Use: Click on the icon

or choose the command Surface > Imprint... from the drop down menu.

1. Select the shape to modify 2. Select the imprint type Sections By two points By point and edge Isoclines

Sections

:

Select the different sections or sketches to imprint on the shape. Direction: This option allows you to choose the projection direction of the profiles: Orthogonal: The sketch is projected normal to each face. Specified: You are then prompted to provide a projection direction. Orthogonal

By two points

Following the sketch normal

:

Select the start and end points, a line passing by these 2 points will be imprinted of the face. It is unnecessary to create this line. Direction: This option allows you to choose the projection direction of the profiles: Orthogonal: The sketch is projected normal to each face. Specified: You are then prompted to provide a projection direction.

By point and edge

:

Select the start point and the end edge, a line passing by the point and normal to the edge will be imprinted on the face. It is unnecessary to create this line. Direction: This option allows you to choose the projection direction of the profiles: Orthogonal: The sketch is projected normal to each face. Specified: You are then prompted to provide a projection direction.

Isoclines

:

Direction: It is the reference direction for the measurement of the Isoclines angle. Angle: Enter the value of the angle.

3. Select the Sections, points and/or edges to imprint and the direction or the direction and the angle.

Available Options: Faces: Using this option you can specify the: Faces to consider: only the faces selected in this list will undergo imprinting of the sketches. Faces to ignore: the faces selected in this list will not undergo imprinting.

Advanced Options : Hidden faces : With this option, it's possible to not imprit profil hidden by a shape or a face. Faces Mode

Shape Mode

Hidden faces = No

Hidden

If the projection is on the faces, the projection is only made on the selected faces.

If the projection is on the shape, the projection is made on all the faces of the shape.

Faces Mode

Shape Mode

faces = Shape

If the projection is on the faces, the If the projection in on the shape, the projection is only made on the selected projection is made on all the faces not faces but not on the faces hidden by the hidden by the shape. shape. Shape Mode

Faces Mode

Hidden faces = Faces

If the projection is on the faces, the projection is only made on the faces selected by not hidden by the selected faces.

If the projection is on the shape, the projection is made on all the faces not hidden by the faces selected.

Connection of imprinted edges: None This option don't make connection between the disjoint edge. Side faces If possible, this option will connect all the disjoint edge with the imprint of other side edge. This option imprint side edge only if they connect disjoint edge. Side and hidden faces If possible, this option will connect all the disjoint edge by imprinting of side edge or hidden edge in the direction of the projection. All side faces This option allow to connect all the side edge whether they don't connect disjoint components of the imprint. All side and hidden face This option allow to connect all the disjoint edge by side edge or hidden edge in the direction of the projection.

Marking

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This command allows you to either affect a property or imprint a sketch on a part face. Marking if often used to display Manufacturing Index ant/or Mounting Index properties.

Creation stages / Use: Select Surface > Marking... command from the drop-down menu. With Automated mode: 1. 2. 3. 4. 5. 6. 7.

Select the property to mark. Enter the temporary text to display. Select the face to mark. Select the text origin. Select the text direction. Select the wire text family to use for marking. Enter the font size.

Without Automated mode: 1. Select the shape to modify. 2. Select the sketch to imprint.

Marking with Automated mode creates an auxiliary element named Sketches to Mark with all marking sketches inside. It is this auxiliary entity that will be displayed in upper assemblies (with possibility to show/hide it). In the part document, marking is represented by the temporary text until a marking operation is done in the assembly containing the part. The auxiliary element Sketches to Mark is then automatically hidded and the imprint is done on the face of the part.

Marking for mounting index with $ symbol as temporary text

After marking operation in the assembly containing the part, the temporary text is replaced by the value of the property and the imprint is done on the face of the part

Marking operation created from the assembly in which the part has been included will modify it according to settings of parts operation options.

Available Options:

Lightweight (available when Automated mode is off) : This option will not imprint the sketch on the part but will store all marking attributes to display sketch on upper documents. This allows to not reduce performances since no edges are adding to the shape. In the operation tree, Ø symbol is added in front of the lightweight marking.

Machining process (available when Automated mode is off) : This option allows to assign a machining process to the operation. This machining process is recognized by TopSolid'Cam. It can also assign a color to the operation.. 1. Select a machining process document in the drop-down list. 2. Select a process in the drop-down list.

Modifications / Additional information: With Automated mode, user can enter a part of the property to use. TopSolid will filter the properties drop-down list to display properties containing entered text. It is possible to use several properties in the same marking operation. Use & symbol to seperate them. To add text between properties you must add ". 'Mounting Index'&'Manufacturing Index' 'Mounting Index'&" - "&'Manufacturing Index'

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This command removes faces on a shape with the possibility to automatically refill the hole resulting from the removal of these faces.

Creation Stages / Use: Click on the icon drop down menu.

or choose the command Surface > Removing... from the

1. Select element type to remove: faces, edges loop, restrictions, bodies, edges. 2. Select entities to remove.

When selecting the faces to remove, in order to select all of the faces tangent to the one clicked, you simply need to perform a rotative picking. If this command was used to create several bodies, it is then possible to automatically generate an assembly made of these bodies (1 part file by body will be created) thanks to the partial parts command.

Available Options: Type You can choose different types of elements to delete: Face: Deletes faces from a shape. This mode has several options to heal a hole obtained by deleting surfaces (see "Heal type" option). The keep faces option allows to unsew selected faces. Edges loop: Deletes an edge loop from within a surface. It is easy then to delete a hole in a surface using this mode.

Restrictions: Deletes restrictions from a surface. We then get a surface without a hole and with extended trims.

Bodies: Allows to remove or separate a body of a shape multi bodies. To separate bodies, you have to check the Keep bodies option. Edges: Allows to remove an edge which separates 2 faces like it is the case with an imprint..

Keep faces: Deleted parts are hidden. By checking this option, they stay visible and can be used. For example, the removing of a face without healing, unsews this face if this option is checked.

Heal type: Here you can choose the type of heal made on the hole resulting from removing faces. None: leave the hole (no heal). Cap: Attempt to create a surface to cap the hole. Stretch: Attempt to stretch the neighboring faces until there is no more hole. Blend: same principle as "Stretch" but is adapted to the deletion of the fillets.

Before

Faces selection

Heal = Blend

Heal = None

The Blend heal mode is not provided for deleting chamfers and only functions for fillet type surfaces.

Additional Information: When you remove a face from a volume element without healing, it becomes surfacic. If a face is missing (for example the bottom face of a pocket), the operation becomes invalid.

Fill hole

This command fills holes in any position (included in the surface or beyond a border).

Creation Stages / Use: Click on the icon menu. 1. 2. 3. 4.

or choose the command Surface > Fill Hole... from the drop down

Select the hole's border edges. Choose the method to use to build the surface. Fill in the additional information, depending on the chosen method Validate with .

The result is an operation on the shape, which returns the border edges. No new shape is created in the shape folder in the entity tree.

Available Options: Hole edges: This option lets you define edges that define the limits of the hole. By default, the entire detected edge loop is automatically selected. If the hole to fill is on the border of the surface, there are other possible ways to make a selection. Selecting one edge and a profile: Use rotative selection to select a single edge rather than the entire loop. The profile option is then available. In addition to the edge, select a profile to define the closed trimmings. Example: In this example, the edge that is selected by rotative selection is the additional profile that determines the trim of the hole to be filled.

Select an edge path and a profile: Click the button, and select the "Border edges between vertices..." command. You must then select one of the path's edges and the two end points for the path. Confirm your selection. Next, select the profile and the edge path to define the closed trims. Example: In this example, we see the selected edge marked by a dotted line, along with the two end points. Automatically selected edges are displayed in orange.

Method: This option allows you to choose the method used for creating the surface. There are several available methods: Fill: This method allows to fill the hole thanks to one or several surfaces created automatically. The filling ends at the limits defined by the selection of the hole edges. Extend: This method does not work for surface border holes. Only the hole's edges must define a closed contour. With this method, instead of getting a filling inside the limits, you get an extended surface up to the limits of the neighboring faces. Example: Fill

Extend

Trim the hole: With this method, the hole is plugged using an initial surface, which the user selects using the "Shape Filling" option. The surface is trimmed at the edges of the hold and then sewn to the main shape. Trim the surface: With this method, the hole is plugged using an initial surface, which the user selects using the "Shape Filling" option. The main shape is trimmed by the surface edges that were then sewn. Example: In blue, the surface to fill In yellow, the filled surface

Trim at the hole

Trim at the surface

Continuity: This option is only available with the "Fill" method None: no tangency or curvature constraint is used on this edge. Tangency: the surface will be tangent with the neighboring face along this edge. Curvature: the curvature radius of the neighboring face is used to define the curvature of

surface.

Special edges: This option is only available with the Fill method. it allows to define specific continuity on some edges of the hole: Either by using the contextual menu on the edge, and selecting the required continuity in the "Selection" section of the menu. Or by selecting the edge as special edges in the dialog and editing the label to choose the required continuity.

Minimal division: This option is only available with the Fill method. It allows to minimize as far as possible the number of faces generated by the filling.

Extension

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This command allows you to extend the borders of a surface.

Creation Stages / Use: Click on the icon

or choose the command Surface> Extension... from the drop down menu.

1. Select a face's border edges or select a face if you want to extend all of the faces dimensions. 2. Choose the calculation mode for the length of the extension: Length mode: The value of the extension is entered manually. Shape Mode: The surface is extended to the first intersection between the faces and a shape. In this mode, the selected shape must absolutely exceed the face to extend. Face mode: The surface is extended to the intersection with a face.

3. Validate with the

button.

It is not possible to select border edges that belong to different shapes.

Available Options: Linear mode allows for a tangent extension, while Curvature mode also respects the curvature of the face. Modify faces: This command can either create new faces (option activated) or modify the reference faces (option deactivated).For example, if the face is extended by 5mm and the option is activated, the initial face will not change but a second face will be created with a 5 mm length. If the option is activated the face is extended by 5 mm.

Boundary type: Exact : Boundary extensions represent an exact measure of the distance from origin boundaries. Approximate : Boundary extensions represent an approximate measure of the distance from origin boundaries. Only the lateral boundaries length is exact.

Exact

Approximate

Side edge: Automatic: TopSolid selects for each edge the best method. Following adjacent edge: The extension side edge is created following the adjacent edge and/or its extens Orthogonal to base edge: The side edge is created orthogonal to the base edge.

Following adjacent edge

Orthog

This option is only applied on the extremities of an edge path. In the upper examples, if the faces are are impacted.

Smoothing Links / Videos:

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This command can produce a single-face surface from a multi-face surface.

Creation Stages / Use: Click on the icon drop down menu.

or choose the command Surface > Smoothing... from the

1. Select the face smoothing mode: By Points: The smoothing is done by distributing points on U and V isoparametric curves on the faces. By Plane: The points on the reference plane are projected on the faces to smooth. These points are then used to calculate a surface by limited interpolation by the outer borders of the faces to be smoothed. By Tolerance: The smoothing is done with a given tolerance.

2. According to the smoothing mode chosen: Select the reference plane for the smoothing or check Automatic plane. Enter the number of isoparametric curves following U and V directions Enter the tolerance value. 3. Validate with the button.

The reference plane's normal should not intersect the faces to smooth multiple times. It is not possible to select faces that belong to different shapes.

Available Options: Sewing tolerance:

When the smoothing is done on a part of the shape, the smoothed face is then reconnected to the shape. The sewing tolerance reconnects the faces whose border edges were deformed.

Example:

Surface before smoothing

Surface after smoothing

Replacing Links / Videos:

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This command can replace several faces of a shape by a surface.

Creation Stages / Use: Click on the icon or choose the command Surface > Replacing... from the drop down menu. 1. Select the faces to replace. 2. Select the type of replacement surface. Mono-face: A surface with one face is replaced by another mono-face surface. This mode allows to activate the Edges options explained below. Multi-faces: Allows to replace a batch of faces by a multi-faces surface. This mode can't work if the faces to replace have boundary edges while it is not possible to find the edge matchings.

3. Select the replacement surface. 4. Check the Hide surfaces option to hide replacing surfaces. 5. Validate with the button.

Example:

In red: The faces to replace In yellow: The replacement surface

Result

with mono-face mode, the replacing surface must also be a monoface surface.

Available Options for the mono-face mode: Edges: In some cases, the replacement can fail. It is possible to help TopSolid by selecting face edges to replace. Edge to replace: Select an edge to replace. Replacement curve: When an edge to replace is selected, you also have to select the replacement curve.

Sew

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This command sews together a set of surfaces.

Creation Stages / Use: Click on the icon

or choose the command Surface > Sew... from the drop down menu.

1. Select the surface shape or the main surface on which to sew the other surfaces. 2. Select other surface shapes or surfaces to sew.

The sewing combines 2 separated faces by merging their common edges of these 2 faces.

Available Options: Hide: The box allows to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Tolerance: This option defines the sewing tolerance between the faces. For two surfaces to be able to be sewed together, the edges common to these two surfaces must not be farther apart than the sewing tolerance.

Number of iterations: Using this option, you can optimize the sewing of a set of faces. This is how this option functions: If you validate the function, a first sewing is made as per the tolerance given. However, surfaces that are too far from each other will not be sewn. The value of the tolerance is thus multiplied by 2 and new sewing of the remaining surfaces occurs with this new tolerance. The value of the tolerance is then multiplied by 2 again and so on; as many times as the number of iterations. For example, for a initial tolerance of 0.01mm and a number of iterations of 3, here is what will happen: first sewing at the 0.01mm tolerance second sewing has a tolerance of 0.02mm (0.01mm x 2) third sewing at a tolerance of 0.04mm (0.02mm x 2)

The maximum number of iterations is 10. And the minimum number is 1 (the first sewing).

Separate: Without this option, when sewing separated batches of surfaces in a single sewing operation, TopSolid generates a single shape made of several bodies. When using this options, the separated batches of surfaces are sewed as independent shapes. In the example bellow, we can get a single shape with four surfaces into two bodies (without "separate" option) or two shapes made of 2 faces each (with the "separate" option)

Sewing of separated surfaces

Sewing result with 2 shapes made of 2 faces

Associative: This option allows to keep the sewing information as an operation that can be edited from the operation tree. When this option is not activated, the result of the sewing is a non associative part. it is to say that the shape does not have historic of the operations made previously on it and it will not be possible to edit them anymore. The result is the equivalent of an imported shape.

It is not possible to modify the associativity type afterward. If it has been made in non associative mode, it will not be possible to modify the operation made previously on the part. The shape has become a non associative body.

Preserve colors: This option allows to keep the entity color on tool faces and this, after sewing.

If some faces have been colored with the Coloring command, the color will be kept on these faces during the sew, even if the option is not checked. The Preserve colors option only takes in account the color attribute of shapes.

Advanced options: Merge: This option allows to merge the imprinted surfaces with the sewing.

Sewing with an imprinted surface (the rectangular surface in the middle)

Sewing result

Create boundary edges: This option allows to create boundary edges. Only surfaces have boundary edges. A solid has not.

Modifications / Additional information: If the sewing has been made in associative mode, it is possible to edit the operation and add or extract surfaces from the list of surfaces to sew.

At the end of the sewing operation, a message indicates the number of solid, surfaces and holes. If the message displays "solid=1", the part is a solid shape. If the message displays a number of surfaces and holes, the sew is not complete. Some missing surfaces have to be created before trying to sew again.

Unsew Links / Videos:

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This command separates all of a shape's faces.

Creation Stages / Use: Click on the icon or choose the command Surface > Unsew... from the drop down menu. 1. There are two ways to choose the faces to remove: Faces: faces to unsewed are manually selected. Shape: All of the selected shape's faces are removed. 2. Validate with the button.

It is not possible to remove faces that belong to multiple shapes.

Available Options: Associative : This option preserves a link between reference faces and removed faces When this mode and Shape mode are checked, the shapes corresponding to the faces of the reference shape are created and are no longer available. They are grayed in the entity tree..

Preserve color : This option allows to preserve the colors of coloring faces.

Advanced Options: This option allows to define a layer for new created faces.

Modifications / Additional information: This command generates as many new shapes as there are selected faces or faces that make up the selected shape.

Convert into Solid Links / Videos :

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This command allows to convert a surfacic shape into a solid shape.

Creation stages / Use: Select the Surface > Other > Conversion into Solid... command from the drop-down menu. 1. Select the shape to convert. 2. Valid with the button.

When the surfacic shape is opened, the hole are automatically filled using the Fill option of the Fill Hole... command.

Modifications / Additional information: This command generate an operation which can be deleted from the operation tree.

Conersion into Sheet Links / Videos :

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This command allows to

Creation stages / Use: Select the Surface > Other > Conversion into Sheet... command from the drop-down menu. 1. Select the shape to convert. 2. Valid with the button.

Modifications / Additional information: This command generate an operation which can be deleted from the operation tree.

Conversion into Faceted Shape

This command allows to convert an exact shape or a polyhedron into a faceted shape.

Creation stages / Use: Select the Surfaces > Other > Conversion into Faceted Shape... command from the drop-down menu. 1. Choose the shape type to convert (Exact shape or Polyhedron) 2. Select the shape to convert. 3. Confirm with the button.

Available options: Convert: When this option is checked, the selected shape is converted into a faceted shape and its history is definitely lost. When this option is unchecked, a new shape containing the faceted shape is created.

Advanced options: The linear and angular tolerance options allows to get a faceted shape more or less close to the exact shape.

Exact shape

Faceted shape with a Faceted shape with a linear tolerance of linear tolerance of 0.2mm and an 1mm and an angular angular tolerance of tolerance of 15° 15°

In Polyhedron mode, 2 additional options are available: Clean: this option allows to clean the invalidity of the polyhedrical mesh. The main cause of invalid mesh are: the height of a triangle is lower than the tolerance value, a selfintersecting face or the distance between 2 vertex of a triangular face is lower than the tolerance value. Find faces : when this option is checked, it allows to rebuild the faces, otherwise the faceted shape will be made of one face only.

Modifications / Additional information: Faceted shapes are made of triangular faces. Generally, they are coming from STL or IFC import.

Normal Reversal

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This command allows you to reverse the direction of surface faces. This command can be useful to correct import errors due to bad file quality or for surface machining with TopSolid'Cam.

Creation stages / Use: Click on the icon or choose the command Surface > Normal reversal... from the drop down menu. 1. Select the faces to invert. 2. Click the arrow to reverse. 3. Validate by clicking .

Available Options: Hide: The box allows to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Modifications / Additional information: You can modify or delete using the operations tree.

Heal Links / Videos:

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This command allows you to heal a geometry by verifying it, making cuts if necessary, simplifying it and verifying it again. This command is very useful after a file import.

Creation Stages / Use: Click the icon or select the Surface > Healing > Heal... command from the drop-down menu. 1. Select shapes to check or All shapes by clicking on the icon. This order and its result are explained in the online help for the Check command. 2. Click to the next step: Sewing. This command and its result are explained in the online help for the sewing command. 3. Click to the next step: Result of the sewing. If the number of solid is 1 and the number of holes is 0, the shape is a solid. If some surfaces are listed, it is possible to sew again by clicking the New sewing button. 4. Click to the next step: Simplification. This command and its result are explained in the online help for the simplify command. 5. Click to the next step: Result of the simplification. This dialog indicates the number of simplified faces and shows them. 6. Click to the next step: Result of the verification. This step indicates the number of invalid faces that must be removed.

7. Validate by clicking

.

For each detected invalidity, a graphic entity is created for viewing and locating the invalidity in the document. The list of invalid entities is found in the "Warning" section of the entity tree.

The healing can only be apply on imported surfaces. You have to move down the insertion cursor on the import operation (via the operations tree). To heal after sewing, you need to clean the shape. But it is strongly discouraged to sew invalid surfaces. If the All shapes option is used, all the visible shapes will be selected.

Available Options: Hide: The box allows to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Modifications / Additional information: When the cleaning is finished, and if some invalidities have been detected, a Defaults folder is created in the entities tree which lists all invalidities. It contains: an invalidities sub-folder with Check command results. a Gaps sub-folder with Detect gaps command results. A popup menu allows you to interact with each of them to hide/show or zoom.

Check

This command performs a verification on the geometry of shapes and surfaces in order to highlight what is invalid.

Creation Stages / Use: Click the icon or select the Surface > Healing > Check... command from the drop-down menu. 1. Select shapes to verify or All shapes by clicking the icon. 2. Move to the next stage with the button. 3. The number of invalid shapes and the list of detected invalid items than appears. You can place these invalid shapes on a particular layer or simply validate the command with

For each detected invalidity, a graphic entity is created for viewing and locating the invalidity in the document. The list of invalid entities is found in the "Warning" section of the entity tree.

If the All shapes option is used, all the visible shapes will be selected.

Available Options: Advanced Options: Layer:

This option allows you to place invalid shapes on a specific layer.

Modifications / Additional information: Once the verification is finished and invalid items have been detected, a "Warning" section is created in the entity tree, listing the invalid items. A popup menu allows you to interact with each of them to hide/show or zoom.

Clean

This command lets you quickly repair some invalid items in an invalid shape (generally following an import).

Creation Stages / Use: Click on the icon or choose the command Surface > Healing > Clean... from the drop down menu. 1. Choose the shape type that you want to clean: Shapes: Allows you to select the exact shapes. This mode allows you to select several shapes and the icon allows you to select all the exact shapes of the document. Faceted shapes: Allows you to select faceted shapes (triangular faces meshing) that comes from from an STL or IFC import or converted with the Surface > Other > Conversion into Faceted Shape... command. This mode allows you to select one shape only. 2. Indicate the linear and angular tolerance value to comply with when cleaning up the geometry. 3. Move to the next stage with the button. 4. The number of cleaned shapes is shown, and there is a list to identify them. You can place the cleaned shapes on a particular layer or validate the command with .

If the All shapes option is used, all the visible shapes will be selected. The cleaning of faceted shapes consist in cleaning the mesh invalidities which size is lower than the given tolerance. The main causes of an invalid meshing are: the triangle height is

lower than the tolerance value, a self-intersecting shape or the distance between two vertices is lower than the tolerance value.

Available Options: Hide: The box allows to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Optimize: Simplify faces: This option allows to increase the level of simplification of the shapes, it allows to reduce the model size, increase preformances and get a better reliability for the coming operations. In return, it may change the topology so you will have to deactivate it if the part becomes invalid. It is recommend to use the same tolerance than for the cleaning (see 2. upper). If the user changes the cleaning tolerance, the simplification tolerance is updated. Optimize blend faces: This option allows to recognize fillet faces and convert them.

Advanced options: Repair edges: Check this option if you also want to repair the edges of the faces. You then have the ability to specify the tolerance for the edges to comply with. It is recommended to enter a tolerance for edges healing greater or equal to the global cleaning tolerance. Delete small edges: By checking this option, edges whose length is less than the specified value are deleted. The surface is then rebuilt on the remaining edges.

Delete small topologies: This option is for deleting "micro-surfaces" that could be ignored, considering only the neighboring surfaces to model the shape. Different deleted topologies are: small edges and faces tips fines faces nicks

Simplify

This command simplifies the topology of a shape by converting surfaces that can be it and the edges of online faces into a planar, cylindrical, or conical surface, or into arcs for edges that can be it, while complying with the given tolerance.

Creation Stages / Use: Choose the command Surface > Healing > Simplify... from the drop down menu. 1. 2. 3. 4.

Select shapes to simplify or All shapes by clicking on . Enter the tolerance to respect during the simplification. Move to the next stage with the button. The number of simplified edges and faces is indicated, and there is a list to identify them.

This command is useful for files that come from an IGES import, for example. In fact, surfaces from an IGES are b-spline surfaces (not true planar or cylindrical faces in the mathematical sense of the term). Simplification will therefore result in a lighter value, authorizing the use of command that require planar or cylindrical faces as reference.

If the All shapes option is used, all the visible shapes will be selected.

Available Options: Hide: The box allows to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Tolerance: By checking this option, all of the shapes contained in the document are selected and added to the list of shapes to be simplified.

Preserve tangencies: This option allows to preserve tangencies between faces in some cases. It is not compatible with the optimization below. It is recommended to use the optimize option. If the result is not satisfying, check this option.

Optimize: Repair edges: Check this option if you also want to repair the edges of the faces. You are able to enter a tolerance to respect. It is recommended to enter a tolerance for edges healing greater or equal to the global cleaning tolerance. Optimize blend faces: This option allows to recognize fillet faces and convert them.

It is recommended to always optimize the shape after cleaning to reduce the model size. The fillet's faces are always considered as simplified faces. So, they are always displayed in the dialog which

displays the simplification results (even when the operation is run several times).

Advanced options: Merge: This option allows to activate or deactivate the merge of faces with the same support. If it is unchecked, the option below is grayed. Merge tolerant planar faces: By activating this option, all the planar faces with a common edge and with the angle between their normals is smaller than the given tolerance will be merged into a single face. Angular tolerance: This option allows you to specify the tolerance to complied with during the simplification of surfaces. Therefore, a face will be simplified only if the new surface remains within the tolerance limits of the initial surface.

Modifications / Additional information: Given that this order rebuilds surfaces, it can also be used to repair some invalid items through rebuilding the face. The opposite is also true; an invalid item may occasionally appear after a geometry simplification. It is therefore recommended to always verify shapes after simplification is complete.

Detect gaps Links/Videos:

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This command allows to detect and localize small gaps between faces. This is useful when working on surface sewing on an imported shape.

Creation stages / Use: Click on the icon or choose the command Surface > Healing > Detect gaps... from the drop down menu. 1. Select shapes to analyze or All shapes by clicking the icon. 2. Enter the tolerance gap (minimum and maximum tolerance). 3. Click on the next step arrow. A list displays the gaps detected between faces. Once the command has been validated, this list can be consulted into the entities tree, into the folder Warning > Gaps.

Once the gaps between faces are known, it is possible to adjust them each other through the command Adjust continuity available into the contextual menu on one of the gaps from the list into the entities tree.

If the All shapes option is used, all the visible shapes will be selected.

Available Options: Hide: The box allows to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Adjust continuity Links/Videos:

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This command allows to adjust the continuity between faces by applying a deformation on the edges.

Creation stages / Use: Choose the command Surfaces > Healing > Adjust continuity... from the drop down menu. Two modes are available. Adjust continuity of source edges on destination edges: allows to adjust the continuity between independent faces (not sewed surfaces) 1. Select the source edge of the face to modify. 2. Select the destination edge on the face that will be used as reference for the continuity. Adjust continuity of tolerant edges: allows to adjust the continuity of internal edges of a shape in the case of tolerant edges. In this case, the modified support surface has a reduced accuracy. 1. Select a source edge. 2. Select the face to modify on one side or the other of this edge.

Before using this command it is recommended to clean the geometry of the surfaces in order to make the calculation of the

adjustment more consistent.

Available Options: Swap Edges: This button allows to reverse the "source" and the "destination".

Continuity: Adjust position: simply move the edge onto the reference edge. Adjust tangency: move the edge onto the reference edge and also adjust the tangency between the faces.

Influence Distance: This option allows to set the distance along which the surface to modify can be deformed to get the continuity.

Source Extremities: This option allows to define the way the command will make the source geometry fits with the extremities of the edges. The start or the end of the source edge corresponds to the extremity of the destination edge. The start and the end source edge are projected on the destination edge.

Linear Tolerance: This value represent the modeling accuracy of the adjusted surfaces.

Additional information:

When this icon is displayed, the preview is deactivated. If the mode is deactivated (no preview), it will not be possible to temporary activate it in the command. You must first activated the preview mode, to be able to temporary deactivate it in a command by clicking on .

Edit trimming curves Links / Videos :

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This command allows to redefine the trimming curves of a surface. The goal is to "repair" an invalid surface by redefining its trimming curves then recreate the surface using the new curves.

Creation stages / Use: Click the icon or select the Surface > Healing > Edit trimming curves... command from the drop-down menu. 1. Select the face to treat. 2. Click the Edit button. A new Model 2D document is created with the trimming curves U and V of the selected face in it. Rebuild the curves using the 2D sketch commands. You can just passing existing restrictions with the contour command or modify them which will have an impact on the surface geometry. 3. Validate the sketch. 4. Validate the restrictions edition. 5. Validate the command with the button .

If one of the selected shape is not basic (without associativity), TopSolid will ask you to basify them. If you answer "No", the command is stopped. The document in which you create the new curves is just temporary and is not saved; no links are created between this

two files.

Available options: Adjust curves: When a face is invalid, its profiles can be unjoined. This option allows to adjust them together.

Modifications / Additional information: The shape has been basified, there is no more history in the operations tree.

Detect Superpositions

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This command allows to detect superposed shapes from an imported document.

Creation stages / Use: Click the icon or select the Surface > Healing > Detect Superpositions... command from the drop-down menu. 1. Select shapes to verify or All shapes by clicking the icon. 2. Move to the next stage with the button. 3. Superposed shapes are listed into a new dialog Superposition result. Les faces superposées sont regroupées par lots.

If superpositions are found a Defects folder will be created in the entities tree containing these superposed shapes. A right click on a Superposition node allows to: Zoom on this et of faces. Run the Superposed Shapes layer.

Available options:

Hide: The box allows to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Linear and angular tolerances: These values are used to refine the detection of superposed shapes.

Fast Bspline comparison: Option checked by default for faster processing of B-splines faces. By disabling this option, additional nodes will be included in the processing, which will take longer to obtain a result.

Similar faces: Allows similar faces to be considered. Search faces with: More active loops: While the analysis of two faces, if one of them has more loops, these faces will be considered to be similar. Less loops: While the analysis of two faces, if one of them has less loops, these faces will be considered to be similar. Different loops: If the faces to analyze have loops with a different geometry or position, these faces will be considered to be similar. No active option: This looks only for faces that are completely identical. No concept of similar faces.

Introduction to FreeShape Functions

Introduction On an imported part, it is now possible to modify operation because there are none. (However, it is possible to create new operations to modify the shape's geometry.) This is why, when working with a rather simple imported shape, we can imagine wanting to manipulate it as with sketches, moving the faces (instead of sketch segments) with the mouse, or having dimensions or relationships that would impose constraints on the imported geometry. This is possible with FreeShape.

Creating a FreeShape When a file is imported that contains geometric solids with conversion, the shapes of the produced parts are FreeShape by default. It is also possible to create a FreeShape by converting a shape produced using operations in TopSolid, using the FreeShapes > FreeShape... command. . This command removes all operations from the existing shape and creates a new Resolution operation that handles the form as FreeShape (like for sketches whose constraints are resolved by such an operation).

Using commands to work on the FreeShape is done in edit mode. Commands in the FreeShape menu are therefore accessible only if the user is currently editing the FreeShape.

Editing a FreeShape A FreeShape is modified just like a sketch. You must first edit it, then you can add dimensional or relationship constraints or any other modification using functions in the Shape > FreeShape menu. It is also possible to make some modifications directly with the mouse by selecting a face and moving the mouse without releasing the button. To edit a FreeShape, use the Edit command in the shape's popup menu to move to edit mode for the resolution. To finish the FreeShape edition, click the button upper the graphic area..

Automated dimensioning To avoid having too many degrees of freedom, which would lead to uncontrollable behavior, it is useful to impose some natural constraints, such as the fact that a planer face retains its orientation. Other common constraints include maintaining the coaxiality of two aligned holes or even multiple faces making up the same hole (smooth hole with spot facing). These constraints can be created at the time of conversion by using the command in TopSolid or by using the FreeShape > Automatically Constrain... command later. (This command must be used for imported FreeShapes, which are not constrained.) As fro a sketch, it exists a color code to indicate the level of constraint of an element. Under-constrained is magenta, totally constrained is blue, fixed is gray.

This color code can be modified in the Tool > Options > Design Colors command.

Operation Extraction The main interest of FreeShape is being able to easily and quickly work with a shape that is essentially made up of faces with a simple geometry: plane, cylinder, sphere, etc. It is therefore often useful to get rid of all the small complex faces that can cause problems during resolution. In particular, if the shape has fillets or chamfers, they should be extracted, or removed from the "resolution" portion, to make traditional operations from them, to recreate the resolved shape, with the resulting shape being the same. To do this, edit the FreeShape and use the FreeShape > Extract Operation... command. .

Operation Deletion On the same principle, it is possible to simply delete an operation/geometry. Unlike extract, deletion does not recreate an equivalent operation outside of FreeShape. The operation must therefore be manually created once the valid FreeShape is edited. To delete a face, use the FreeShape > Delete Faces... command.

Insertion Conversely, we may want to add faces to a FreeShape to be managed with constraints. The shape should then be modified using traditional operations (pocket, boss, etc.), and the result should be converted into a FreeShape with the FreeShapes > FreeShape... command.

Dimensions Once the FreeShape geometry is finalized, it will be possible to constrain it by adding dimensions with the FreeShape > Dimension... command, in the same way as for a sketch.

Relations Similarly to dimensions, it will also be possible to impose relationships between faces through the FreeShape > Relations menu commands.

Geometry: Associated geometries (points, axes, planes, etc.) can be created on the shape's entities using commands in the FreeShape menu.

FreeShape Links / Videos:

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This command generates a FreeShape shape. This command deletes all existing operations for the shape and creates a new Resolution operation that handles the shape like FreeShape.

Creation Stages / Use: Click the icon or select FreeShape > FreeShape... from the dropdown menu. 1. Select the shape to convert in FreeShape. 2. Validate

Available Options: Conversion mode: A part in FreeShape can be converted in two ways: Convert This mode completely deletes the existing operations history before the conversion. Modify This mode saves the history of operations performed on the part before conversion. You can therefore work in FreeShape mode and modify operations outside of FreeShape.

Operations tree before conversion

Conversion in Convert mode

Conversion Modify mode

It is not possible to drag an entity (like a point) when using the Modify mode. It can be dragged if using the Convert mode.

Modifications / Additional information: Using commands to work on FreeShape is done in its edit mode Commands in the FreeShape menu are accessible only if the user is currently editing in FreeShape. To do this, use the "Edit" command in the shape's popup menu to switch to resolution edit mode.

During conversion in FreeShape, fixity constraints are automatically created on all of the faces of the shape receiving the constraint. Therefore, to be able to make geometric or dimensional modifications, you must remove the fixity using the Unfix command in the contextual menu for the selected face.

Extract fillet or chamfer Links / Videos:

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This command extract a fillet or chamfer operation from the FreeShape resolution. This operation is automatically recreated in the operation history for the part outside of the FreeShape resolution. This command is only available in FreeShape edit mode. To do this, use the "Edit" command in the shape's popup menu to switch to resolution edit mode. To finish editing in FreeShape, click the button at the top of the graphic area.

Creation Stages / Use: Click the icon or select the FreeShape > Extract fillet or chamfer... from the drop-down menu. 1. Choose the type of operation to extract (fillet or chamfer). 2. Select the faces that correspond to the operation. 3. Validate.

Modifications / Additional information: After validating the command, the operation visually disappears from the part in the graphic zone. A new operation appears in the operation tree. When a FreeShape edit is validated, the operation (now outside of the FreeShape resolution) visually appears on the

part. This new operation is handled like any other operation that you perform on the part with the usual functions.

Extract drillings Links/Videos:

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This command allows to extract drilling from an imported shape (FreeShape), in order to transform them into an operation and be able to modify (change the diameter) or delete it.

Creation stages / Use: Click on the icon or choose the command FreeShape >Extract Drillings... from the drop down menu. 1. Select the cylindrical faces of the drilling to extract. 2. Validate by clicking .

This command generate an operation into the operations tree. If it is deleted the associated drillings on the shape are also deleted.

Available Options: Mode: Unit: This mode allows to select drillings one by one.. Group:

This mode allows to group same type drillings (spot facing for example) ,with same characteristics and with a common flat face. This command creates one or several operations (Drilling or Drillings group).

Check: If the operation can't be validated a Check button appears. It allows to filter drillings to remove those with a problem. It is possible that removed drillings from the list, can then be extracted by a second operation.

Modifications / Additional information: The drilling extraction can be edited, modified or deleted.

Delete faces Links / Videos:

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This command removes a set of faces from FreeShape with the possibility of automatically filling the hole resulting from the removal of the faces. This command is only available in FreeShape edit mode. To do this, use the "Edit" command in the shape's popup menu to switch to resolution edit mode. To finish editing in FreeShape, click the button at the top of the graphic area.

Creation Stages / Use: Click the icon or select FreeShape > Delete Faces... from the drop-down menu. 1. Select the faces to remove. 2. Validate.

Available Options: Heal type: Here you can choose the type of heal made on the hole resulting from removing faces. None: leave the hole (no heal).

Cap: Attempt to create a surface to cap the hole. Stretch: Attempt to stretch the neighboring faces until there is no more hole. Blend: same principle as "Stretch" but is adapted to the deletion of the fillets. Before

Faces selection

Heal = Blend

Heal = None

The Blend heal mode is not provided for deleting chamfers and only functions for fillet type surfaces.

Modifications / Additional information: When you remove a face from a volume element without healing, it becomes surfacic.

Grab operation Links/Videos:

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This command allows to absorb a operation created after the Freeshape converted.

Creation stages / Use: Click on the icon or choose the command FreeShape > Grab operation... from the drop down menu. 1. Validate your converted FreeShape by cliking on . 2. Create the new operation with the usual commands (pocket, drilling,...) 3. Edit the FreeShape entity from the operation tree or graphic area. 4. Start the command Grab Operation. 5. Select the operation to grab in the drop down list. 6. Validate by clicking .

This command can only be used for converted FreeShapes.In the case of a modified FreeShape, you just need to drag the operation bellow the FreeShape operation in the operation tree. Only some type of operation can be grabbed. It is the operation such as fillet, chamfer, boss, pocket, slot, groove, draft, drilling, faces modification, offset, ... In other terms, all the shape modification operations that work only the shape of the

FreeShape et are not linked to other elements created by operation that are not absorbed The shape is modified and the new faces are set as fix into the FreeShape definition.

Before the grabbing, the operation is above the FreeShape into the construction tree. After the grabbing, it is integrated into the FreeShape and does not appear anymore as an operation into the operation tree. It could only be modified by editing the FreeShape.

Offset point

This command allows a point to be created offset by a value in a given direction.

Creation Stages / Use: Click the icon or select FreeShape > Offset Point... from the drop-down menu. 1. Select the point of origin. If no point is selected, the absolute point is used automatically (coordinates 0,0,0). 2. Choose the direction of the offset. 3. Enter the offset value in the given direction or use the label.

The point can be seen and edited only in FreeShape mode. By using this command, the point is created inside the resolution of the FreeShape and therefore can only be modified or updated in FreeShape edit.

Midpoint

This command allows you to create a midpoint by selecting the 2 end points in a FreeShape item.

Creation Stages / Use: Click the icon or select FreeShape > Midpoint... from the dropdown menu. 1. Select an end point. 2. Select the second end point.

The point can be seen and edited only in FreeShape mode. By using this command, the point is created inside the resolution of the FreeShape and therefore can only be modified or updated in FreeShape edit.

Axis by 2 points

This command allows to create a axis passing by two points in a FreeShape element.

Creation Stages / Use: Click the icon or select FreeShape > Axis by 2 points... from the drop-down menu. 1. Select the first passing point. 2. Select the second passing point.

The axis can be seen and viewed only in FreeShape mode. By using this command, the axis is created inside the resolution of the FreeShape and therefore can only be modified or updated in FreeShape edit.

Offset axis

This command allows you to create an offset axis in a direction in relation to the reference axis in a FreeShape item.

Creation Stages / Use: Click the icon or select FreeShape > Offset Axis... from the drop-down menu. 1. Select reference axis. 2. Select offset direction. 3. Enter the offset value.

The axis can be seen and viewed only in FreeShape mode. By using this command, the axis is created inside the resolution of the FreeShape and therefore can only be modified or updated in FreeShape edit.

Midaxis

This command allows you to create a middle axis with two axes in a FreeShape element.

Creation Stages / Use: Click the icon or select FreeShape > Midaxis... from the dropdown menu. 1. Select the direction of the first axis. 2. Select the direction of the second axis.

The axis can be seen and viewed only in FreeShape mode. By using this command, the axis is created inside the resolution of the FreeShape and therefore can only be modified or updated in FreeShape edit.

Pivoted axis

This command allows you to create a pivoted axis around another axis in a FreeShape element.

Creation Stages / Use: Click the icon or select FreeShape > Pivoted Axis... from the drop-down menu. 1. 2. 3. 4.

Select reference axis. Select the rotation axis. Enter the rotation angle. Check Reverse to reverse the angle.

The axis can be seen and viewed only in FreeShape mode. By using this command, the axis is created inside the resolution of the FreeShape and therefore can only be modified or updated in FreeShape edit.

Offset plane Links / Videos:

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This command allows you to create an offset plane in a FreeShape element.

Creation Stages / Use: Click the icon or select FreeShape > Offset Plane... from the drop-down menu. 1. 2. 3. 4.

Select the reference plane. Enter the plane's offset distance. Reverse the offset direction, if necessary. Validate with the button.

The plane can be seen and edited only in FreeShape mode. By using this command, the plane is created inside the resolution of the FreeShape and therefore can only be modified or updated in FreeShape edit.

Midplane Links / Videos:

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This command allows you to create a midplane in a FreeShape element.

Creation Stages / Use: Click the icon or select FreeShape > Midplane... from the dropdown menu. 1. Select the first plane or the first reference face. 2. Select the second plane or the second reference face. 3. Reverse the direction, if necessary. Both arrows must be pointing toward the midplane. 4. Validate with the button.

The plane can be seen and edited only in FreeShape mode. By using this command, the plane is created inside the resolution of the FreeShape and therefore can only be modified or updated in FreeShape edit.

Pivoted plane

This command allows you to create a pivoted plane around another plane or face in a FreeShape element.

Creation Stages / Use: Click the icon or select FreeShape > Pivoted Plane... from the drop-down menu. 1. Select a reference plane. 2. Select the rotation axis. 3. Enter the rotation angle of the plane.

The plane can be seen and edited only in FreeShape mode. By using this command, the plane is created inside the resolution of the FreeShape and therefore can only be modified or updated in FreeShape edit.

Constrain Automatically Links / Videos:

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This command automatically creates constraints on FreeShape faces. This command is only available in FreeShape edit mode. To do this, use the "Edit" command in the shape's popup menu to switch to resolution edit mode. To finish editing in FreeShape, click the button at the top of the graphic area.

Creation Stages / Use: Click the icon or select the FreeShape > Constrain Automatically ... option from the drop-down menu. 1. Check the types of constraints that you wish to use. 2. Validate.

Only non-constrained faces (magenta) are managed with this command. Therefore, all fixed (gray), fully constrained (blues), and unconstrainable (yellow) faces cannot accept new constraints.

Available Options:

Automatic axes: This option automatically creates axes on the cylindrical surfaces and creates diameter dimensions and coaxiality constraints between the axes and the cylindrical surfaces.

Automatic orientations: This option automatically creates orientation constraints on the planar faces of the shape with respect to the support plane and its orthonormal planes. You can specify the angular tolerance to use to determine whether a face is coplanar.

Automatic tangency: This option automatically creates tangency constraints between the planar, cylindrical, and conical faces.

Angular tolerance: This value allows to define in which tolerance, the constraint should be applied. If the tolerance is set to 0.1° and if the angle between two faces is 0.05°, these two faces will become coplanar.

Dimension Links / Videos:

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This command allows you to create dimensions between FreeShape axes or faces, thereby modifying its dimensions. This command is only available in FreeShape edit mode. To do this, use the "Edit" command in the shape's popup menu to switch to resolution edit mode. To finish editing in FreeShape, click the button at the top of the graphic area.

Creation Stages / Use: Click the icon or select FreeShape > Dimension... from the drop-down menu. 1. Select the first geometry. 2. Select the second geometry. 3. Validate.

When changing the value of a dimension, the part's geometry is changed only on the faces that do not have a fixity constraint. TopSolid generally tries to comply with the new dimension indicated by changing the possible face minimum and complying with defined constraints.

Perpendicularity Links / Videos:

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This command allows you to create a perpendicularity constraint between two FreeShape geometries.

Creation Stages / Use: Click the icon or select FreeShape > Relations > Perpendicularity... from the drop-down menu. 1. Select the first geometry. 2. Select the second geometry. 3. Validate.

If two geometries aren't totally constrained, they can move. If two geometries are totally constrained, this relation will not be applied.

Coaxiality Links / Videos:

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This command can add a coaxiality constraint between two FreeShape elements.

Creation Stages / Use: Click the icon or select FreeShape > Relations > Coaxiality... from the drop-down menu. 1. Select the first geometry. 2. Select the second geometry. 3. Validate.

If two geometries aren't totally constrained, they can move. If two geometries are totally constrained, this relation will not be applied.

Tangency Links / Videos:

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This command allows you to create a tangency constraint between two FreeShape faces.

Creation Stages / Use: Click the icon or select the FreeShape > Relations > Tangency... command from the drop-down menu. 1. Select the first geometry. 2. Select the second geometry. 3. Validate.

If two geometries aren't totally constrained, they can move. If two geometries are totally constrained, this relation will not be applied.

Orientation along an axis Links / Videos:

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This command allows you to create a constraint on the orientation of a FreeShape line (ex. hole axis) alone one of the axes of the FreeShape reference plane.

Creation Stages / Use: Click the icon or select FreeShape > Relations > Orientation Along Axis... from the drop-down menu. 1. Select the line/axis whose orientation you would like to constrain.

The orientation constraint is automatically created with respect to the reference frame axis whose orientation is the closest to the selected line.

Orientation along a plane Links / Videos:

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This command allows you to create a constraint on the orientation of a FreeShape face along one of the orthonormal planes of reference in FreeShape.

Creation Stages / Use: Click the icon or select the FreeShape > Relations > Orientation along a plane... command from the drop-down menu. 1. Select the planar face whose orientation you would like to constrain.

Alignment Links / Videos:

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This command constrains the alignment of two FreeShape points along one of the axes of the FreeShape reference plane.

Creation Stages / Use: Click the icon or select FreeShape > Relations > Alignment... from the drop-down menu. 1. Select the first point. 2. Select the point. 3. Validate.

The alignment constraint is automatically created with respect to the reference frame axis whose orientation is the closest to the direction defined by the two selected points.

If two geometries aren't totally constrained, they can move. If two geometries are totally constrained, this relation will not be applied.

Coincidence Links / Videos:

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This command can add a coincidence constraint between two FreeShape elements.

Creation Stages / Use: Click the

icon or select FreeShape > Relations > Coincidence... from the drop-down menu.

1. Select the first element. 2. Select the second element. 3. Validate.

If two geometries aren't totally constrained, they can move. If two geometries are totally constrained, this relation will not be applied.

Centering Links / Videos:

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This command can add a centering constraint between two FreeShape elements.

Creation Stages / Use: Click the icon or select FreeShape > Relations > Centering... from the drop-down menu. 1. 2. 3. 4.

Select the first geometry. Select the second geometry. Select the geometry. Validate.

If two geometries aren't totally constrained, they can move. If two geometries are totally constrained, this relation will not be applied.

Parallelism Links / Videos:

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This command allows you to add a parallelism constraint between two FreeShape elements.

Creation Stages / Use: Click the icon or select FreeShape > Relations > Parallelism... from the drop-down menu. 1. Select the first geometry. 2. Select the second geometry. 3. Validate.

If two geometries aren't totally constrained, they can move. If two geometries are totally constrained, this relation will not be applied.

Fixity Links / Videos:

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This command allows you to add a fixity constraint to a FreeShape geometry.

Creation Stages / Use: Click the icon or select FreeShape > Relations > Fix... from the drop-down menu. 1. Select the geometry on which you would like to add the fixity constraint.

Faces with a fixity constraint appear in gray. When converting a shape in FreeShape, all of the faces are fixed. You must therefore delete the fixity constraint on the faces to be "freed" for the purpose of geometric or dimensional changes to the part. To delete the fixity relationship, select the fixed element and then choose the Remove fixity command from the popup menu displayed when right-clicking. In order to simplify the entities tree display, the fixity constraints symbols are not displayed into the constraints list of the FreeShape.

Ask dimension value

This mode allows asking for the dimension value to be enabled or disabled.

Use: Click the icon or select the FreeShape > Modes > Ask dimension value... command from the drop-down menu. When this mode is enabled, the value of the dimension put in is proposed, all you need to do is validate or modify it. When this mode is disabled, the dimension is put in without its value being asked for.

Modifications: The modification of the value of a dimension is made by doubleclicking on the dimension text when no command is launched (neutral mode).

Additional information: This mode is enabled when the icon is pressed (the background remains colored).

Show relations

This mode allows the display of relations to be enabled or disabled.

Use: Click the icon or select the FreeShape > Modes > Showr relations command from the drop-down menu. When this mode is enabled, the relations (alignment, horizontal, vertical, tangency, coincidence, ...) are visible. When this mode is disabled, the relations are not displayed.

Additional information: This mode is enabled when the icon is pressed (the background remains colored).

Overview of the sheet metal commands Sheet metal design is an integral part of the design commands of TopSolid. These commands will enable you to design sheets and to carry out their unbending in compliance with the unbending rules. These are divided into three major categories: Creation commands: from the sketch (Sheet metal on sketch), from shapes (Sheet metal by thickening) or from documents from other CADCAM software (Sheet metal recognition). Modification commands: Flange, Bends upon edge, Bend along a line, Angle relief, Edge relief, Standard layout and Change faces side Unbending commands: Unfolding rules... The unbending is then done in a unfolding document which also contains the part to unbend. What is an unfolding surface?: A lot of definitions are available, but intuitively, each surface which can be created with a lofted surface between 2 curves or between a curve and a point can be considered as unfoldable for an unfolding operation. Examples of unfolding surfaces: - Cylinders - Cones - Extruded surfaces - Inclined cylinders - Inclined cones - Inclined pipes - Helix These surfaces are characterized by the presence of linear section curves in one or two of their main directions. Strictly speaking, a surface is unfoldable if, along one of each section curve, all normals to the surface are parallels. In the opposite case, the surface is said "quasi developpable". TopSolid allows to unfold this kind of surfaces, but they are modified by adding an additional deformation, so they are not strictly "rollable". With transition part, we are sometimes forced to use this kind of surfaces, if the additional deformation is low. In this case, we add some intermediate folding lines to allow the manufacturing by crunch faces.

If this deformation is too important, the shape obtained after manufacture will not be strictly the same the initial surface used to create the unfolding.

Developpable surface

Quasi developpable surface (normal in red are not parallels between themselves along iso curves in green).

Sheet metal on sketch

Links/Videos:

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This command creates extruded sheet metal from an open or closed plane sketch.

Creation stages / Use: Click the

icon or select Sheet metal > Sheet Metal on sketch... from the drop-down menu.

1. Enter the value of the thickness of your sheet metal (the Invert mode inverts the direction of thickness of the basic shape of the sheet metal). 2. Select the type of basic shape: Extruded shape: The section (not filled) is extruded directly, the sheet metal is achieved by thickening at the indicated value of the extruded shape. Flat shape: A flat shape is created on the section, the sheet metal is achieved by thickening at the indicated value of the flat shape. This option is not available for an open section. Section to be extruded

Sheet metal with extruded shape

Sheet metal with flat shape

3. Select the section to be extruded. 4. Define its extrusion limit (see below for available options for the different modes). 5. Validate the sheet metal creation with the button.

Available Options: Limit (Extruded shape mode only): You can define the extrusion limit in several ways: Length: Enter the value for the extrusion height Offset limit: When a limit of type Point, Plane, Surface, Face set or Shape has been defined,it is possible to add a positive or negative offset according to this limit. The Reverse option reverses the extrusion direction of the section, this mode is not available when the Center mode is checked. Center (Extruded shape mode only):

By checking this option, the operation is mode symmetrically on both side of the section. If you enable this option, then the operation limit can only be defined by a length. Second side: If the basic shape is an extrusion and it is not centered, a second side can be entered (limits, offset, ...) Offset: Using this option, you can offset the start of the extrusion by a distance given in relation to the section. The check box Negate allows you to apply the offset in the opposite direction of the extrusion. Bends: By checking this option, you can add bends to each vertex of your section. These bends can be defined by different ways: The indicated radius corresponds to the inner bending radius. Manual: The radius has to be entered. Thickness: The radius is synchronised with the thickness of the sheet metal. Unfolding rules: The radius of bend to use is search in the table defined in the unfolding rules associated to the part. According to the thickness of the sheet metal to consider, TopSolid uses the first favorite bending radius found in the list of available radii. The Delimit bends option allows to isolate faces of the bend from those of connected faces for example to be able to use the covering.

If an unfolding rule is selected, bends defined in this rule are displayed with green highlight

Thickness Split: This option defines the position of the neutral fiber, the value indicated must be between 0 and 1. (it is a factor).

Sheet metal by thickening

Links/Videos:

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This command creates a sheet metal by thickening of one or more faces of a shape.

Creation stages / Use: Click the icon or select Sheet Metal > Sheet Metal by Thickening... from the dropdown menu. 1. Select the shape to transform to sheet metal (the handle and thickness modification label will be created on this face). 2. Enter the value of the thickness of your sheet metal (the Invert mode inverts the direction of thickness of the basic shape of the sheet metal). 3. Select the special faces of your shape and their conservation mode: Faces to Ignore: Only the selected faces are used to create the sheet. Basic shape with selected faces in red.

Resulting sheet metal

Faces to Consider: The faces selected are not used to create the sheet. Basic shape with selected faces in red.

Resulting sheet metal

Faces with inverted thickness: This option inverts the thickness of the selected faces, it can be very useful during the sheet design supported on the faces. Root face (View from above)

Option unchecked: The resulting sheet metal remains parallel to the basic shape.

4. Validate the sheet metal creation with the

Option checked with inversion of thickness of the upper face.

button.

Available Options: Bends: By checking this option, you can add bends to each vertex of your selection. These bends can be defined by different ways: The indicated radius corresponds to the inner bending radius. Manual: The radius has to be entered. Thickness: The radius is synchronised with the thickness of the sheet metal. Unfolding rules: The radius of bend to use is search in the table defined in the unfolding rules associated to the part. According to the thickness of the sheet metal to consider, TopSolid uses the first favorite bending radius found in the list of available radii. Check the All sharp edges option to rapidly create a bend with the inner bend radius indicated on all the square edges of your parts. The Delimit bends option allows to isolate faces of the bend from those of connected faces for example to be able to use the covering.

Without Delimit bends option

With Delimit bends option

This option can be activated by editing the command or by using the Delimiting of Bend command.

When you have indicated the bends on certain edges, the Break square edges option automatically creates edge relief operations with the offset value indicated on the remaining square edges.

Thickness Split: This option defines the position of the neutral fiber, the value indicated must be between 0 and 1. (it is a factor).

Transition Sheet Metal

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This command allows you to create sheet metal between 2 sections. (for example, a hopper)

Creation stages / Use: Click the 1. 2. 3. 4.

icon or select Sheet metal > Transition Sheet Metal... from the drop-down menu.

Check Surface Only to not manage the width. The sheet metal will be a surface sheet metal. If the option below is not checked, enter the thickness of the sheet metal. Indicate whether or not the dimensions indicated are external dimensions. Select the transition type. Point and Point: Allows you to define the transition by 2 points. Select the first point. Select the second point. Select the orientation of the sections. (X direction of sections). Must be normal to the direction of the 2 points. Point, Direction and Height: Allows you to define the transition by a point, direction or height. Select the first point. Select the direction. Enter the positioning height of the second profile. Select the orientation of the sections. (X direction of sections). Must be normal to the chosen direction. Point, Direction and Point: Allows you to define a transition by 2 points and a direction. Select the first point. Select the direction. Select the second point. Select the orientation of the sections. (X direction of sections). Must be normal to the chosen direction.

No Orientation

5.

With Orientation

Select the geometry of the first section and inform the dimensional values. If the geometry is not proposed or if it exists, click User section

and select the profile.

6. Enter the incline angle of the first section. If the incline is not around the proper axis, the orientation of the sections must be modified (see explanations in section 4. Choice of transition types below). 7. Select the incline direction of the first section. It is preferable to select the same direction as the direction between the 2 sections.

No Incline

With Incline

8. Select the geometry of the second section and inform the dimensional values. 9. Enter a longitudinal and/or lateral shift value if necessary.

Without shift

With shift

10. Enter the orientation angle that allows you to turn the second section around the direction.

Without Orientation

With Orientation

11. Enter the incline angle of the second section. (see above images) 12. Select the inclination direction for the second profile.

If two sections use Circle mode, the Conical surface option will be available in the second section. This option ensures to have a surface strictly developable, to the detriment of the geometry of the second section which will no longer be strictly circular. The position of crunching lines will be modified accordingly.

This option does not allow a lateral misalignment.

Obtained shapes comparison with and without the conical surface option. Obtained shapes comparison with and without the conical surface option. The blue surface is obtained without activating the Conical surface option. the blue section is circular. Blue lines on the surface are used for the crunching surface. The green surface is obtained by activating the Conical surface option. The main surface of the shape is an angled cone. The green section is an ellipse. Green lines on the surface are used for the crunching surface. The superposition of the crunched lines shows the difference between these 2 constructions.

Unfoldings comparison. Both unfoldings are really different. (the unfolding with blue lines comes from the blue surface, green lines from the green surface).

It is not necessary to create profiles before creating the transition sheet metal, except when profiles are created by the user. If the second profile is identical to the first (without orientation or offset), check this section.

You cannot use both a standard profile and a user profile. If the user profile is used, the 2 profiles must be created by the user. the user section mode can only manage sections with a similar type as those proposed with others modes (circle, ellipse, square, rectangle, slotted) There are no values to enter for user profiles. It must be well positioned and oriented.

Flange

Links/Videos:

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This command adds a linear part to a sheet part utilizing the length of one of its edges..

Creation stages / Use: Click the

icon or select Sheet Metal > Flange... from the drop-down menu.

1. Select the flange edge Click yellow handles for a rapid and dynamic modification of the length and the angle of your flange. Double-click the labels to enter the length and angle values of the flange.

(several edges can be selected to create several identical flanges). 2. Enter the bend parameters (inner radius, angle, position). 3. Enter the length of the flange. 4. Enter the width of the flange. 5. Indicate the parameters of the notches. 6. Validate the creation of the flange with the button.

Click yellow handles for a rapid and dynamic modification of the length and the angle of your flange. Double-click the labels to enter the length and angle values of the flange.

Available Options: Bends: This section allows you to define the bend parameters: the position in relation to the edge selected. Bend upon edge: The flange is offset form the selected edge. The distance is the bend radius. Thickness upon edge: The inner face of the flange is coincident with the selected edge. Thickness below edge: The outer face of the flange is coincident with the selected edge. the bend radius calculation mode: Manual: Enter the inner bend radius.

Thickness: The inner bend radius is the thickness. Unfolding rule: The inner bend radius is defined by an unfolding rule regarding the thickness and the material. the bend angle the additional length: Basic sheet without flange

Flange with a null additional height (bend upon edge)

Flange with an additional height (bend upon edge)

When the reference face of the flange (face used to calculate the angle) is cylindrical, the Thickness on the edge mode and Thickness under the edge are not functional.

Length: This section defines the length of the flange: Select the mode for calculating the length: Enter the value of the length of the flange. Tangent length: The length is calculated in relation to the tangent to the bend radius. External length: The length is calculated in relation to the external face connected to the flange. Internal length: The length is calculated in relation to the tangent of the inner bend radius. Linear part length: The length is calculated on the plane part of the flange. Enter the flange offset value if needed. This offset is the distance between the entered length and the real length of the bend. For example if the bound is defined as plane and if a plane is selected, the offset will be the distance between this plane and the bound of the bend.

Width: This section defines the width of the flange: Select the calculation mode of the width: No shift: The width of the flange equals the length of the edge. Symmetric shift: The flange is centered on the middle of the selected edge. Start and end shifts: The arrow drawn on the selected edge indicates the direction

Start shift and width: The arrow drawn on the selected edge indicates the directio Width: The flange is centered on the middle of the selected edge. Enter the values of offset and/or width of the flange. The option Close neighbor borders allows, when several edges are selected, to have bor in account. Without Close neighbor borders option Select the type of bend transition: Trimmed bend

Adjusted

Line

Arc

Double arc

With Close neighbor borders option

The Release bends extremities option allows to operate neighboring bends of the selecte Notches: This section defines the notches located on each side of the bend:

Select the type of notches: - Rectangular - Oblound, Depth of arc bottom - Oblound, Depth of arc center Enter the values of width and depth of the notches. If a bend is not defined on an edge, you can select the depth origin: Edge or Line

Base of bend

Enter the value of the extra thickness to precisely adjust flanges for some configurations (see pictures below).

Start and end notches must be identical (type and parameters).

Advanced options: When the flange is made on several edges, you can indicate a gap for the auto-trim of the flange: This gap corresponds to the width of the slot where the flanges should intersect.

By activating the Create sketch option, TopSolid creates a sketch (rectangular) for each flange, you can then modify the shape of the flange by editing the corresponding sketch.

Modifications / Additional information: When the flange is created, a double click on one face of the flange displays the main driver dimensions (length, angle, inner radius, width, etc.). The bend angle cannot be higher or equal to 180°, otherwise another reference face must be indicated.

Hem bend

Links/Videos:

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This command bends the extremity of a sheet on itself.

Creation stages / Use: Click the icon or select Sheet Metal > Hem Bend... from the drop-down menu. 1. Select the edge of the bend (several edges can be selected to create several identical hem bends). 2. Enter the length of the bend. 3. Enter the gap in relation to the reference face (this gap corresponds to the inner diameter of the bend). 4. Select the bend position regarding the selected edge: The bend is done under the selected edge, the initial length of the sheet is not modified. The bend is done on the selected bend, the initial length of the sheet is extended (gap/2 + thickness of the sheet).

Corresponding parameters: Length

Gap

A hem bend cannot be done when the reference face of the bend (face used to calculate the gap) is cylindrical.

Available Options: Additional rolling: By default, the inner face of the bend is parallel to the reference face, the additional rolling angle curves the bend towards the reference face of the value of the indicated angle:

The Automatic rolling curves the bend towards the reference face until the trimming gap defined in the Advanced options section is reached. Bend below edge: The bend will not exceed the edge. The sheet metal overall length will not change. Bend upon edge: The bend starts at the edge. The sheet metal overall length will change.

Width: This section defines the width of the flange: Select the calculation mode of the width: No shift: The width of the flange equals the length of the ed

Symmetric shift: The flange is centered on the middle of th Start and end shifts: The arrow drawn on the selected edge Start shift and width: The arrow drawn on the selected edg Width: The flange is centered on the middle of the selected Enter the values of offset and/or width of the flange. The option Close neighbor borders allows, when several edges a in account. Without Close neighbor borders option Select the type of bend transition: Trimmed bend

Adjusted

Line

With Close n

e

Arc

Double arc

The Release bends extremities option allows to operate neighbor Notches:

This section defines the notches located on each side of the bend:

Select the type of notches: - Rectangular - Oblound, Depth of arc bottom - Oblound, Depth of arc center Enter the values of width and depth of the notches. If a bend is not defined on an edge, you can select the depth origin: Edge or Line

Base of bend

Enter the value of the extra thickness to precisely adjust flanges for some configurations (see pictures below).

Start and end notches must be identical (type and parameters). Advanced options: When the flange is made on several edges, you can indicate a gap for the auto-trim of the flange: This gap corresponds to the width of the slot where the flanges should intersect.

This gap is also used when calculating the Automatic rolling.

Covering Links/Videos:

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This command rapidly "fills up" the space between two lateral faces of a sheet by extruding the faces until their intersection.

Creation stages / Use: Click the

icon or select Sheet Metal > Covering... from the drop-down menu.

1. Select the type of covering: Covering type: The first face selected covers the second. Symmetrical type: The faces are extended up to their intersection. Extended type: The face selected is extended by a given distance.

2. Select a face, TopSolid proposes the nearest intersecting neighboring face or extends the face of the value indicated if the Extended mode was previously selected. You may then select other faces. 3. Validate the creation of the covering with the button.

With Covering type, a double-click on the arrow extremity allows to reverse the covering face.

Available Options: Gap: This parameter controls the gap between two covered faces:

Covering: These parameters controls the gap between two covered faces: Proportion: Enter a value between 0 and 1. The value 0 does not correspond to any covering, the value 1 corresponds to a full covering. The additional value is a length totaling the proportion indicated. Bound: The extend can be done regarding the planar faces, a point or a plane to select or regarding a length to enter. For the bounds like planar faces, point or plane, a negative or positive offset can be entered. Advanced options: The Direction option controls the extrusion direction of the covering: Root bend: The extrusion direction is parallel to the direction of the bend.

Normal: The extrusion direction is perpendicular to the face selected.

Swept flange

Links/Videos:

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This command creates a flange along a path of edges on a piece of sheet metal

Creation stages / Use: Click the

icon or select Sheet Metal > Swept Flange... from the drop-down menu.

1. Select the edges of the flange (path), the edges selected must be boundary edges connected to each other. 2. Enter if needed Radii to ignore. It is possible to enter a radius to define edges to ignore along the path of the swept flange. This value is optional. 3. Select the mode for defining the generator of the swept flange: Profile

Length + angle

The bend is defined by a sketch. This sketch is moved along the path, it must be positioned the path and in the normal plane at the first path director. The sketch must be open and the with the side face connected to the boundary edge must be between 0° and 270°. Inverting inverts the side of the swept flange. Select the position in relation to the selected edge. Bend upon edge: The flange is offset form the selected edge. The distance is the bend radius. Thickness upon edge: The inner face of the flange is coincident with the selected edge. Thickness below edge: The outer face of the flange is coincident with the selected edge. The bend is defined by a length and an angle. The defined line is moved along the path. Bend upon edge: The flange is offset form the selected edge. The distance is the bend radius. Thickness upon edge: The inner face of the flange is coincident with the selected edge. Thickness below edge: The outer face of the flange is coincident with the selected edge. Enter the length of the flange. Select the length calculation mode: Enter the value of the length of the flange. Tangent length: The length is calculated in relation to the tangent to the bend radius External length: The length is calculated in relation to the external face connected t flange. Internal length: The length is calculated in relation to the tangent of the inner bend radius. Linear part length: The length is calculated on the plane part of the flange. Enter the angle. Enter if needed, the additional height to apply for the generator profile of the flange.

3. Validate the creation of the swept flange with the

button.

Available Options: Bends: By checking this option, you can add bends to each used edge. These bends can be defined by different ways: The indicated radius corresponds to the inner bending radius. Manual: The radius has to be entered. Thickness: The radius is synchronised with the thickness of the sheet metal. Unfolding rules: The radius of bend to use is search in the table defined in the unfolding rules associated to the part. According to the thickness of the sheet metal to consider, TopSolid uses the first favorite bending radius found in the list of available radii. The Delimit bends option allows to isolate faces of the bend from those of connected faces for example to be able to use the covering.

Without Delimit bends option With Delimit bends option This option can be activated by editing the command or by using the Delimiting of Bend command.

Edge Relief: By checking this option, you can enter the gap and extension values of the edge relief. Shifting value: This parameter controls the gap between the two faces of the edge relief:

Extension value: This parameter controls the release for the relief tool. When the faces are not perpendicular, without extension, the edge may not be fully broken. In this case, the sheet is not unbendable.

The edge relief can only affect the part created by the swept flange or it can extend along the tangent edges: Non-extended edge relief

Extended edge relief

Offset: An offset value can be added at the start and end of the edge path. This function is not available when the path is closed.

Example of swept edge with offset at the start and end of the path

Notches: This section defines the notches located on each side of the bend:

Select the type of notches: - Rectangular - Oblound, Depth of arc bottom - Oblound, Depth of arc center Enter the values of width and depth of the notches. If a bend is not defined on an edge, you can select the depth origin: Edge or Line

Base of bend

Enter the value of the extra thickness to precisely adjust flanges for some configurations (see pictures below).

Start and end notches must be identical (type and parameters).

Forming flange straightening

Links/Videos:

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This command allows you to straighten the fallen edges and create trunk corners.

Creation stages / Use: Click the

icon or select Sheet Metal > Forming flange straightening... from the drop-down menu. Face Straightening: 1. Select the face that will not be straightened . 2. Select the border edges between the reference face and the fallen borders. (the edges have to be s 3. Select the straightening mode. Deletion: Allows you to delete the fallen border. Extension: Allows you to extend the reference face by entering an extension value. Extension by measurement: Allows you to extend the reference face. The extension len automatically calculated by taking into account the length of the rounding + the length of t flange. The selection point on the border is therefore important

Initial Sheet Metal

After Deletion

After Extension

After Extension by Measurement

The forming flange straightenings are always created by extending border edges.

Sheet metal to straighten (perspective view)

Sheet metal to straighten with boundary edge (top view)

Straightened sheet metal (top view)

Extension on unfolding: This mode allows to define on the 3d part extension areas. They will be automatically reported on the un on the 3d. Edges to extend have to be identified as well as the extended value to apply. Edges to extend can be on the boundary of the part to treat. In this case the extension will be added on t

Example of Forming flange straightening only on the unfolding. They can also be in the part. In this case, the extension will replace the area of the part identified by the o

Round corner: This mode allows to create an unfolding shape of a «round corner». Several configurations are supported: 3 connected edges (the design must be completed by a slot).

Initial Sheet Metal

3 connected edges

2 connected edges.

Initial Sheet Metal

Result

Initial Sheet Metal

Result

Initial Sheet Metal

In order to not work on the basic part, you can create a derived part.

Available Options: Keep Border Edges: Allows you to mark the face at the location of the borders.

Result

Bend on edge Links/Videos:

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This command creates bends on square edges of a part of sheet metal.

Creation stages / Use: Click the

icon or select Sheet Metal > Bend on Edge... from the drop-down menu.

1. Select the mode for managing the inner bend radius: Identical: the same inner bend radius is applied to all bends. Different: the inner bend radius is managed independently on each bend. Bends can be defined by different ways: The indicated radius corresponds to the inner bending radius. Manual: The radius has to be entered. Thickness: The radius is synchronised with the thickness of the sheet metal. Unfolding rules: The radius of bend to use is search in the table defined in the unfolding rules associated to the part. According to the thickness of the sheet metal to consider, TopSolid uses the first favorite bending radius found in the list of available radii.

2. Enter the value of the inner bend radius (radii). 3. Select the edges. 4. Validate the bends creation with . Only the edges with a relevant edge on the opposite face of the sheet can be selected.

Available Options: The All bends option rapidly selects all the square edges of the parts. This mode est associative, if a modification after the creation of bends on edges generates a square edge on the part, a bend will automatically be created on this edge. By default, the bend is calculated up to the neighboring faces, the Limit to extremities option makes a bend only on the length of the edge selected. The Delimit bends option allows to isolate faces of the bend from those of connected faces for example to be able to use the covering.

Without Delimit bends option

With Delimit bends option

This option can be activated by editing the command or by using the Delimiting of Bend command.

Bend along a line

Links/Videos:

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This command allows to bend a sheet along a line or an edge.

Creation stages / Use: Click the

icon or select Sheet Metal > Bend Along Line... from the drop-down menu.

1. Select the face(s) to bend. 2. Select a bending line type (extended line, line or edge). 3. Depending on the chosen selection mode, select : either a line then an edge on the fixed side of the sheet (this edge must not intersect the bending line). or an edge of the face to bend. 4. Enter the bend parameters (inner radius, angle, position). 5. Validate the creation of the bend with the button.

The bending line must be created beforehand in a sketch with only one segment.

Available Options: Faces to bend: You can select several faces to bend. To allow this type of bend, these faces must be coplanar:

Selection of 2 coplanar faces enabling to bend this shape in this area

Bending line: The bending line may be defined by a line (sketch) or an edge:

Extended line

Line

Edge

The bend line is extended on all the face to bend.

The bend is carried out along the length of the line (this must be at least equal to the length of the part to bend).

The bend is carried out on the selected edge. This edge must not be connected to a lateral face.

The bend line is represented in red

Bend: (Only for the Line or the extended line options). This section allow you to define the bend parameters for a bending line like Extended line or Line: the bend radius calculation mode: Manual: Enter the inner bend radius. Thickness: The inner bend radius is the thickness. Unfolding rule: The inner bend radius is defined by an unfolding rule regarding the thickness and the material. the bend angle the position in relation to the selected edge: Rolled

The face of the bend starts at the bend line.

Thickness under the line

When we are placed between the fixed edge in green and the bend line in red, the thickness of the bended sheet is located under the line.

Thickness on the line

When we are placed between the fixed edge in green and the bend line in red, the thickness of the bended sheet is located on the line.

Centered

When the sheet is flat, the bend is centered on the bend line.

the shift allows to move the bend in parallel with the line, its value can be negative.

Bend: (Only for the Edge option). Whole face: The goal is to have a rolling of the face which matches with the length of this face (by taking into account the used unfolding rule). Given angle: Enter the angle. The radius is automatically calculated. Given radius: Enter the radius. The angle is automatically calculated. Given angle and radius: Enter the angle and the radius. In this cas, the unfolding rules aren't taken into account.

This Whole face option is rather destined to TopSolid'Strip.

This section allow you to define the bend parameters: it is not available if Whole face with Given angle is checked. the bend radius calculation mode: Manual: Enter the inner bend radius. Thickness: The inner bend radius is the thickness. Unfolding rule: The inner bend radius is defined by an unfolding rule regarding the thickness and the material. the bend angle the position in relation to the selected edge:

Notches: (not available for extended bending line).

This section defines the notches located on each side of the bend:

Select the type of notches: - Rectangular - Oblound, Depth of arc bottom - Oblound, Depth of arc center Enter the values of width and depth of the notches. If a bend is not defined on an edge, you can select the depth origin: Edge or Line

Base of bend

Enter the value of the extra thickness to precisely adjust flanges for some configurations (see pictures below).

Start and end notches must be identical (type and parameters).

Trimming profile: Check this option to limit the face to bend by a profile (open). This profile must have two intersections with the bend line. Example: The bend line is in red, the trimming profile in green.

Clearance can be indicated between the reference face of the sheet and the bent face, checking the Invert box positions this clearance inside or outside the trimming profile.

Dimpling: Check this option to create a dimpling. Enter the dimpling height. Select the dimension position .It can be between external faces, between internal faces or a global dimension. A second bending radius can be entered. By default, it has the same radius than the face to bend.

Unbending method:

Refer to the unfolding rules command for more details.

Advanced options: Hide tools: This option allows to hide or not the sketch of the selected line. Allow surface result: If errors are found, a message is displayed and you can get a surface shape thanks to this option.

Modifications / Additional information: The bend angle cannot be higher or equal to 180°, otherwise another reference face must be indicated.

Unbending Links/Videos:

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This command allows you to locally unfold a (or several) bend(s), in order to remove the bend and if required in the neighboring faces, then to rebend it.

Creation stages / Use: Click the icon or select Sheet Metal > Unbending... from the drop-down menu. 1. Select a fixed edge of the sheet. 2. Select faces of the bend(s) to unbend. 3. Validate the creation of the unbending operation with the button.

Select a bend by clicking on a cylindrical face of the bend.

Available Options: The All bends option automatically unbends all the bends of the part. This mode is associative, if a modification after the creation of the unbending operation generates a bend, this bend will automatically be unbent. Unbending method:

Refer to the unfolding rules command for more details.

Corners relief: This option allows you to add corners relief on the unbending at the intersection of the center of the unbending bends. It allows to modify on parts coming from import and conversion to sheet metal to enable their industrialization punching. Only neighboring bends connected to the same base surface will be considered. Corners relief type / Dimensions: Select the corner relief type to use (spherical or cubical) and its dimension. Extract on unfolding: Created corners relief can be extracted on the unfolding to have straight edges.

Example of unbending of bend with corners relief

Advanced options: Allow surface result: When reconstruction problem of the lateral faces of rebent bends is detected, the sheet is then invalid. This option allows a valid

sheet to be achieved nevertheless but the result will be on the surface. Without bend lateral face: In some complex cases, this option allows to ignore the lateral faces rebuild steps which can be complex and which can failed the operation. In this case, the Allow surface result option must be checked.

When no value or rule is specified for the unfolding rules and the unbending methods, the default method is that of neutral fiber i i d 0 5 (K f 05 ih i )

Modifications / Additional information: This command can process bends with zero internal radii, but there must be one cylindrical bend face on the external side. It is also possible to unroll a cylindrical face by itself, or a succession of cylindrical faces.

Example of unbending a bend from a sheet with cylindrical faces (in blue).

Rebending Links/Videos:

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This command unbends a flat bend with the Bend unbending command.

Creation stages / Use: Click the

icon or select Sheet Metal > Rebending... from the drop-down menu.

1. Select the Mode : Bend or Bend with transformation Bend Current use Bend with transformation We use this option for the parts with deformation made before the folding : like a pocket, chamfer, groove

2. Select a fixed edge of the sheet metal. 3. Select the faces of the bend(s) to rebend. 4. Select all the faces to deforms To Select the faces easier, uncheck the preview

5. Validate the rebending with the

button.

The selection of a bend is done by clicking on a face of the flat bend. For the Bend with deformation, cut the bend with an imprint before choose the part to deform.

Available Options: The All bends flat option automatically rebend all the unfolded bends of the part. This mode is associative, if a modification before the creation of the rebending operation generates the unfolding of a bend, this bends will automatically be rebent. Advanced options: Allow surface result: When reconstruction problem of the lateral faces of rebent bends is detected, the sheet is then invalid. This option allows a valid sheet to be achieved nevertheless but the result will be on the surface. Without bend lateral face: In some complex cases, this option allows to ignor the lateral faces rebuild steps which can be complex and which can failed the operation. In this case, the Allow surface result option must be checked.

Modifications / Additional information: If an unfolded bend is cut in two by an operation, both bends will be rebent.

Delimiting of Bend Links/Videos:

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This command adds edges from start to end of bend to the lateral faces.

Creation stages / Use: Select the Sheet metal > Delimiting of bend... command from the drop-down menu. 1. Select the (internal or external) face of on or several bend(s). 2. Validate the creation of delimiting with the button.

Modifications / Additional information: This command is particularly useful when we wish to do a covering with a sheet created from the extrusion of a sketch. In this case, the lateral faces are only made up of a single face which does not enable the desired result to be achieved. Example:

Creation of a sheet on sketch from the red sketch. We can see that the lateral face (green) is only made up of a single face.

Creation of a flange on an edge.

Bends delimiting, the red edge is then added to the lateral faces of the bend.

After delimiting, the covering operation can be carried out on a part of the lateral face.

During the creation of a covering operation, one part of the lateral face cannot be selected.

Angle relief Links/Videos:

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This command allows rapid production of fillets or 45° chamfers on the lateral faces of a sheet.

Creation stages / Use: Click the icon or select Sheet metal > Angle Relief... from the drop-down menu. 1. Select the type of corners to be made (fillet or chamfer). 2. Select the mode for managing fillets or chamfers: Identical: the same radius or chamfer value is applied to all the edges selected. Different: the radius or chamfer value is managed independently on each edge selected. 3. Enter the value of the fillet(s) or chamfer(s). 4. Select the edges. 5. Validate the creation with the button.

Only edges of lateral faces of the sheet metal may be selected.

Relief assistant Links/Videos:

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From thick sheet metal defined without a bend radius or relief and from a basic face, this command allows you to create corner reliefs, edge reliefs and the associated bends in one operation. It allows you to unbend the sheet metal in one operation.

Creation stages / Use: Click the

icon or select Sheet Metal > Relief Assistant... from the drop-down menu.

1. Select the reference face. 2. validate by clicking .

The shape must first be converted into sheet metal and for density shapes before conversion, a face must be removed.

Converted Sheet Metal

Result by clicking the back face

Available Options: Corner Relief: Allows you to automatically add corner reliefs. Select Spherical or Rectangular. Spherical type corner relief Rectangular type corner relief Enter the corner relief value. Check or uncheck Extract on Draft to place or not place corner reliefs on the flattening.

Edge Relief: Allows you to automatically add edge reliefs. Select Symmetrical or Welded. Symmetrical edge relief

Welded edge relief

Enter the shifting value. This setting controls the shifting between the two faces of the edge relief. Enter the extension value. This parameter controls the release for the relief tool. When the faces are not perpendicular, without extension, the edge may not be fully broken. In this case, the sheet is not unbendable.

Bends: By checking this option, you can automatically add bends. These bends can be defined by different ways: The indicated radius corresponds to the inner bending radius. Manual: The radius has to be entered. Thickness: The radius is synchronised with the thickness of the sheet metal. Unfolding rules: The radius of bend to use is search in the table defined in the unfolding rules associated to the part. According to the thickness of the sheet metal to consider, TopSolid uses the firs favorite bending radius found in the list of available radii. The Delimit bends option allows to isolate faces of the bend from those of connected faces for example to be able to use the covering.

Without Delimit bends option With Delimit bends option This option can be activated by editing the command or by using the Delimiting of Bend command.

Modifications / Additional information:

You can modify or subtract the relief assistant using the popup menu or the operations tree.

Corner relief Links/Videos:

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This command removes a vertex with a tool to avoid a roll of material during bending.

Creation stages / Use: Click the

icon or select Sheet Metal > Corner Relief... from the drop-down menu.

1. Select the type of corner relief: Spherical type corner relief Cubical type corner relief

2. Select the Creation or Identification mode: The creation mode allows to create a corner relief, the identification mode allows to recognize one of the corner relief created by an unknown mode (with the creation functions like flange or recovering available in TopSolid or with an imported part converted as sheet metal). The corner relief extraction or simplification options available in the unbending document will be usable for these operations. Creation mode: 1. Select the vertexes of your part. 2. Enter the corner relief value. (sphere diameter or block dimensions ). Identification mode: Select the root face of the corner relief. It is a face where the corner reliefs (rectangular) are connected. In this case, TopSolid tries to automatically find them. If the faces are not found or if there are too many, it is possible to add or remove them in the Faces to consider or to ignore field. This command can be used with these usual configurations: Single recovering:

Double recovering:

3 bends intersection:

In each of these cases, the selected faces gap is signifiant and influences the result in the unfolding document.

2.

Enter the corner relief value. (sphere diameter or block dimensions).

if you only want to extract corners reliefs in the unfolding document, the kind of selected corner relief is n signifiant.

3. Validate the creation of the corner relief(s) with the button. Advanced options: Extract on unfolding: By checking this option, corner reliefs won"t be displayed in the unfolding document.

Corner Filler

This command allows you to fill the corners.

Creation stages / Use: Click the menu.

icon or select Sheet Metal > Corner Relief... from the drop-down

1. Select the different lateral faces of the corners or check all corners. 2. Select the method. Maximum Material: Allows you to "fill" the hole to its maximum. Minimum Material: Allows you to "fill" the hole to its minimum.

Initial Corner

3. Validate by clicking the

Maximum Material

Minimum Material

button.

Available options: Extend on tangent faces: This option allows you to solve some invalidity cases, it may be useful to uncheck it.

Edge relief Links/Videos:

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This command opens a sheet along an edge.

Creation stages / Use: Click the menu.

icon or select Sheet Metal > Edge Relief... from the drop-down

1. Select the type of edge relief: Symmetrical

Welded

2. Select the edges of the sheet. 3. Validate the creation of the edge relief with the

button.

Available Options: Shifting value: This parameter controls the gap between the two faces of the edge relief:

Extension value: This parameter controls the release for the relief tool. When the faces are not perpendicular, without extension, the edge may not be fully broken. In this case, the sheet is not unbendable.

Slot Links/Videos:

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This command produces a slot (material removal) based on a sketch.

Creation stages / Use: Click the

icon or select the Sheet metal > Slot... command from the drop-down menu.

1. Select the slot type to achieve. Path: Select one or several path(s) (segment, profile or section created before). For each path selected of the slot can be selected (right, center or left) in relation to the path and the direction which will be position any extremities. Enter the high and low overthicknesses. To image the overthickness, the slot can be an extruded th substracted rectangle. If there is not overthickness, the extrusion is done at the value of the sheet m thickness. It may cause problems in some cases. By 2 points: Select the 2 end points. Select the position of the slot in relation to 2 points. Enter the high and low overthicknesses. To image the overthickness, the slot can be an extruded substracted rectangle. If there is not overthickness, the extrusion is done at the value of the sheet thickness. It may cause problems in some cases. Open: This mode is intended for easily opening parts for which the initial shape is comparable to a tu transition shapes). If Plane is selected: From a face, an axis and a point, the slot is made in the passing plane by the point. If the selected face can provide an axis, the reference axis is automatically taken. If the sele a peak connected to a lateral face, it is automatically taken as the reference point. This point also complementary rotation origin of the cutting plane.

If Iso Parametric is selected: The slot is positioned according to the "pertinent" generator allowing correctly open the selected face. This mode is intended for opening developable faces such as th cones of hoppers.

Select the support face. Select the slot axis. Select a point if necessary. Enter an angle. Select the position of the slot in relation to the axis.

2. Select the shape to modify. 3. Enter the slot width value. 4. Validate the creation of the slot with the

button.

A slot can be produced on a lateral face, the depth is then equal to the sheet thickness.

Available options (For path and By 2 points): Extremities (first and second): By default, the length of the slot is equal to the length of the path, at each extremity, you can either extend the slot by a certain value (extension mode), or position the corner reliefs (spherical or cubic).

Example of slot with extension and spherical corner relief

If you select several paths, the extremities of each path will be the same type, the extremities of the different paths selected cannot be disassociated, in this case, it is advised to carry out several slotting operations.

Straightening lateral faces Links/Videos:

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This command straightens the lateral faces inclined perpendicularly to the faces of the sheet.

Creation stages / Use: Click the icon or select Sheet Metal > Straightening of Lateral Faces... from the drop-down menu, then select the edges of the faces to straighten.

Result: Sheet metal before straightening

Sheet metal after straightening

Standard Forming Links/Videos:

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This command modifies a sheet by inserting a pre-defined template.

Creation stages / Use: Click the

icon or select Sheet Metal > Standard forming... from the drop-down menu.

1. Select the shape to modify. 2. Select a Positioning frame from the template. 3. Enter the angle value of the rotation around the Z axis of the positioning frame. The Reverse option allows to reverse the forming side. 4. Select a pre-defined template and select a code or enter the driver values. 5. Validate the modification of the sheet with the button.

The pre-defined template can be added to a face of the sheet or a lateral face.

Modifications / Additional information: A pre-defined template can be repeated or copied on another face of the sheet.

Example of repeated shaping and associated unfolding.

The pre-defined template depends on the thickness of the sheet, if you modify the thickness of the sheet, you must be sure the template exists in this new thickness. The unfolding will not take into account the distortion created by inserting the component. It is possible to define in your templates, a substitution sketch. This sketch which will be inserted in place of the deformation frontiers on the unfolding. It can be composed of several profiles, it must be defined in the XY plane of the positioning frame and the generic document must provide the Standard Forming Unfolding Section (TopSolid Mechanical library) function.

It is possible to use a substitution section only if the deformation has a substraction tool and a non sheet metal union tool. Effectively, in the case of a single substraction tool, TopSolid considers that the user wants an opening corresponding to the shape of the tool. In the case of a sheet metal union tole, TopSolid considers that the user wants unbend the added section.

Deformation Links/Videos:

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This command deforms a sheet by stamping.

Creation stages / Use: Click the

icon or select the Sheet metal > Distortion... command from the drop-down menu.

1. Select the face of the sheet metal to modify. 2. Select the distortion mode: Tool

Distortion is done by an existing shape in the document.

Pocket

Distortion is done by the creation of a pocket on an existing closed sketch.

Stiffener

Distortion is done using an adjustable pre-defined shape positioned on an existing sketch.

Bend stiffener

Distortion is done using an adjustable pre-defined shape positioned on the face of a bend.

3. Set the parameters based on the selected distortion mode. 4. Enter the join radius. It is the radius between the forming and the reference face. 5. Validate the creation of the flange with the button.

The face selected determines the side of the removal, the one which will be "dug". The face selected must be one of the faces which will be deformed. Indeed, the tool shape has to collide with this face and if the tool collides with other faces, these will also be deformed.

Available Options:

Pocket mode: Like for a standard pocket, the parameters are depth, draft angle, base radius and vertical radius. The pocket is created in place at sketch level, the depth is calculated from the position of the sketch in the direction of the face selected. When the plane of the sketch is not parallel with the face selected, the distortion is inclined in relation to the face selected.

Stiffener mode: The parameters of a stiffener are the radius and base width. The stiffener is created in pace at sketch level, the depth is provided by the radius of the stiffener, it depends therefore on the position of the sketch in relation to the face selected.

Bend stiffener mode: The parameters of a stiffener are the radius (inner), depth and angle. It is mandatory that the face selected be a bend face. The stiffener can either be centered in relation to the bend or positioned in relation to one of the edge extremities delimiting the bend by providing an offset distance (the orientation of the edge may be inverted in order to invert the position of the stiffener).

Modifications / Additional information: Unfolding does not take into account the distortion.

Sheet metal recognition Links/Videos:

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This command converts a modeled part with TopSolid or from a file recovery (DWG, Step, Parasolid, etc.) in sheet metal.

Creation stages / Use: Click the icon or select Sheet Metal > Sheet Metal by Recognition... from the dropdown menu. 1. Select a reference face. 2. Select a thickness driver mode: Automatic:

The normal face opposite the nearest reference face determines the value of the sheet thickness. Allows to manually enter the thickness. For example, when recovering a Step, DWG document, etc. or the result of sewing faces gives a thickness of 1.98 mm, you can force the thickness to 2 mm. The topology will not be modified but the achieved sheet will behave like a "real" sheet with a thickness of 2 mm during the unbending and using the bend tables. But the forced value must not be different from the actual sheet thickness.

Forced:

3. Validate the sheet metal creation with the

button.

Available Options: Imposed faces: When automatic face recognition is unsatisfactory, you can indicate the side of a face of the shape manually. T d

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Advanced options: TopSolid verifies permanently the coherence of the faces selected, i.e. TopSolid verifies that all faces of the first side are properly connected to each other and that the faces of the second side are also properly connected together. If this is not the case, the faces detected as "badly identified" are indicated in red and a warning label is positioned over them.

If the shape is a surface or if it was solid and becomes surfacic, the operation will be invalid with this option. Also if the shape has edges with a length smaller than the operation tolerance, the shape will be invalid with this option. The Deactivate the inspections option does not carry out this verification.

You can quickly change the type of face by right-clicking and displaying the popup menu:

Modifications / Additional information: In general, automatic recognition of faces fails when the templates are not correct or when they include singularities, the most common cases are as follows: Opposite non-parallel faces.

Face side Links/Videos:

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This command allows you to modify the side of a face of a sheet at any time.

Creation stages / Use: Click the icon or select Sheet metal > Face side... from the dropdown menu. This command is also available in the Unfolding menu of an Unfolding document. When automatic face recognition is unsatisfactory, you can indicate the side of a face of the shape manually. T d hi l ff h l h f Modifications /hAdditional information:

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When sheet metal is united with another shape, all the faces of the shape are considered as lateral faces, the Change face sides command allows you to identify the faces of the united part. An error message upon opening and/or closing the dialog box if non-lateral faces on the same side are not connected to each other: "Checking process has detected some faces discontinuities."

In general, automatic recognition of faces fails when the templates are not correct or when they include singularities, the most common cases are as follows: Opposite non-parallel faces.

Surface Sheet Metal

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This command allows you to transform a solid sheet metal part into a surface one. Only the selected side of the part will be kept. The surface will keep the sheet metal part properties, it will be possible to apply sheet metal dedicated commands to this surface part.

Creation stages / Use: Click the icon or select the Sheet Metal > Surface Sheet Metal... command from the drop-down menu. 1. Select the side to keep. 2. Validate with .

When you retrieve a part to convert into a sheet metal part (DWG, Step ...), sometimes the side faces and/or the thickness are not well defined. You can use this command to get the best results based on the following scenario: Conversion of the imported part using Sheet Metal recognition. Creation of the Surface sheet metal with a possible redefinition of the thickness. Creation of the Sheet Metal by thickening the surface sheet metal.

Available options: Forced thickness: By default, the Surface Sheet Metal command will use the thickness stored in the Thickness system parameter (this value comes from the Sheet Metal recognition command). This option allows to force the thickness with another value if the default one is not that expected. The Thickness system parameter will be updated with this value. It will be used for Sheet Metal operations calculations and to create Sheet Metal by thickening.

Unbending process Links/Videos:

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This command forces the unfolding method which will be used to calculate the unrolled length of a bend.

Creation stages / Use: Click the icon or select the Unfolding > Unbending process... (from Unfolding document) or Sheet Metal > Unbending process... (from Part document) command from the drop-down menu. 1. Select the internal or external face of a bend. 2. Select on of the 3 proposed unfolding methods: Definition of the unbending method by imposing of Method, factor K and Correction parameters (refer to Unfolding rule for more details). Definition of unbending type (Not specified, Air coining, Coining, Hem bend, Dimpling, Rolling ...). Definition of the tool used (by its description). 3. Validate the unbending process with the button.

In the operations tree, the Unbending processes operations are automatically inserted before the part unfolding operation.

Available Options: Rolling/Breaking: It is possible to define rules for rolling / breaking to use for this unfolding. Limit bending radius: It is the value from which the bend will be rolled or broken. Rolling: Approximation tolerance: It is the rolling approximation accuracy. The 0.1mm is a good value for most Breaking: Number of bending lines: The number of bending lines can be forced. Generally, it is a odd number. Automatic number : By checking this option, the number of bending lines it not taken into account, but automatically calculated regarding the entered spacing. The spacing is define between 2 bend centers. Intermediate bending lines: Allows to add Intermediate bending lines. Alternate Intermediate bending lines: This option is only available if the Intermediate bending lines checked. The internal bending radius of breaking bends can be forced by entering a value or can be equal to th checking this option.

By using the Breaking option: It allows you to quickly force the breaking when flattening a transition shape (hopper), for example.

By using the Rolling option: It also allows you to unroll a tube by force ( cylindrical part is not treated as a be

It is possible to apply Local unbending process in Part document. It must be essentially used to parameterize rules for rolling / braking in the generic document of Family.

If local unbending process is applied on a bend in the Part document and in the Unfolding document, the operation will be invalid in the Unfolding document.

Sheet metal properties

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This command allows to extract informations coming from the unfolding calculation.

Creation stages / Use: Click the icon or select the Tools > Sheet metal properties... command from the drop-down menu. 1. If the sheet metal has been derived, its properties are inherited. By unchecking Derive, the sheet metal properties of this derived sheet metal can be changed. 2. Check Automatic refresh, if each sheet metal modification has to update properties. If not, you have to update manually when needed. 3. If the unfolding calculation fails, extracted values stay at 0 except if the update mode of the operation is defined as Strict. In this case, the operation becomes invalid to warm the user. 4. Each property can be managed using 3 modes: Automatic: TopSolid calculates regarding the geometry modifications. Manual: The user sets the value, which can be very useful for an imported part. Non-managed: For this document, the property is not managed. Different types of properties are: Bends number

Box length (unfolding) = minimal box length Box width (unfolding) = minimal box width Perimeter (unfolding) Cut-outs perimeter (unfolding) Cut-outs number (unfolding) Surface area (unfolding) Surface area without holes (unfolding) 4. Validate by clicking .

These datas are available for the title block and the bill of material information extraction of the part (section Standard > Sheet metal to add bill of material columns). The operation is automatically created since a sheet metal is created. It is possible to define the contents of the operation in a template document.

The automatic refresh can generate loss of performances, each entity modification generate a new calculation of the checked properties. The extraction of these datas needs to calculate the unfolding, this can take time during the update of the analysis operation which is done at each backup. It is recommended to activate it only if needed. During the unfolding calculation, the reference face is defined automatically. However, if the part has no plane face, you have to select the origin face by using the Sheet metal > Unfolding positioning command. If the document contains several sheet metal parts,or a multishape, you have to select the original face.

Unfolding Positioning Links/Videos:

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This command allows you to predefine the positioning of the unfold in the unfolding document.

Creation stages / Use: Click the icon or select Sheet Metal > Unfolding Positioning... from the drop-down menu. 1. Select the reference face of the sheet metal. 2. If necessary, select a point of origin and/or a reference direction. 3. Validate with the button.

The point of origin must absolutely be found on the reference face.

Available Options: Put on / Turned over : This option allows to turn the unfolding result to 180° around the X axis of the destination frame. All bends will be reversed (upward bends become downward bends and vice versa) and also the bend angles signs The Put on mode corresponds to an usual use: The origin face is put on the destination plane of the frame. It gives the bend direction.

The Turned over mode allows to reverse the sheet metal regarding the selected origin face. The bend direction is inverted, otherwise we will obtain a symmetrical sheet metal of the reference sheet metal.

Point of Origin: By default, in the Unfolding document, the center of the selected reference face is positioned on the XY plane of the absolute frame. This option allows you to select a point on the reference face, which will then be positioned on the origin of the Unfolding document's absolute frame.

Orientation: This option allows you to select a direction that will be joined to the X axis of the Unfolding document's absolute frame.

Modifications / Additional information: The definition of a positioning creates an operation that can be modified from the operations tree.

Unfolding rules Links/Videos:

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This command allows to define or select sheet metal unfolding rules. In this case, the preferred radii for the current thickness are automatically proposed during the sheet metal creation and also all the associated unfolding parameters.

Creation stages / Use: Click the

icon or select Sheet Metal > Unfolding Rules... from the drop-down menu.

1. Select an unbending method. 2. Indicate the position of the neutral fiber (K factor) and any additional losses if applicable (correction). 3. Validate the unfolding rules with the button.

Available Options: The Predefined Rules option allows you to use the rules defined in the Unfolding Rules document (bend tables). These Predefined rules can be of two types: Document (selection of a single rule) or Parameter (selection of Unfolding rules parameter or Switch unfolding rules parameter). Parameter allows to drive the rule with a family document or according to a material. By checking Imposed Bend Tool, the bend tool to apply is defined no matter the internal radius defined in the design (in the "standard" case, the bend tool is selected based on the associated bend radius).

You can rapidly define the unfolding rules by selecting an unfolding rules document in the project tree then by moving it to your part document by holding the left mouse button, and releasing the button to make the connection between the two documents. The Analyze sheet metal contextual command summarizes applied unfolding rules on the sheet metal (by taking in account the thickness).

If the Imposed bending tool option is checked, the thickness used to create the sheet metal is not yet known, TopSolid doesn't check if the selected tool is compatible with this thickness. The user must be careful of this. Imposing the bending tool at that time means that you do not have to do it when creating the flattening (you can therefore only make this choice when creating the flattening), which is interesting if you wish, for example, to automatically generate the unfolds via the multiple flattening command.

To force the global bending tool during the unfolding operation, you have to edit the sheet metal inclusion operation and use the unfolding tools section of the dialog. Only available tools for the current thickness are proposed. You can also force locally the tool with the unfolding process command in the unfolding document.

Modifications / Additional information: All sheet shaping processes deform the material. These distortions cause the material to elongate or contract. There are two main modes for calculating losses in bends: Calculations by neutral fiber:

The sheet metal length is considered as constant at the neutral fiber. But the neural fiber position changes along the thickness regarding materials or bend characteristics. Under the neutral fiber, the material is compressed, on the neutral fiber it is stretched. The most elementary method is to provide the neutral fiber to be applied (K factor, position of the neutral fiber) directly, but there are also other methods for calculating this coefficient depending on the material, thickness and bend radius (DIN6935). Another option is also to store these coefficients in tables based on material, thickness, bend radius and bending tool used.

Characteristic lengths in a neutral fiber calculation Loss calculations on draft:

Internal dimension

The length of the unfolded sheet is assimilated to the internal or external face lengths that are extended to eliminate bends. There are three types of calculations: internal, external or tangent dimension. Loss calculation on draft for internal dimension:

External dimension

Tangent dimension (internal or external)

Loss calculation on draft for external dimension:

Loss calculation on draft for external tangent dimension:

K factor: This factor corresponds to the position of the neutral fiber. Correction: Additional losses can also be applied to the results produced by different calculation modes (correction), the values of which can also depend on the material, thickness, bend radius and bending tool used. Therefore, these values are generally stored in tables.

When no value or rule is specified for the unfolding rules and the unbending methods, the default method is that of neutral fiber positioned at 0.5 (K factor 0.5 without correction).

Overview of the assembly commands

The assembly functions enable an assembly to be constructed by including parts, profiles or sub-sets. This component inclusion complies with a positioning. The assembly can also create parts in place, which will "depend" on the surrounding geometry. Parts, sub-sets and library components can be included in an assembly. Each item inserted in the assembly will be positioned by constraints, the objective being to remove the degrees of freedom (1 translation following X, Y, Z and a rotation around X, Y and Z) required for its positing. Until the 6 degrees of freedom have been deleted by the constraints, the part or the sub-set can move. Most of the commands used to define and manipulate an assembly are located in the 'Assembly' menu and will also be very practical to us the content of the 'Constraints' folder in the entities tree, which will contain all relevant information on the constitution of the constraints being defined.

Include part or assembly Frame on frame Axis on plane Repetition

Create part in place Orientation

Show constraints

Auto wizard

Local displacement

Plane on axis

Constraint Point on point Axis on point Filter unpublished contents Automatic process

Plane on plane Point on plane Point on axis

Axis on axis

Inclusion in last positioning

Autofill representations

Plane on point Surface on surface Dynamic positioning

Part

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This command allows to create an in place part but as if it has been included, it means without synchronization like by using the in place part.

Creation stages / Use: Click the icon or select the Assembly > Part... command from the dropdown menu. 1. Select the XY plane as support of the part to create. 2. Select the origin point of this plane. 3. Select the X or Y direction of this plane. These 3 selections allow to create the inclusion frame.

The created part isn't synchronized with the assembly. It is an included part, but in place created. its positioning can be edited if it is not fixed.

Available options: Inclusion at origin: If this option is checked, the part is included on the origin of the assembly.

Fix:

If this option is checked, the created part is fixed. Otherwise, it will be non constrained.

If the part is unfixed, its positioning can be edited to add constraints.

Rigid group: If a mechanism exists, this part can be included in one of the listed rigid groups.

Same folder: If this option is checked, the part is created in the same folder than the assembly. If it is unchecked, its destination folder will be asked.

Once the in place part has been created, it must be validated by clicking the In Place Editing button situated in the center at the top of the graphic display.

Modifications / Additional information: In the project tree, the created part isn't linked to the assembly. It is at the same level or in another folder.

Assembly

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This command allows to create an in place assembly but as if it has been included, it means without synchronization like by using the in place assembly.

Creation stages / Use: Click the icon or select the Assembly > Assembly... command from the drop-down menu. 1. Select the XY plane as support of the assembly to create. 2. Select the origin point of this plane. 3. Select the X or Y direction of this plane. These 3 selections allow to create the inclusion frame.

The created assembly isn't synchronized with the assembly. It is an included assembly, but in place created. its positioning can be edited if it is not fixed.

Available options: Inclusion at origin: If this option is checked, the created assembly is included on the origin of the assembly.

Fix:

If this option is checked, the created assembly is fixed. Otherwise, it will be non constrained.

If the assembly is unfixed, its positioning can be edited to add constrain

Rigid group: If a mechanism exists, this assembly can be included in one of the listed rigid groups.

Same folder: If this option is checked, the assembly is created in the same folder than the assembly. If it is unchecked, its destination folder will be asked.

Once the in place assembly has been created, it must be validated by clicking the In Place Editing button situated in the center at the top of the graphic display.

Modifications / Additional information: In the project tree, the created assembly isn't linked to the main assembly. It is at the same level or in another folder.

Inclusion

This command allows you to include a part, a sub-set, a local part or assembly of an assembly into the current assembly document. The assembly is the mechanism which allows you to construct an assembly by including parts, profiles or sub-sets. This component inclusion complies with a positioning.

Creation stages / Use: Click the icon or select Assembly > Inclusion... (from an Assembly document) or select Shape > Inclusion... (from a Part document). The parts and open sub-sets are proposed in the Documents drop down list. 1. 2. 3. 4.

Enter the occurrence name to include, if needed. Select the part or a sub-set to include. Select a code if defined. In the Destination section of the dialog, select the rigid group in which the part or assembly will be included (if a mechanism exists). 5. Position your part or sub-assembly. By checking Inclusion at origin, the included document will be positioned on the absolute frame.

If the above and below options are not required, the part or assembly may be dropped directly from its icon in the tree to the assembly. The first included part or assembly will automatically be fixed (validation of the positioning is not requested), the absolute frame of the part being placed on the absolute frame of the assembly in which it is included. (The Constraint is automatically activated). If a part has several representations and if the current representation is Design, by including this part in an assembly, the detailed representation will be used if the assembly has detailed as current representation. if not, the simplified representation will be used.

From a Part document, this command does not allow to manage bi-materials part (if the included part have not the same material). The material information of the included part is ignored. This command allows to reuse shapes to modeling a part.

Available Options: Mechanism: (Only available for inclusion of assemblies with mechanism). Rigid inclusion: When including an assembly with a mechanism and some configurations, it can be included rigid or not. If Rigid inclusion is checked, the configuration to use can be chosen, but it will be rigid. Use configuration: When several configurations exist in the mechanism, it is possible to select one of them. It will be articulated if it is in the mechanism. Add position constraint: When the Use configuration option is checked, it is possible to automatically create a position constraint during the assembly inclusion.

Inherit: If including an assembly with a mechanism, its rigid groups, forces and/or joints can be inherited.

If the mechanism is included as rigid, it is possible to articulate it by using the Articulate contextual command. When it is included articulate, the equivalent contextual command is Make rigid.

Drivers: (Only available for inclusion of families with drivers). The different available drivers are displayed. Their values can be changed before validating this command. During the inclusion of a family document with a shell block, the Create positioning option allows you to include the family document by giving the shell block dimensions. This option is not available during the edition of a family document with a shell block driver.

Local Part or Assembly: This area is displayed when the assembly contains a local part or assembly only (see the Local Part... and Local Assembly... commands for more details). The button which displays the name of the document or allows you to access to a dialog box which displays the local parts or assemblies of the document to include in order to choose one of them.

Advanced Options: Drivers consistency control: (Only available for inclusion of families with drivers). If a family with drivers is included in an assembly and then a new driver is created in this family: If the Strict option is not checked, the value of this driver in the generic will be used. If the Strict option is checked, the inclusion will become invalid and will indicate that the driver has no value. Sub Components button: This button allows to access to the substitution dialog box to force the family, the code and/or the drivers of a subcomponent.

Substituable in upper level: If this options is activated, this sub-component can be substituted in upper assembly levels by changing its family, its code or drivers.

Sub Components: This button allows to access to the substitution dialog box to force the family, the code and/or the drivers of a subcomponent.

Constraint

This command automatically constrains the parts to be included according to the selected geometries.

Creation stages / Use: Select the Assembly > Constraint... command from the drop-down menu. 1. Select the original geometry. 2. Select the destination geometry. This command will restrict the parts using these constraints: Plane on plane, Axis on axis, Point on point, Frame on frame, Plane on axis, Axis on plane, Axis on point, Point on axis, Point on plane, Plane on point, Orientation and Surface on surface. Sometimes it is necessary to use the rotary picking to select the appropriate geometry. Some of these constraints can be offset by double-clicking on the label value.

The objective of these constraints is to position the part in the assembly by deleting the 6 degrees of freedom. If the part is not fully constrained, it can be moved with the mouse. Each part has its positioning. The positioning of the next part is a function of the previous part, which means that by moving the first part, the second will not move dynamically, but will wait until the first part is in its destination position before being calculated and positioned in order to have very short calculation times. With these conditions, it is impossible to position 3 parts together if the third is positioned on the first 2 without grouping the positionings. There are 2 methods: Either turn on the Include in Last Positioning mode before doing the positioning, or if this is already done, merge them by selecting them from the operations tree.

Available Options: The buttons displayed on the right of the source and destination fields allows you to create middle point, plane or axis on the fly (without stopping the command). The created element will be automatically used to fill the Source or Destination field.

Modifications / Additional information: To edit the positioning of the part, double-click part in the assembly. The labels display and can be modified. You can also use the Edit Positioning popup menu.

Plane on plane

This command constrains a plane of the part to be included in relation to a plane of the destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Plane on plane... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Plane on plane... command from the drop-down menu. 1. Select a plane on the geometry to be included. 2. Select a plane on the destination geometry. 3. Enter the offset. The positioning on Plane on plane, can either be: a contact (the geometries oppose each other in relation to the planes selected). or an alignment (the geometries are on the same side in relation to the planes selected). or an orientation (the geometries have an angle between each other). An offset can be entered between the 2 planes.

it is possible to create a mid plane "on the fly" by clicking the "+" in the corresponding field.

Available Options: Reverse: Allows to reverse the offset size. This option is also available by clicking the label arrow.

Modifications / Additional information: The modification can be carried out either via the popup menu with the Edit a plane on plane command or by clicking on the labels.

The double-click: On both planes, changes the direction of a plane (contact / alignment). On the name, renames the constraint. On the arrow, reverses the direction of the offset. On the value, changes the value of the offset.

Plane on axis

This command allows you to constrain a plane of the part to be included in relation to an axis of the destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Plane on axis ... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Plane on axis... command from the drop-down menu. 1. Select a plane on the geometry to be included. 2. Select an axis on the destination geometry. 3. Enter the offset.

It is possible to create a mid axis and a mid plane "on the fly" by clicking the "+" in the corresponding field.

Available Options: Reverse: Allows to reverse the offset side.. This option is also available by clicking the label arrow.

Modifications / Additional information:

The modification can be carried out either via the popup menu with the Edit Plane on axis command, or by clicking on the labels.

The double-click: On the name, renames the constraint. On the arrow, reverses the direction of the offset. On the value, changes the value of the offset. Axes, edges, arcs, circles and cylindrical faces can be selected.

Plane on point

This command constrains a plane of the part to be included in relation to a point of the destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Plane on point... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Plane on point... command from the drop-down menu. 1. Select a plane on the geometry to be included. 2. Select a point on the destination geometry. 3. Enter the offset.

It is possible to create a mid point and a mid plane "on the fly" by clicking the "+" in the corresponding field.

Available Options: Reverse: Allows to reverse the offset side. This option is also available by clicking the label arrow.

Modifications / Additional information:

The modification can be carried out wither via the popup menu with the Edit Plane on point command, or by clicking on the labels.

The double-click: On the name, renames the constraint. On the arrow, reverses the direction of the offset. On the value, changes the value of the offset.

Axis on plane

This command allows you to constraint an axis of the part to include regarding a plane of the destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Axis on plane... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Axis on plane.. command from the drop-down menu. 1. Select an axis on the geometry to be included. 2. Select a plane on the destination geometry. 3. Enter the offset.

It is possible to create an mid axis and a mid plane "on the fly" by clicking on "+" in the corresponding field.

Available Options: Reverse: Allows to reverse the offset side. This option is also available by clicking the label arrow.

Modifications / Additional information:

The modification can be carried out either via the popup menu with the Edit Axis on plane command, or by clicking on the labels.

The double-click: On the name, renames the constraint. On the arrow, reverses the direction of the offset. On the value, changes the value of the offset. Axes, edges, arcs, circles and cylindrical faces can be selected.

Axis on axis This command constrains an axis of the part to be included in relation to an axis of the destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Axis on axis... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Axis on axis... command from the drop-down menu. 1. Select an axis of the geometry to be included. 2. Select an axis of the destination geometry. 3. Enter the distance.

The Axis on axis positioning can be reversed. It is possible to create an mid axis "on the fly" by clicking on "+".

Available Options: Parallel: When this option is cleared, you can only create a contact point between the two selected axes.

Modifications / Additional information:

The modification can either be carried out via the popup menu with the Edit axis on axis command or by clicking on the labels.

The double-click: On the icon, reverses the constraint. On the name, renames the constraint. Axes, edges, arcs, circles and cylindrical faces can be selected.

Axis on point

This command constrains an axis of the part to be included in relation to a point of the destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Axis on point... command from the drop-down menu. It is also possible to add constraints to a configuration of a mechanism. In this case, select the Mechanism > Axis on point... command from the drop-down menu. 1. Select an axis of the geometry to be included. 2. Select a point of the destination geometry. 3. Enter the distance.

It is possible to create an mid axis and a mid point "on the fly" by clicking on "+" in the corresponding field.

Modifications / Additional information: The modification can be carried out either via the popup menu with the Edit axis on point command or by clicking on the labels. Double-clicking on the label renames the constraint. Axes, edges, arcs, circles and cylindrical faces can be selected.

Point on plane

This command constrains a point of the part to be included in relation to a plane of the destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Point on plane... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Point on plane... command from the drop-down menu. 1. Select a point on the geometry to be included. 2. Select a plane on the destination geometry. 3. Enter the offset.

It is possible to create a mid point and a mid plane "on the fly" by clicking the "+" in the corresponding field.

Available Options: Reverse: Allows to reverse the offset side. This option is also available by clicking the label arrow.

Modifications / Additional information:

The modification can be carried out either via the popup menu with the Edit Point on plane command or by clicking on the labels.

The double-click: On the name, renames the constraint. On the arrow, reverses the direction of the offset. On the value, changes the value of the offset.

Point on axis

This command constrains a point of the part to be included in relation to an axis of the destination geometry.

Creation stages / Use: Click the icon or select Assembly > Point on Axis... from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Point on axis... command the drop-down menu. 1. Select a point on the geometry to be included. 2. Select an axis on the destination geometry. 3. Enter the distance.

It is possible to create a mid point "on the fly" by clicking the "+".

Modifications / Additional information: The modification can be carried out either via the popup menu with the Edit Point on axis command or by clicking on the labels. Double-clicking the positioning label changes the name of the constraint.

Point on Point

This command constrains a point of the part to be included in relation to a point of the destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Point on point... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Point on point... from the drop-down menu. 1. Select a point on the geometry to be included. 2. Select a point on the destination geometry. 3. Enter the distance.

It is possible to create a mid point "on the fly" by clicking the "+".

Modifications / Additional information: The modification can be carried out either via the popup menu with the Edit Point on point command or by clicking on the labels. The double-click changes the name of the constraint.

Orientation

This command orients the part to be included in relation to a destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Orientation... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Orientation... command from the drop-down menu. 1. Select a direction on the geometry to be included. 2. Select a direction on the destination geometry. 3. Enter the angle.

Available options: Normal: You can activate this option in order to define a third direction. This direction is used define the plane in which the angular value is applied. It is possible to select this direction a the part to position (Source) or in the assembly environment (Destination)

Modifications / Additional information: The modification can be carried out either by the popup menu with the Edit orientation command or by clicking on the labels.

The double-click: On the name, renames the constraint. On the two arrows, reverses the orientation direction. On the value, changes the value of the angle.

The orientation constraint is not signed (spatial angle). Due to this fact, the constraint can become invalid by entering the angle. In this case, you just have to move the part with the mouse in one direction or the other.

Frame on Frame

This command constrains a frame of the part to be included with a frame of the destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Frame on frame ... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Frame on frame... command from the drop-down menu. 1. Select a frame in the geometry to be included. 2. Select a frame on the destination geometry. 3. Enter the offset. 4. Possibility to enter a rotation angle around each axes if necessary.

Available Options: Reverse: Allows to reverse the offset side and/or rotation angle. The offset option is also available by clicking the label arrow. Rotate around Z then Y then X: Allows to change the solving order of rotation angles.

During positioning of Frame on frame, the X, Y and Z axes of both frames will be pointing in the same direction. An offset can be entered between the 2 frames. It is possible to turn a frame around another by entering an angle.

Modifications / Additional information: The modification can be done by with the Edit frame on frame contextual command or by clicking the labels.

The double-click: On the name, renames the constraint. On the arrow, reverses the direction of the offset. On the value, changes the value of the offset.

Surface on Surface

This command constrains a surface of the part to be included in relation to a surface of the destination geometry.

Creation stages / Use: Click the icon or select the Assembly > Other constraints > Surface on surface... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Surface on surface... command from the drop-down menu. 1. Select a surface on the geometry to be included. 2. Select a surface on the destination geometry. 3. Enter the offset. The Surface on surface positioning can either be: a contact (the geometries oppose each other in relation to the surfaces selected). an alignment (the geometries are on the same side in relation to the surfaces selected). An offset can be entered between the 2 surfaces.

Surfaces are always consider as unlimited.

Summary of the different supported cases for the Surface on surface constraint. Surface / surface Plane Cylinder Cone Sphere Torus

Plane

Cylinder

Cone

Sphere

Torus (1)

(2) (1)

(1) A torus is only constrained if it is positioned with a surface which is a plane. The contact or the alignment torus with this plane is punctual. (2) When 2 cones are selected, some limitations exist: If a full cone is constrained with a hollow cone, its angle must be smaller or equal to the hollow co angle. Also in this case, the vertex of each cone (even if they are truncated) are coincident. The contact or the alignment between two cones is always linear. (The axis is projected on the sur is this projected line which is in contact with the equivalent line of the other cone). When the conicities are different, you have to use the profile on plane constraint. Depending on the surface orientation, you will get a cone on cone or a cone in cone positioning:

Face selection (case #1)

Face selection (case #2)

Result

Cone on cone positioning

Cone in cone positioning

Available Options: Reverse: Allows to reverse the offset side. This option is also available by clicking the label arrow.

Modifications / Additional information: The modification can be carried out either via the popup menu with the Edit surface on surface command or by clicking on the labels.

The double-click: On the 2 surfaces, change the direction of a surface (contact / alignment). On the name, renames the constraint. On the arrow, reverses the direction of the offset. On the value, changes the value of the offset.

Direction on Frame Links/Videos:

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This command allows you to constrain a direction on the part to include with an existing frame in the assembly. Contrary to the orientation constraint, which is a spatial orientation, this constraint allows an orientation with respect to the YZ plane of the chosen frame.

Creation stages / Use: Click the icon or select Assembly > Other Constraints > Direction on Frame... or Mechanism > Other Constraints > Direction on Frame... from the drop-down menu. It is also possible to add constraints to a configuration of a mechanism. In this case, select the Mechanism > other constraints > Direction on frame... command from the drop-down menu. 1. Select a direction on the geometry to be included. 2. Select a frame on the destination geometry. 3. Enter the angle. When positioning the Direction on Frame, the direction will be parallel to the X axis of the frame. The angle entered will be between the direction and the X axis of the selected frame.

Modifications / Additional information:

The modification can be done by with the Edit Direction on frame contextual command or by clicking the labels.

The double-click: On the symbol, reverses the orientation. On the name, renames the constraint. On the value, changes the value of the angle.

Frame on direction Links/Videos:

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This command allows you to constrain a frame of the part to include with a direction in the assembly. Contrary to the orientation constraint, which is a spatial orientation, this constraint allows an orientation with respect to the YZ plane of the chosen frame.

Creation stages / Use: Click the icon or select the Assembly > Other constraints > frame on direction... command from the drop-down menu. It is also possible to add constraints to a configuration of a mechanism. In this case, select the Mechanism > Other constraints > frame on direction... command from the drop-down menu. 1. Select a frame published in the geometry to include. 2. Select a direction in the assembly. 3. Enter the angle. When positioning the Frame on Direction, the direction will be parallel to the X axis of the frame. The angle entered will be between the X axis of the part frame and the direction.

Modifications / Additional information: The modification can be done by with the Edit frame on direction contextual command or by clicking the labels.

The double-click: On the symbol, reverses the orientation. On the name, renames the constraint. On the value, changes the value of the angle.

Profile on point

This command constrains a profile of the part to be included in relation to a point of the destination geometry.

Creation stages / Use: Click the icon or select Assembly > Other constraints > Profile on point... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Profile on point... command from the drop-down menu. 1. Select a profile on the geometry to include. 2. Select a point on the destination geometry.

It is possible to create a profile on edge, on boundary edge or a mid point "on the fly"by clicking the corresponding button.

Modifications / Additional information: The modification can be carried out either via the popup menu with the Edit Point on point command or by clicking on the labels. Double-clicking the positioning label changes the name of the constraint.

Plane on profile

This command allows you to constraint a plane of the part to include regarding a profile of the destination geometry.

Creation stages / Use: Click the icon or select Assembly > Other constraints > Point on profile... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Point on profile... command from the drop-down menu. 1. Select a point on the geometry to be included. 2. Select a profile on the destination geometry.

It is possible to create a profile on edge, on boundary edge or a mid point "on the fly"by clicking the corresponding button.

Modifications / Additional information: The modification can be carried out either via the popup menu with the Edit Plane on profile command or by clicking on the labels. Double-clicking the positioning label changes the name of the constraint.

Profile on plane

This command constrains a profile of the part to be included in relation to a plane of the destination geometry.

Creation stages / Use: Click the icon or select Assembly > Other Constraints > Profile on Plane... from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Profile on plane... command from the drop-down menu. 1. Select a profile on the geometry to be included. To view the profile, it must be published. 2. Select a plane on the destination geometry. 3. Enter the offset.

It is possible to create a profile on edge, on boundary edge or a mid plane "on the fly"by clicking the corresponding button.

Available Options: Reverse: Allows to reverse the offset side. This option is also available by clicking the label arrow.

Modifications / Additional information: The modification can be carried out either by the popup menu with the Edit Profile on plane command or by clicking on the labels. The double-click: On the name, renames the constraint. On the icon, reverses the direction of the offset. On the value, changes the value of the offset.

Plane on profile Links/Videos:

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This command constrains a plane of the part to be included in relation to a profile of the destination geometry.

Creation stages / Use: Click the icon or select Assembly > Other Constraints > Plane on Profile... from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Plane on profile... command from the drop-down menu. 1. Select a plane on the geometry to be included. 2. Select a profile on the destination geometry. To view the profile, it must be published. 3. Enter the offset.

It is possible to create a profile on edge, on boundary edge or a mid plane "on the fly"by clicking the corresponding button.

Available Options: Reverse:

Allows to reverse the offset side. This option is also available by clicking the label arrow.

Modifications / Additional information: Modifications can be done via the popup menu with the Edit Plane on Profile command, or by clicking on the labels. The double-click: On the name, renames the constraint. On the icon, reverses the direction of the offset. On the value, changes the value of the offset.

Point on shape Links/Videos:

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This command constrains a point of the part to be included with a frame of the destination geometry.

Creation stages / Use: Click the icon or select Assembly > Other Constraints > Point on Shape... from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Point on shape... command from the drop-down menu. 1. Select a point on the geometry to be included. 2. Select a destination shape. 3. Enter the offset.

It is possible to create a mid point "on the fly" by picking the "+".

Available Options: Reverse: Allows to reverse the offset side. This option is also available by clicking the label arrow.

Modifications / Additional information: Modifications can be done via the popup menu with the Edit Point on Shape command or by clicking on the labels.

The double-click: On the name, renames the constraint. On the value, changes the value of the offset.

Shape on Point

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This command constrains the shape be included in relation to a point of the destination geometry.

Creation stages / Use: Click the icon or select Assembly > Other Constraints > Shape on Point... from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Shape on point... command from the drop-down menu. 1. Select the shape to include. 2. Select a point on the destination geometry. 3. Enter the offset.

It is possible to create a mid point "on the fly" by clicking the "+".

Available Options: Reverse: Allows to reverse the offset side. This option is also available by clicking the label arrow.

Modifications / Additional information: Modifications can be done via the popup menu with the Edit Shape on Point command or by clicking on the labels.

The double-click: On the name, renames the constraint. On the value, changes the value of the offset.

Shape to normal Links/Videos:

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This command allows you to create a constraint so that a part is normal to another.

Creation stages / Use: Click the icon or select the command Assembly > Other constraints > Shape to normal... from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, you should choose the command Mechanism > Other constraints > Shape to normal... from the drop down menu. 1. Select the source shape (the blue shape on the example bellow). 2. Select the destination axis (the orange shape) 3. Validate by clicking .

Example: the blue part is included into the assembly and must be positioned normal to the orange part

It is possible to create a mid axis "on the fly" by clicking the "+".

Modifications / Additional information: Modifications can be done through the popup menu with the Edit Shape to normal command or by clicking on the labels. The double-click: On the name, renames the constraint. On the arrow, reverses the axis direction.

Normal to shape Links/Videos:

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This command allows you to create a constraint so that a part is normal to another.

Creation stages / Use: Click the icon or select the Assembly > Other constraints > Normal to shape... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Normal to shape... command from the drop-down menu. 1. Select the axis from the source part (the orange part in the example above). 2. Select the destination shape (the blue part) 3. Validate by clicking .

Example: the orange part included in the assembly which contains the blue part and this orange part has to be normal to the blue one.

It is possible to create a mid axis "on the fly" by clicking the "+" in the field.

Modifications / Additional information: The modification can be done via the popup menu with the Edit normal to shape command, or by clicking on the label.

The double-click: On the name, renames the constraint. On the arrow, reverses the axis direction.

Joint driving

This command allows you to enter a joint driving value for a subcomponent. For example, if a jack with a prismatic joint with limits, and for which a configuration has been created, can be inserted in an assembly and an exit value may be imposed with this function.

Creation stages / Use: 1. Select the sub-set for which the joint will be driven and edit the positioning with the popup menu. 2. Click the icon or select the Assembly > Other constraints > Joint driving... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Joint driving... command from the drop-down menu. 3. Select the joint to be driven in the drop down list. 4. Enter the value or check minimum limit or maximum limit to have this value of this driven joint. 5. Validate. 6. Validate the positioning.

Limits defined in the joint are taken in account. For example, if the output shaft of the jack is limited to 250mm,the joint driving will not be possible above this value. In this case, it is possible to click the maximum limit option.

Configuration position Links / Videos :

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This command allows to fix the relative position of several (or all) rigid groups of an articulated sub-assembly so it will be the same than the one defined in one of its configurations. For example, a robot can be included with articulation, but can be imposed to its " configuration" position in the assembly.

Creation stages / Use: Select the Assembly > Other constraints > Configuration Position... command from the drop-down menu. 1. Select in the drop-down list, one of the assembly occurences to position. 2. Select the mechanism configuration to use. 3. Select All rigid groups to apply this constraint to all rigid groups of the included assembly or select rigid groups to constrain. 4. Validate.

This constraint can also be automatically created during the inclusion of an assembly with a mechanism by checking the Add position constraint option.

Modifications / Additional information:

The modification, the 'activation/deactivation, the deletion and the renaming can be done from the contextual on the label during the positioning edition or from the Constraints folder of the entities tree.

Stacking Links / Videos :

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This command allows to constrain parts with a "stacking" process.

Creation stages / Use: All the parts managed by this constraint have to be inserted in the same positioning.

Click the icon or select the Assembly > Other constraints > Stacking... command from the drop-down menu. 1. Select a part that contains a Stackable component provided function. 2. Add at least another part that also contains a Stackable component provided function. 3. TopSolid "stacks" the parts, bottom frame on top frame, according the stack order.

The order is modificable with the 2 side arrows you can add a new part in the current stack with

. .

An offset can be set between 2 parts.

To set correctly the offset, select the "top" part in the stack.

An angle can be set to manage a rotation between the 2 stacked parts:

Available Options: Reverse: Allows to invert the offset direction.

Modifications / Additional information: The modification can be carried out either via the popup menu with the Stacking edit command, or by bright-click on the label :

The double-click: On the name, renames the constraint.

Neighboring Assembly

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This command allows you, when editing a part in place, to transparently see the neighboring parts that can be pressed.

Creation stages / Use: Select Assembly > Assembly Neighborhood... from the dropdown menu. The command is also available from the popup menu of a part. 1. Select the part on which to define a neighborhood. 2. Select the parts of the neighborhood. 3. Validate by clicking .

Note that the creation of a neighborhood synchronizes the part that receives the neighborhood and assembly, therefore creating neighborhoods when it is not really necessary must be avoided in order to limit the global complexity.

Options: Hide: The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Example of use: In an assembly done by ascent, part "A" should be modified associatively depending on the relative position of part "B" in this assembly. That is, if part "B" changes, or if the relative position of "B" in relation to "A" in the assembly changes, "A" should be updated automatically to take into account the modifications, without having to perform manual modifications on "A". In this case, part "B" must be defined in the neighborhood of part "A".

Assembly Context

Using an assembly neighborhood will synchronize the part and assembly, which will guarantee the instant recognition of modifications of one on the other and vice versa. However, this may be inconvenient when performing group work on the same assembly. In fact, upon the first modification, the assembly and all parts containing a defined neighborhood are locked for exclusive use by the user that triggers it, so that no one else can work on these parts. In order to allow collaborative work on the same assembly, it is possible in location and in place of the assembly neighborhood to define an assembly context, in the same way as for the neighborhood. The assembly context does not synchronize the part and assembly, so work can be done on the part without locking the assembly. However, the update is not automatic, so it must be done manually.

Creation stages / Use: Click the icon or select Assembly > Assembly Context... from the drop-down menu. 1. Select the part for which the context will be included. 2. Select the different entities of the context.

The entities of the assembly context appear transparent, when the part document is open.

Entities of the assembly context can be deleted form the Contexts folder in the part's entities tree. The context can be refreshed manually, when one of the entities of the context or the reference assembly changes, by using the popup menu in the work area. A same part can have several contexts of several or the same assembly (in the Contexts folder in the entities tree).

Options: Hide: The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Additional information: The different defined assembly contexts are listed in the Contexts folder of the entity tree.

In entities tree: An up-to-date context is indicated with this

icon.

A context not updated is displayed with this different: icon

To update a context, use the Update command from the popup menu.

Removing Links/Videos:

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This command allows you to delete one or more parts in an assembly document by keeping its inclusion. For example, a part P1 is included in an assembly, manually or by a wizard. Several other parts are constraints regarding this part. By deleting P1 with this command, other parts keep their positioning But it is not possible to constraint new included parts with P1. P1 does not appear in the assembly draft neither in the BOM. A using case could be the deletion of a part in the derived to be able to replace it by another.

Creation stages / Use: Click the icon or select Assembly > Removing... from the dropdown menu. 1. Select parts or sub-assemblies to delete. 2. Validate

You cannot delete parts belonging to a subassembly. It is the all of this that is selected and therefore deleted. When a part is deleted, it is grayed in parts folder of entities tree. Parts included after this deletion , can not be constrained with this part. The part is not physically deleted. It is deleted in the representation and is not displayed in the draft neither in the BOM.

Type for BOM

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This command allows you to select the level of detail of the assembly for the BOM.

Creation stages / Use: Select Construction > Parameters > Type for BOM... from the drop-down menu. You can choose between 4 modes: Absent: The document will not be displayed in the BOM. This mode can be useful to include a document in an assembly without taking it into account in the BOM. For example, if you design a factory layout, you want to include human mannequins but you don't want to get them in the BOM. Composite: All the items of the assembly can be listed in the BOM. In Multilevel mode, a line will be added for the set. Simple: The BOM will only display information of the assembly even for a flat BOM. The constituents of this assembly will not be detailed. Transparent: This mode is the same as the Composite mode. In the case of a multilevel BOM, the line with respect to the set will not be added.

This command is available in an assembly document only.

Dynamic positioning

This mode activates or deactivates the dynamic positioning of the parts.

Use: Click the

icon in the Assembly or Mechanism tab icon bar.

When this mode is activated, the part to be constrained "sticks" to the mouse and the positioning is proposed, near the destination part. When this mode is deactivated, the part to be constrained remains in its starting position until the constraint is validated.

To improve the response time when inserting parts in the assemblies including many constraints, it may be wise to deactivate this mode.

Additional information: This mode is enabled when the icon is pressed down. (background stays in color). This mode applies to all documents in the TopSolid session.

Show constraints

This mode activates or deactivates the viewing of positioning constraints by double-clicking on the parts.

Use: Click the

icon in the Assembly or Mechanism tab icon bar.

When this mode is activated, the constraints can be viewed by double-clicking on the parts. When this mode is deactivated, the constraints are not visible by double-clicking on the parts.

To improve the response time when inserting parts in the assemblies including many constraints, it may be wise to deactivate this mode.

Additional information: This mode is enabled when the icon is pressed (the background remains colored). This mode applies to all documents of the TopSolid session.

Automatic wizard

This mode activates or deactivates the automatic wizard for parts during insertion.

Use: Click the icon or select the Assembly > Modes > Automatic wizard... command from the drop-down menu. When this mode is activated, the wizard created in the wizard document is proposed to assemble the part. When this mode is deactivated, the wizard created in the wizard document is not proposed and the part will be positioned without wizard.

Additional information: This mode is enabled when the icon is pressed (the background remains colored). This mode applies to all documents of the TopSolid session.

Automatic destination wizard Links/Videos:

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This mode allows to propose destination wizards when they exist like for example when including a part in a vice. This mode is usually used by TopSolid'Cam. (see the Destination option of the include command).

Creation stages / Use: Click the icon in modes of the assembly icons bar or select the Assembly > Modes > Automatic destination wizard... command from the drop-down menu. When this mode is activated, the destination wizard created in the wizard document is proposed to assemble the part. When this mode is deactivated, the destination wizard created in the wizard document is not proposed and the part will be positioned without wizard.

Additional information: This mode is enabled when the icon is pressed (the background remains colored). This mode applies to all documents of the TopSolid session.

Automatic process

This mode activates or deactivates the automatic processes of parts during insertion.

Use: Click the icon in the Assembly tab icon bar or select the Assembly > Modes > Automatic process... command from the drop-down menu.. When this mode is activated, the process is proposed when the part is included in the assembly. When this mode is deactivated, the process is not proposed. The process could be added manually using the Use process command.

Additional information: This mode is enabled when the icon is pressed (the background remains colored). This mode applies to all documents in the TopSolid session.

Inclusion in last positioning

This mode activates or deactivates the inclusion of the part in the last positioning.

Use: Click the icon in the Assembly tabs or select the Assembly > Modes > Inclusion in last positioning... command from the dropdown menu.. When this mode is activated, the constraints of the new parts inserted are added to the last positioning. The constraints are calculated at the same time, enabling positioning of parts requiring the displacement of other parts during assembly (constraint system). For example, the assembly of a jack between the chassis and the mobile portion, requires this part to move during the creation of the constraint. When this mode is deactivated, the constraints of the new inserted parts are added to a new positioning. When the parts are moved with the mouse, the parts move one after another, the position of the first part must be known to be able to position the following part.

The deactivated mode gives better performances when the parts are moved with the mouse.

Additional information:

This mode is enabled when the icon is pressed (the background remains colored). This mode applies to all documents of the TopSolid session.

Local displacement

This mode activates or deactivates the local displacement of parts.

Use: Click the icon in the Assembly or Mechanism tab icon bar or select the Assembly > Modes > Local displacement... command from the drop-down menu.. When this mode is activated, only the selected part moves when the mouse is displaced. When this mode is deactivated, all joined parts move at the same time as the mouse is displaced.

Additional information: This mode is enabled when the icon is pressed (the background remains colored). This mode applies to all documents of the TopSolid session.

Workspace

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This command allows to create areas in a Workspaces manager document in order to decompose a project into several documents (workspaces). These documents could be managed by different users to include parts or assemblies in it. An Assemble workspaces command will allow to create a new Assembly document with the content of the representations of the selected workspaces as well as the contexts

Creation stages / Use: Select the Workspace > Workspace... command from the dropdown menu of a Workspaces manager document type. 1. 2. 3. 4. 5. 6.

Give a name to the workspace to create. Enter the author. Select contexts to use. Select part or assembly occurrences to add into the workspace. Select the limitation volume. Validate.

The inclusion of assembly to decompose can be done with standard commands (Assembly > Inclusion or with drag-anddrop). Validate the command will create two new documents: A Workspace background document with selected contexts and occurrences. This document type cannot be modified and can be created by the Workspace command only. It is use as background document in the workspace document. An assembly corresponding to the workspace document. It is inside this document that user will work including new parts or assemblies (relying on background describe above). These documents do not reference the current document (management document). There are not updated automatically if it is modified (see at the end of this page). Export one of these documents will not export neither the management document or the initial assembly (assembly include in the management document).

Available options: Origin frame: You can select an origin frame that could help your construction in the workspace. This frame will be available in the workspace even if it is outside the limitation volume.

Background document location: By default the background document of the workspace document is created in the same folder as the workspaces management document.

This option allows to specify another folder. This modification is available creating the workspace, this field will be grayed out editing the workspace.

Workspace document location: By default the workspace document is created in the same folder as the workspaces management document. This option allows to specify another folder. This modification is available creating the workspace, this field will be grayed out editing the workspace.

Modifications / Additional information: Author: The Author field lists the users declared in the PDM. This field is editable allowing to manually enter a user that does not exist in the PDM. Created documents will have the Author property filled with this value. But these new documents will be visible for the current user only until they have been checked-in.

Contexts definition: Definition of workspaces contexts must be done from the entities tree, contextual menu on the system sub-set Sets > Workspaces Contexts... then select the Set command. A part or assembly can be use in several contexts (except if the user made these sets Exclusive). Contexts can also contain sketches, points, frames...

Limitation volume: Limitation volume definition is done with shapes commands, from the Shape tab. Background document will contain all context elements and occurrences that are inside the volume. Elements intersected by the volume will be trimmed.

Modification and updating of workspaces: It is possible to edit an existing workspace in order to add/delete contexts and/or occurrences. Validating the modified workspace, modifications have been saved but not done. The workspace needs to be updated. Operation icon, Entity icon and Workspaces folder icon have been changed. The Update Workspaces command is available in contextual menu (it updates the background document).

Assemble workspaces

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This command allows to create the final assembly with the content of the selected workspaces representation as well as contexts.

Creation stages / Use: Select the Workspace > Assemble workspaces... command from the drop-down menu of a Workspaces manager document type. 1. 2. 3. 4.

Enter the name to give to the final assembly. Select contexts to consider in the final assembly. Select workspaces. Validate.

It is possible to select contexts that have not been used to define workspaces. It is possible to assemble several workspaces. Validate this command will create assembly documents: One assembly document per selected context (containing parts/assemblies of each context). The final assembly with the workspace assemblies and context assemblies.

Available options: Update final assembly: This option allows to select an existing final assembly to modify its content in order to add/remove contexts and/or workspaces. The final assembly must be opened to be available in this menu.

Modifications / Additional information: As explained above the validation of this command will create, among other things, one Assembly document by selected context. The content of these assemblies is maintained by Workspace context assembly operations in the management document. These operations are not editable. They are updated automatically and maintain the content of context assemblies. These operations can be deleted but it will not delete context assemblies documents. Right click on these operations gives access to the Open Document command that allows to open the context assembly from the management document.

In Place Part

This command creates a part directly in the assembly by using the geometries of the surrounding parts.

Creation stages / Use: Click the menu.

icon or select Modeling > In place part... command from the drop-down

1. Select a part template. 2. Validate. The parts of the assembly become transparent, they act as support or anchor points for the sketches and shapes of the part designed in place.

After clicking In place part and in order to sketch directly on the right plane, select the sketch support face BEFORE starting the sketch.

Once the in place part has been created, it must be validated by clicking the In Place Editing button situated in the center at the top of the graphic display.

Additional information: In the project tree, the part in place is directly attached to the assembly in which it was created.

In Place extruded Parts Links / Videos :

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This command allows to extrude several shapes from several planar sections defined in an assembly. Each shape becomes an in place part of the assembly.

Creation stages / Use: Click the icon or select the Modeling > In Place extruded Parts... command from the drop-down menu. 1. Select sections to be extruded. 2. Define, if need be, the extrusion direction (normal to the profile by default). 3. Define the extrusion bound.

The direction and the limit will be applied to all sections to extrude.

All options are explained in the extruded help.

In Place Assembly

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This command allows to create an in place assembly in order to group several in place parts achieved in an assembly, in a new subassembly, called an in place assembly. This allows you to reorganize an in place design in order to identify a subassembly that will have it's own designation. For example, an assembly with 3 parts P1, P2 and P3. The In place assembly A2 allows to group P1 and P2 in a sub-assembly which is created in the main assembly without creating before this sub-assembly A2 and without having to include it. Then the main assembly be composed of A2+P3.

Creation stages / Use: Click the icon or select Modeling > In place assembly... command from the drop-down menu. 1. 2. 3. 4.

Select the different parts to include. Validate. Select an assembly template. Validate.

Parts and sub-assemblies not made in place in the in place subassembly may be inserted in an in place assembly.

A piping line can be inserted in an in place assembly.

Non rigid subsets (on which there are degrees of freedom) cannot be inserted into an in place set. In the projects tree, the in place assembly can be found by unrolling the assembly in which it has been created. When you declare an in place sub-assembly in a mechanism, if all constituents are in the same rigid group, the in place assembly is added in the same rigid group. If one of its constituent isn't in any rigid group or if they are not in same rigid group, the in place assembly will not be included in any rigid group and you will have to do it manually.

Modifications / Additional information: You can open the In Place Assembly document, draft it, insert it in another assembly, ... To add or remove parts of the in place assembly, simply edit the inclusion.

Extruded bar This command positions the extruded bars in the assembly.

Creation stages / Use: Click the icon or select Modeling > Extruded Bar... command from the drop-down menu.

To be able to use the extruded bars, it is essential that the libraries required for the project be referenced beforehand. The referencing is done via the Add reference contextual command from the references icon in the project tree.

1. Select a type of extruded bar in the drop down list. 2. Select the code of the extruded bar in the drop down list. This command allows you to position an extruded bar on each selected edge, segment, profile or face. 3. Select the reference profile, a segment, edge or face. 4. Select the reference direction to be able to orient the extruded bar. This command positions the extruded bar by selecting its 2 end points. 3. Select the first and second point. 4. Select the reference direction to be able to orient the extruded bar. This command positions the extruded bar on a frame and indicates its length.

3. Select the destination frame. 4. Enter the length of the extruded bar. This command allows to position the extruded bar by constraint positioning. 3. Enter the length of the extruded bar. 4. Position the extruded bar in the graphic area (if the dialog is unpinned, you are able to constraint your extruded bar).

5. Enter the orientation of the extruded bar. The orientation is a rotation around the longitudinal axis. 6. Check or uncheck the Reverse extruded bar. This option reverses the direction of the extruded bar. 7. Select the offset type by clicking one point in the extruded bar preview of the dialog. The selected point becomes blue. The longitudinal axis of the extruded bar will be on this point. It can also be changed by double-clicking one of the yellow points (in the graphic area) 8. If required, enter the value of the horizontal offset. 9. Select the type of vertical offset from the drop down list. 10. If required, enter the value of the vertical offset.

The orientation can be done in the graphic area by dragging handles. The offset can be modified by double-clicking one point in the dialog preview. If a face is selected with the first option, an extruded bar will be positioned on each edge of this face. It is the same thing for the profile, an extruded bar will be positioned on each line of this profile. The extruded bar command is also available by contextual menu from a sketch.

The case of a family of an extruded bar assembly with boolean drivers to manage inclusions into the generic is not managed. In

place parts of the generic assembly must not have conditions to activate/deactivate them.

To use the same profile than an existing one, just select it before using the Extruded bar command.

Available Options: Substituable in upper levels: This option allows to authorize the substitution (replacing) of the extruded bar when the assembly document is included into another assembly. When it is not checked, the extruded bar will be greyed in the substitution dialog box. See the sub-component substitution command for more details.

Modifications / Additional information: To modify the type of extruded bar, its offset, its orientation, use the Edit contextual command. The extruded bar family can contain drivers to be able to modify them during extruded bar inclusion. An extruded bar can be an assembly to allow to manage a different material for each part of the assembly as for example a extruded bar with a seal. During the in place edition of an extruded bar, it is possible to associatively hang on the assembly. The Replace contextual command allows to interchange several extruded bars at the same time.

Miter trim This command creates miter trims on the extruded bars.

Creation stages / Use: Click the icon or select Modeling > Miter Trim... command from the drop-down menu. 1. Select the different extruded bars to cut. The offset is symmetrical. The offset value is the total distance between the 2 cross sectioned planes. The offset is symmetrical. The offset value is the distance between a cross sectioned plane and the center plane. This is half of the total length. The offset is asymmetrical. The first offset is from the side of the first selected extruded bar (sky blue).

2. Enter the offset between 2 extruded bars.

Extruded bars before miter

Extruded bars after miter

trims

trims

The Miter trim operation is displayed in the operations tree. If several profiles are selected, several cuts will be done.

Modifications / Additional information: The Variable angle allows to create a miter trim when the extruded bars have a different width.

Without variable angle

With variable angle

The Create folder option groups all cuts (when several profiles are selected) in a folder of the operations tree. The modification of the tabs cross section is performed contextually from the operations tree or on the edge from the graphic.

Main trim This command creates a main trim on extruded bars. The first extruded bar will extend to the first planar face on the tool extruded bar .

Creation stages / Use: Click the icon or select Modeling > Main trim... command from the drop-down menu. 1. Select extruded bars to modify. 2. Select the tool extruded bar. 3. Check Use Closest Plane so that the first plane of the tool extruded bar encountered is the trimming plane, otherwise the furthest plane is used for trimming. 4. Enter the offset between the 2 extruded bars.

Extruded bars before the main trim

Extruded bars after the main trim

The Main trim operation is displayed in the operations tree. If several profiles have been selected, several cuts will be done.

Contrary to the tabs cross section, only profiles with the same tool extruded bar must be selected..

Modifications / Additional information: The Create folder option groups all cuts (when several profiles are selected) in a folder of the operations tree. The modification of the main cross section is performed contextually from the operations tree or on the edge from the graphic.

Planar Trim Links/Videos:

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This command allows you to create a planar cross section on extruded bars. The first extruded bar will extend to the selected plane on the tool extruded bar.

Creation stages / Use: Click the icon or select Modeling > Planar Trim... command from the drop-down menu. 1. Select extruded bars to modify. 2. Select a trimming plane 3. Enter the offset between an extruded bar and the selected plane.

Extruded bars before the planar trim

Extruded bar after the planar trim in relation to the

selected face

The Planar trim operation is displayed in the operations tree. If several profiles have been selected, several cuts will be done.

Contrary to the miter trim, only profiles with the same trimming plane must be selected..

Modifications / Additional information: The Create folder option groups all cuts (when several profiles are selected) in a folder of the operations tree. The modification of the planar trim is performed contextually from the operations tree or on the edge from the graphic.

Piping Line

This command allows to create a 3D sketch which is the base for the piping line. This sketch uses the 3D sketch Contour command mixed with the piping line creation. The components (flanges, tees, reducers,...) could be added with the Insert contextual command.

Creation stages / Use: Click the icon or select the Modeling > Piping line... command from the drop-down menu. 1. Enter a name and a description for your piping line. 2. Select the piping rule to use with this piping line. 3. Enter the minimal diameter for this piping line. The tubes and elbows with a diameter near but upper or equal to the minimal diameter will be used. For example, if it exits some tubes with diameters of 15mm, 20.3mm and 32 mm, by entering 20mm or 20.3mm as minimal diameter, it is the tube with a diameter of 20.3mm which will selected. A minimum diameter of 0mm allows to use tubes and elbows with the smallest diameter. 4. Select the type of tube and elbow to use and validate with 5. The next stage consists in creating the trajectory (neutral fiber) of your piping line via 3D sketch commands. Reminder: to change the plane, use CTRL+Space keys. When finished, validate this sketch edition. 6. Validate the sketch.

The tubes and elbows are automatically positioned on these segments during the piping line design. If fillets are not added to the sketch, elbows will automatically adapt. If fillets are added to the sketch, the pipe is said "flexible" and will be composed with an elbow and adjacent lines. This tube will be considered as a single part in a bill of material.

This dialog is only used for the creation of a new piping line or to complete the sketch of an existing line. To modify the diameter of an existing line, you have to: Edit the sketch of the piping line. Double-click on a tube to display its dimensions. Double-click the dimension to modify. Validate the sketch.

Available Options: Minimal thickness: For the same diameter, different thickness for tubes and elbows can exist. The entered minimal thickness allows to use the tube and the elbow with the near upper thickness. A minimal thickness of 0mm allows to use the thinnest thickness.

Neutral Fiber: Allows to define the neutral fiber representation when the piping line is projected in a draft. Style: select the style of the neutral fiber. Attributes: by checking this option, you can define the type of line, its thickness and the color of the neutral line. Delete the color by clicking on the cross. Half tone: uses the half tone of the color. (black becomes gray, ....)

Modifications / Additional information:

The Show tubes and elbows mode allows to show or hide tubes and elbows during the piping line sketch edition. To modify the sketch, use the Edit sketch contextual command from the piping line to modify. To modify one of the information upper after validating the piping line, use the Edit contextual command from the piping line to modify. To add component on the piping line (Flanges, reducers, tees, ...) use the Insert contextual command on the piping line to modify.

Angle weld

This command creates a weld angle in an assembly.

Creation stages / Use: Click the icon or select Modeling > Angle Weld... command from the drop-down menu.

To be able to use the weld angles, it is essential that the libraries required for the project be referenced. The referencing is done by using the Add reference contextual command from the References icon of the project tree.

1. Select the type of weld angle seam in the drop down list. 2. Enter the height of the weld seam. 3. Select the first batch of faces. All the faces selected must be on the same side of the weld. 4. Select the second batch of faces. All the faces selected must be on the same side of the weld 5. Checking Limit by neighboring faces to limit the weld extremities by the neighboring faces otherwise 6. Enter the value of the end withdrawal. 7. Enter the joint withdrawal value.

The limit by neighboring faces only supports planar faces.

To accumulate the limitation by neighboring faces on one side and an end withdrawal on the other, the weld must be modified locally.

End withdrawal

Joint withdrawal

Angle weld

Options: Material: To select a specific material for this weld, a material document needs to be opened. Then it will be available in the drop-down list. Made on side: This information will be automatically indicated in the draft by using the Weld symbol command and by checking the Projected symbol welding option.

Modifications / Additional information:

To modify the type of weld, the faces, the withdrawals, use the Edit contextual command .

Groove weld

This command creates a groove weld in an assembly.

Creation stages / Use: Click the icon or select Modeling > Groove Weld... command from the dropdown menu.

To be able to use the groove welds, it is essential reference the libraries required for the project. The referencing is done by using the Add reference contextual command from the References icon of the project tree.

1. 2. 3. 4. 5. 6. 7.

8. 9. 10. 11.

Select a type of groove weld seam in the drop down list. Select the front edge of the weld. Checking Inverted inverts the direction of the front edge. Enter an angle to reposition the weld if required. Checking Limit by neighboring faces to limit the weld extremities by the neighboring faces otherwise Enter the value of the end withdrawal. Check Reverse backing if required (to also have the weld on the opposite edge). a. Select a type of groove weld seam in the drop down list. b. Enter the thickness of the parts to be welded. Enter the height of the high weld. Enter the angle of the upper plug. Enter the height of the plug of the upper weld. Enter the width of the plug of the upper weld.

Frontal view of weld with plug height and width different by 0mm

12. 13. 14. 15.

Frontal view of weld without plug height and width ( at 0mm)

Enter the height of the lower weld. Enter the angle of the plug of the lower weld. Enter the height of the plug of the lower weld. Enter the width of the plug of the lower weld.

The limit by neighboring faces only supports planar faces.

To accumulate the limitation by neighboring faces on one side and an end withdrawal on the other, the weld must be modified locally.

Options: Material: To select a specific material for this weld, a material document needs to be opened. Then it will be available in the drop-down list. Made on side: This information will be automatically indicated in the draft by using the Weld symbol command and by checking the Projected symbol welding option.

Modifications / Additional information: To modify the type of weld, the faces, the withdrawals, use the Edit contextual command .

Weld definition

This command defines a shape like weld seam. In certain cases, an angle or groove weld cannot be created, so simply make a template of a shape and define it as weld.

Shape must be created in the assembly, without creating a part, by using Extruded, Revolved, Pipe command from the drop-down menu Modeling > Local Shapes.

Creation stages / Use: Click the icon or select the Modeling > Weld definitions... command from the drop-down menu. 1. Select the local shape(s) to be defined like weld seam. 2. Select the face in contact with the weld on the first welded part. 3. Select the face in contact with the weld on the second welded part.

Options: Material: To select a specific material for the weld, a material document needs to be opened. It will appear in the drop-down list.

Modifications / Additional information:

To modify the selections of the weld definition, use the Edit contextual command.

Distribution

This command allows to distribute components along a line in an assembly document. For example, you can use this command to distribute partitions into an open-space, a handrail and its supports or drawers into a cabinet (distribute 3 drawers by specifying the height of one of them for example).

Creation stages / Use: It is possible to distribute up to two components at the same time. The components will be included alternately. The first component always appear at the start and the end of the line. So the first component has always one more occurrences that the second component. One of the component can be a blank space; which allows to get an alternating of a component and a blank space with a given length. For each component, you can set its length, its position according to the line and its family code as well as the drivers of the component. The provided length represent the base length along the line. This value is a reference length that will vary according to the settings and options used. In an assembly document, click the icon or select the command Construction > Distribution... command from the drop-down menu.

The components that can be used with this commands are family document from distributable part document or assembly. The generic documents of these family documents must provide the function Distributable component and the family documents must provide the driving Distributable family (by using the command "Tool>Provide Driving"). This driving is available into the library " TopSolid Mechanical>Components>General ".

Available options: Distribution: This rubric allows to define the path of the distribution. several modes are available: Allows to use a sketch, segment, or edge as path. You also need to define the vertical direction. Allows to use two points that define the extremities of the path.

You also need to define the vertical direction. Allows to define the path through a frame and a length. The frame origin is used as starting points and the Z axis is used as the path direction.

Distribution mode: Two distribution modes are available: Distribute: The components are positioned with a fix length one after the other until the end of the path line. Mark out: You provide the number of components and their length is adapted so the sum of the components length is equal to the path length. The "distribute" mode can result in an empty gap at the end (a remainder) too small to be filled with an additional component. While the "mark out" mode never gives remainder.

First component: The first component can be: A family document: The drop down list propose all the distributable families from references libraries and project. One the family chosen, you can select the code and/or the drivers values. A blank space: In this mode, the blank spaces are distributed along the line. This can be useful, for example, if you want to distribute a bar with fixed width and variable blank spaces between the bars.

For each component, you can set its length, its position according to the line and its family code as well as the drivers of the component. The provided length represent the base length along the line. This value is a reference length that will vary according to the settings and options used. Sub Components: This button allows to access to the sub components configuration windows (see Sub Components windows) To get access to these settings, you must have activated the advanced option "Substituable in upper level" while assembling the consituents of this component in the generic document.

Second component: The second component has an additional mode: No component: Allows to distribute only one component.

First / Second component positioning: These two rubrics allows to define the initial positioning of the first and second component. Orientation: the orientation angle applies a rotation of the component around the axis defined by the path line. Invert: turn around the component around the vertical direction defined in the first rubric. Key Points: allows to choose the hooking point of the component on the path line. To select the key point, just select it in the component graphic preview. Horizontal / Vertical shift: if needed, you can apply a vertical or horizontal shift to the position of the component.

Advanced Options: Numbering: This option describe the way the component are ordered along the line: Ascending / Descending: the components are ordered one after the other from the starting point (ascending) or from the end (descending) of the path line. Alternate Ascending / Descending: in these modes the first component is positioned on one extremity and the second one at the other extremity and so on.

The alternate mode is important when the number of components can change (modification of the component length or the path line length). Thus, whatever the number of occurrence of the component, it will always be the occurrence 1 and 2 that are located at the extremities of the path. So this make the design more reliable if you used these occurrences to create other entities.

With the Distribute distribution mode, the following options becomes available: Remaining length: With the "Distribute" mode, you may get a remainder (empty gap). This option allows you to specify if this remainder must be at the end, at the start or distributed on both extremities of the path line. Remainder distribution mode: It is possible to decide how you manage the remainder: Do not distribute: the blank space of the remainder is left in its state.

Fill remainder: the blank space is filled with an additional component. But only if the remainder length is higher that the value provided in the option "Minimum for filling".

Distribute remainder: the length of the included occurrences is extended so their cumulated length fill the blank space of the remainder.

Distribute one more: an additional occurrence is added and the length of all occurrences is reduced so this additional component will fill the remainder.

Modified component: If you distribute two components, and the remainder is distributed (Distribute remainder or Distribute one more), you can choose to alter the first component, the second or both. Remainder spread mode: When you alter the length of both component, you can add or remove either an equal value of length on both component or a proportional length value according to the reference length given for each family component.

Modifications / Additional information: In the graphic area, a numbered label is created for each occurrence of the components. You can drag these labels (using drag and drop). In the contextual menu that appear on a label, you have access to the commands "Exception" and "reset position" (if the label has been moved). It is also possible to start the command Exception if you double-click on the label. Exception: This command open a dialog box that allow to replace this specific occurrence. You can replace the family by another, replace a blank space by a family, change the code or drivers of the family,... If you want to change the length without changing the family, you must give the length value and leave the family list empty. You can replace a family by a black space: select the black space option and give the length if you want a specific dimension, or leave the length field empty to keep using the reference length.

Modify an occurrence: If you need to modify the geometry of some occurrences (drilling, pocket, trimming,.....) you need to convert them into local part as you would do for a repetition.

Distributable component: The creation of a component that can be used with this command follow the same conception method as any other common parameterized component. To make this component available into the family list of the Distribution command, you need as well to: Provide the function "Distributable component" into the generic document (part or assembly) of your component. On this function, you need to provide the following publications:

Top Right Point: this is the upper right point of the component on the XY plane of the provided frame bellow. Bottom Left Point: this is the lower left point of the component on the XY plane of the provided frame bellow. Additional Key Points: allows to define additional key points you may need to position your component. Frame: the plan XY of this frame must be normal to the distribution line (the Z axis represent the direction of the distribution line). Length: it must be associated with the parameter that drives the length of the component (the variable dimension along the distribution line).

Provide the driving "Distributable Family" into the family document of your component by using the command "Tools>Provide driving"

Use process

This command uses the processes of a component already included on a part to be operated.

Creation stages / Use: Select Modeling > Use process ... command from the drop-down menu. 1. Select the part with a process. 2. Select the process to apply in the drop down list.

Available Options: Automatic part process choice: This option allows to automatically select the process to use according to the definition of the Process Rules document dragged in the Favorites folder of the project. These rules select the most adequate process to use. For example, if the process rule is defined to create a tapped hole when a hexagonal head screw is included on top head, in this case, the process will be automatically done without displaying any dialog. If one of the rule condition does not match, the process dialog will be displayed. Manual mode: This mode allows you to select the process operation to apply. For example, the process of a screw comprises 3 operations, spot facing, drilling and tapping. 1. Select the operation to use. 2. Select the part to operate.

Drivers: Some processes use drivers. These values can be changed during the process use. For example, during a screw inclusion, the hole driver is the type of the clearance hole diameter. It can be Fine, medium or large. The drivers for a tapped hole are: Through all tapping or Complete tapping. Subcomponent Processes: This option is displayed when a component of components has its own processes (provided by a function document for example) and also contains one (or several) processing part(s). It option allows to apply the processing part processes. Such components are available in the TopSolid Meusburger Tooling library (in the Components\Movement\Guiding Rails directory).

In manual mode, operations are applied one by one.

Parts Operations: Possibility to activate additional dialog box using process (generally when modifying parts from assembly operations). This dialog allows to define how TopSolid will manage modifications done on parts (from a process or another operation). Activating of this dialog is done from Tools > Options > Assembly > Parts Operation (see on-line help on this chapter for more information).

Create Processes

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This command allows to make the processes of several occurrences of component at once

Creation stages / Use: Select the Modeling > Create Processes... command from the drop-down menu. In the Occurrences list, choose the occurrences of which you want to make the processes. In the Exclusions list, choose the occurrences of which you do not want to make the processes. If you run the command again, this list will be initialized with the occurrences previously selected. The Detect occurrences without process button allows you to automatically select the occurrences that can use a process that has not been used. The repeated occurrences from which the processes have been done in Assembly mode are not detected, where as the ones from which the processes have been done in Part mode are not. In such case, it is recommended to remove them from the Occurrences list or to add them in the Exclusions list.

When the dialog is validated, the processes of each occurrence are executed one by one. The processes of sub components are not executed. This command does not manage the extruded bar processes.

Available options: Hide: This option allows you to hide the selected element, it allows to select the elements located behind.

Use Weld Process Links/Videos:

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This command allows you to subtract the weld lengths in parts in contact with the selected lengths. Operated parts can be selected automatically or manually.

Creation stages / Use: Click the icon or select Modeling > Use Weld Process... from the drop-down menu. 1. Select the weld lengths. 2. Validate

Available Options: Hide: The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind. Manual mode: This mode allows you to select the parts to sew manually. Representations: This option allows to select if parts to be operate will be operate in all representations or only in the detailed representation.

Parts to weld must be in contact with the weld in order to be operated. The process generates associative operations in part documents or local operations if parts can be modified locally. It is the weld length shape that is used for subtractions. When All Representations is checked, the weld length appears in all representations. If Detailed Representation is selected, the weld lengths only appear in the detailed representation (and the design representation). No matter the representation option chosen, the process will be performed.

Reproduce Process

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This command allows you to apply process of an occurrence to several occurrences.

Creation stages / Use: Select the Modeling > Reproduce Process... command from the drop-down menu. In the Reference occurrence field, select a reference occurrence in order to get its process. In the Additional occurrences area, select one (or several) occurrence(s). The Process field displays the process of the reference occurrence, it cannot be modified and it will be applied by all the additional occurrences.

In order to be selected, the additional occurrences must provide the same function than the reference occurrence. The repeated occurrences which process has been repeated cannot be selected as reference occurrence, nor as additional references.

Available options:

Hide: This option allows you to hide the selected element, it allows to select the elements located behind. Create processes: When this option is checked, the occurrences where process has not been used can be selected, then new process operations are created. When this option is unchecked, existing process operations are modified only, occurrences where the same process (the same or using the same function) has been used can be selected only.

Marking

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This command allows to apply marking defined in the part document to the shape.

Creation stages / Use: Select the Modeling > Marking... command from the drop-down menu. With Automated mode: 1. With this mode TopSolid scans all the parts and detects the ones that can be marked (those that contain a marking operation). 2. Validate to apply marking to the part. Without Automated mode: 1. Select the shape to modify. 2. Select the sketch to imprint.

Marking operation will modify the part according to settings of parts

operation options.

Available options: Lightweight: With this mode, no imprint will be done on the part. Automated + lightweight: In the part document, temporary text is replaced by the value of the property defined in the part marking. Not automated + lightweight: Sketch to mark is displayed in the part document. In the operation tree of the part document, Ø symbol is added in front of the lightweight marking.

Machining process (available when Automated mode is off) : This option allows to assign a machining process to the operation. This machining process is recognized by TopSolid'Cam. It can also assign a color to the operation.. 1. Select a machining process document in the drop-down list. 2. Select a process in the drop-down list.

Representations: All representations: Marking will be done on all shape representations. Detailed representation: Marking will be done on detailed representation only. This representation must be displayed to see the operation.

Trim

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This command allows you to trim a part in an assembly, by surface, face or plane.

Creation Stages / Use: Click the menu.

icon or select Modeling > Trim... from the drop-down

1. Select the part(s) to trim. 2. Check or uncheck Detailed Representation. If this option is checked, only the detailed representation will be trimmed. 3. Define the type of trim element. 3. Select the trim element corresponding to the type chosen. 4. Invert if necessary. 5. Validate by clicking .

Available Options: Type of item: Plane: the trim element must be a plane or a planar face. The trimming extends to infinity (a plane does not have borders). Surface: you must select a surface or a single face of a shape. If the surface is planar, then the trim is infinite. If the

surface is not planar, it must completely pass through the parts to trim. Shape: trimming occurs using all of the faces of the shape. The "reverse" option allows you to choose the side that will be removed. Faces: this mode allows you to select a set of faces of a shape. The batch of faces selected must completely pass through the parts to trim. The "reverse" option allows you to choose the side that will be removed

Offset: This option allows you to add an offset on the trimming in relation to the trimming element. You can enter a negative value to apply to the offset in the opposite direction. The offset is computed by offsetting the trimming element. Trimming using a surface with a negative offset.

Representations: Select if the trim has to be done in all representations or only in the detailed representation.

Keep trimmed side: Allows to keep the trimmed side. A new part document is automatically created. This document is a derivation of the original part and contains only the trimmed side.

Straighten lateral faces:

This option allows to straighten lateral faces. They will be normal to the limited faces. This option is useful for sheet metal parts and corresponds to the Lateral faces straightening command from the sheet metal menu.

Trim by profile

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This command allows you to trim a part of an assembly by profile.

Creation Stages / Use: Click the

icon or select Modeling > Trim by Profile... from the drop-down menu.

1. Select the part(s) to trim. 2. Check or uncheck Detailed Representation: If this option is checked, only the detailed representation will be trimmed. 3. Select Trim by Extruded Profile, Trim by Revolved Profile or Trim by Imprinted Profile. 4. Select the trim section. 5. Check or do not check Invert to invert the trim side. 6. Select the direction for a limitation by extruded profile, the axis for a limitation by turned profile or the sections for a limitation by printed profile. In this case, also select the direction.

Available Options: Type of element: Extruded: Trimming occurs by extrusion of the profile according to the chosen direction (by default, this is the normal direction to the plane of the profile). Revolved: Trimming occurs by rotation of the profile around an axis that you define Imprinted: The trim is done by extruding the imprinted sections following the selected direction (by default, it is the direction normal to the section).

Reverse: This option allows you to reverse the trim side. If this option is not checked, the shape generated by the extruded or turned profile is removed from the part to modify. If this option is checked, then the intersection between the shape and the extruded or revolved profile remains. Trim by extruded profile without Reverse option.

Trim by extruded profile with Reverse option.

Trimming by revolved profile without Reverse option.

Trim by revolved profile with Reverse option.

Partial trimming (for trimming by an extruded or revolved profile): This option defines the trimming distance in the 2 directions for trimming with extruded profile and the angle in the 2 directions in relation to the axis chosen for trimming with revolved profile. Partial trimming with extruded profile.

Extend until (for the

Partial trimming with revolved profile.

mode ):

This option allows to choose if the profile will be extended until the next edge or up to the boundary edge .(boundary edge is only available for surfaces, a solid part has no boundary edges). Extend until first edge

Extend until boundary edges

Representations: Select if the trim has to be done in all representations or only in the detailed representation.

Keep trimmed side: Allows to keep the trimmed side. A new part document is automatically created. This document is a derivation of the original part and contains only the trimmed side.

Straighten lateral faces: This option allows to straighten lateral faces. They will be normal to the limited faces. This option is useful for sheet metal parts and corresponds to the Lateral faces straightening command from the sheet metal menu.

Modifications: The modification can be done from the operation tree or graphically in the popup menu from one of the faces resulting from the trim.

If the profile is open, then it should overlap the part. Partial trimming is not possible if the profile is closed.

Reciprocal Trimming Links/Videos:

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This command allows you to limit 2 shapes one in relation to the other, in an assembly.

Creation stages / Use: Click the icon or select Modeling > Reciprocal Trimming... from the drop-down menu. 1. Select the face(s) of the first shape. 2. Check or uncheck Detailed Representation. If this option is checked, only the detailed representation will be trimmed. 3. If necessary, inverse the side to keep. 4. Select the face(s) of the second shape. 5. Check or uncheck Detailed Representation. If this option is checked, only the detailed representation will be trimmed. 6. If necessary, inverse the side to keep. 7. Validate by clicking .

To select only some of the shape's faces, use the rotating selection.

The preview (orange part) indicates what will stay.

Drilling

This command allows to drill a part or a batch of piled parts.

Creation stages / Use: Click the menu.

icon or select Modeling > Drilling... from the drop-down

1. Select and/or create a drilling template. 2. Select (or create by clicking on "+") the drilling frame. 3. If the drilling is blind, by checking the Automatic detection box, impacted parts by the depth will be automatically selected. 4. Select the shapes to drill. 5. Validate the command with the button

To be able to create tapped holes, you need to reference a library containing the standard you wish to use for the tapping.

In/Out counter sinking:

Allow to apply different-sized countersinkings (length and angle) to each type of drilling.

In/Out counter sinking: Allow to activate the counter sinking. A boolean parameter can be used to condition the counter sinking creation. Length: Value of the countersinking length. Pitch factor: If the drilling primitive is a tapping hole, you can use a counter sinking length whose the value is function of the pitch and a factor defined by

Advanced Options: Machining process: Machining process: This option allows to assign a machining process to the operation. This machining process is recognized by TopSolid'Cam. It can also assign a color to the operation.

Available Options: Templates and types of drilling:

With these options you can:

Current Fast Drillings: These three buttons allow you to create a spot faced hole, tapped hole or smooth bore without opening the drilling templates.

Explore Templates: By clicking on this option, you access the list of drilling templates where you can select the one you want to use. Frame: With this option, you define the frame on which the drilling will be carried out. Each drilling operation requires a frame which defines the position of the drilling and its direction. The drilling is done based on the Z- of the frame. The Z- axis must therefore be directed toward the inside of the part so that the drilling can be carried out. If there is no drilling frame, it can be created in a dynamic way on certain types of faces by moving the mouse over this face: Plane face: the frame created is a is a constrained frame on the nearest edges of the face.

Cylindrical face: a radial frame is created.

Face with circular edges: a frame on face and center point which is created.

Reference frame: Possibility to use a reference frame on which be based axes of the constraint frame. Regarding the constraint frame, the reference frame can be used with automatic mode only.

The constraint frame of the drilling uses axes of the reference frame.

Advanced options: Extension process of Countersink: This option defines the countersink drilling process at the entry face. In fact, drilling starts in the origin of the frame. However, in the event of an inclined face or the presence of a shoulder next to the drilling, TopSolid needs to "extend" the drilling above the origin point to achieve a good result. These are the two possible modes: Extend surfaces

Add a cylindrical face

Representation: This option allows you to define if the drilling must be done on all shape representations or only on the detailed one.

Drilling processes: Below the main options, a list of icons is displayed which allows you to modify the parameters of the different procedures of the drilling template used. These icons change regarding the chosen drilling hole type. By default, the values are those of the drilling template. It is therefore not required to access this if the values of the template are those you wish to use. See here for the detailed description of the different procedures.

Repetition Links / Videos :

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This command allows to repeat an operation performed in the assembly.

Creation stages / Use: Click the icon or select the Modeling > Repetition... command from the drop-down menu. 1. 2. 3. 4.

Select operations to repeat. Choose the mode to use (Assembly or Parts). Select the pattern. Validate.

Assembly mode: The repetition operation is performed in the assembly. The part then contains as many original operations as the number of occurrences resulting from the repetition.. Parts mode: The repetition operation is performed in the part. The part contains the initial operation and its repetition. The repetition options of the Part document are then proposed, including the Fast mode

Modifications / Additional information:

This operation is performed automatically when a component is repeated with processes.

Sheet Metals Recognition

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This command allows to analyze all parts of the assembly and to convert them as sheet metal if the entered maximum thickness is taken into account.

Creation stages / Use: Click the icon or select the Modeling > Sheet Metals Recognition... command from the drop-down menu of an assembly document. 1. Select what is to display. All displays all parts of the assembly, Convertible displays only parts which can be converted into sheet metal parts, Sheet metal displays sheet metal parts, Impossible to convert displays all parts which can't be converted. 2. Enter the maximum allowed thickness to convert parts into sheet metal parts. 3. Check the Straighten lateral faces if needed option. faces to straighten are automatically selected without any user interaction. A straighten lateral faces operation is created in each part. 4. Validate.

Parts with a thickness higher then the entered one aren't taken into account for the sheet metal conversion.

Available options: Parts: The table indicates parts name, the part status, information (synchronized), the thickness, its matter and its unfolding rules if any. Parts on cyan background are parts which match the allowed thickness and which can be converted into sheet metal. You can uncheck them to not convert them. Parts on green background are already sheet metal parts.

By clicking a line, the preview of the part is displayed.

Local Assembly

This command allows you to define a part or subassembly selection (created in place or not in place) as a local assembly. A local assembly allows you to restructure the organization of assembly document parts. A local assembly is considered a subassembly and will be listed as such in a bill of material. You can also make the draft as a local assembly only rather than a complete assembly.

Creation stages / Use: Click the icon or select Modeling > Local Assembly... from the drop-down menu. 1. Enter the name of the local assembly. 2. Also provider a description, reference. and comment, if necessary. 3. Select the parts and sub-assemblies to add to the local assembly. 4. Validate.

A local assembly is only defined in the assembly document. There are no specific documents that correspond to its contents. It is preferable and more efficient to use local assembly rather than in place assembly when it does not have to be included in other assemblies, while it is more powerful.

To structure the BOM, it is possible to select a local assembly already existing in the document. It is useful to create many level of sub assembly.

Modifications / Additional information: The local assembly is found in the "Parts" folder of the entity tree. Also, you can edit it to add or delete parts from the list.

Local Parts

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This command allows you to define a part as a local part. A local part of an assembly is a part that is defined locally in the assembly document and not in a separate part document. A local part cannot be reused in another assembly. As opposed to the part designed in place, it is only used once, in the definition assembly.

Creation stages / Use: Select Modeling > Local Parts... from the drop-down menu.

1. Select parts to define as local parts.. 2. Check in the drop-down list, the properties to inherit. Inherited properties will be filled with their origin values, those non inherited will have empty values. Regardless the property (inherited or not) its value can be changed with the Properties contextual command from the part in the Parts folder of the entities tree (Parameters folder)

Once defined, each part is hidden and replaced by a local shape in the assembly. You can then perform operations individually on each copy. It is possible to apply component processes on a local part. In analysis stage of the assembly document, each local part has its own analysis properties management (enclosing box, physical properties, threading management,...). Thus it is possible to edit each one of these properties from the operation tree when set in analysis stage.

When a part is converted into local part, an operation "Conversion" is created in the operation tree. Moreover, its icon is different in the entities tree: Local part In place part Included part

Cases of use: In all cases where this is possible, it is preferable to use the "Other > Derive Part for Modification..." command that corresponds to the usual method. (see the "Special Parts" Chapter in the User's Guide) But there is at least one case where it is not convenient, when the number of special parts is variable. For example, this scenario can occur if you wish to modify all copies of a repetition and that you wish to associatively change the number of copies. In this case, you cannot create a part derivation for each instance (a document cannot be automatically created or deleted for a simple update when the value of a setting changes). It is therefore necessary to use a local part.

Example of a repetition trim by plane: Without definition in local parts

With definition in local parts

Modifications/Additional information: In the Parts folder of the entites tree, you can find details about the local part (by clicking on the [+] symbol. You can access to its properties (eg Occurrence Properties ) and its parameters (description, Part Number, ...).

Disassembly

This command allows to convert a sub-assembly inclusion into an inclusion of all the unitary parts of this sub-assembly. This can be useful for example to modify the bill of material structure for these elements when you display it in multi-layer mode.

Creation stages / Use: Select the Modeling > Disassembly... command from the dropdown menu. 1. Select the sub-assembly you need to disassemble. 2. Validate by clicking on .

In the operation tree, a new operation named "disassembly" is created. It is still possible to access to the original assembly inclusion operation in the operation history. In the part folder of the entities tree, the assemby does not appear anymore and is replaced by all the parts that it contains.

Occurrence Properties

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This command allows to define the bom index and the properties of an occurrence of a part (or sub-assembly). This can be done manually or with a reference occurrence.

Creation stages / Use: Choose the Modeling > Occurrence Properties... command from the drop-down menu or selected an occurrence (or a sub-assembly) of a part and then choose the Other sub menu from the contextual menu. Mode with reference occurrence: In the Reference occurrence field, select a reference occurrence in order to get its properties and/or its index. In the Additional occurrences area, select one (or several) occurrence(s). Chose one or several properties in the Properties area and then define a value of each property and/or type the value of the index. Confirm with the button in order to apply the modifications to the reference occurrence and the additional occurrences as well. Manual mode:

In the Additional occurrences area, select one (or several) occurrence(s) or select one occurrence in the Reference occurrence field. Chose one or several properties in the Properties area and then define a value of each property and/or type the value of the index. Confirm with the button in order to apply the modifications to the reference occurrence and the additional occurrences as well.

The components linked to a part are grouped together in a BOM: for example, you can apply the index 101 to all the M5x30 screws inserted into the plate with index number 100, apply the index 201 to all the M5x30 screws inserted into the plate with index number 200, etc...

Available options: Occurence bom index : This options allows you to grey out the field which allows to type the occurrence bom index.

Modifications / Additional information: The index of parts indexed in this way is displayed in square brackets in the Parts folder of the Entities tree. It is shown on a green background in the bill of material. You can change this color in the Bom page of the Tools > Options command. An index can also be forced directly in a bill of material by selecting a part in the list and checking the Occurrence index

option.

A distinction is made between Occurrence properties and parameters : Occurrence properties are local to occurrence. The properties don't inherit from occurrence to occurrence. Parameters are inherit from occurrence to occurrence.

Occurrence properties are not made to scrapping properties already present in the definition document. A check is made when the occurrence is updated, in case of conflict (property defined in occurrence and in the definition document), it's the property of definition document which is favored and the occurrence property is deleted. Consequently, this command doesn't allows to modify the system parameters.

Envelope

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This command allows to create an envelope shape from shapes visible faces of an assembly representation.

Creation stages / Use: Select the Modeling > Local Shapes > Envelope... command from the drop-down menu. 1. Select the representation to use to create the assembly. All shapes visible faces of this representation are taken into account. 2. Select the destination envelope representation. 3. Validate by clicking .

The result is a shape which can be surfacic. The calculation can take a while. If one part of the used representation is modified, the envelope is calculated again.

To save calculation time when modifying, it is possible to deactivate the Automatic Refresh by using the contextual command via the operation.

Available options: None: The shape is created, but is not in a representation. It can be dragged into it later.

Existing: Select a destination representation for the envelope by selecting it in the drop-down list. Visually the shape will be mixed with other parts.

Simplified: The shape is created in the simplified representation.

New: The shape is created in a new created representation.

Whatever the envelope is in a representation or not, an Envelope operation is added to the operations tree and the shape is added to the Shapes folder of the entities tree.

Modifications / Additional information: It is possible to edit the operation to change the used representation to calculate the envelope.

Make locally modifiable Links / Videos:

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This command allows you to define a part included in an Assembly document or in a Unfolding one, as modifiable to be able to create operations (pocket, trim and drilling) directly in the assembly or in the unfolding document without modifying the main part document.

Creation Stages / Use: Click the icon or select Modeling > Local Shapes > Make locally modifiable... command from the assembly drop-down menu or Sheet Metal > Make locally modifiable... command from the unfolding drop-down menu. 1. Select an included shape in the Assembly or an unfolding document. 2. Validate the modification with .

A part or an unfolding locally modified doesn't create a new document regarding the Pdm management.

A part or an unfolding locally modified keeps the material.

Modifications / Additional information: This command generates an operation named "Modifiable" followed by the name of the shape selected in the operations tree.

Part shapes Links / Videos :

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This command allows to create shapes by copying the shapes of an included part.

Creation stages / Use: Select the Modeling > Local Shapes > Part shapes... command from the drop-down menu. 1. Select the part to copy. 2. Validate the command.

The resulting shapes are listed in the Entities tree's Shapes folder.

Available options: Refresh auto: Shapes can be updated automatically or manually. When a shape needs to be updated, use the Refresh button of TopSolid or right click on the operation (an out-of-date operation will be written in blue in the Operation tree).

Delete part: Using this option, the part will be deleted from the Parts folder of the entities tree.

Modifications / Additional information: In TopSolid'Cam, this command allows you, for example, to create machining operations on the copied shapes to avoid recalculation each time the part is modified.

Overview of mechanism commands

The assemblies can be either rigid or articulated, they are then called mechanisms. Mechanisms (e.g. : Cylinder, Rolling, ...) have internal degrees of freedom that allow them to be included in a higher level assembly in order to satisfy defined positioning constraints. This way, it will be possible to utilize the stem in the casing of the jack to fit it in the assembly being used. Regardless of the method used to create the assembly, a rigid assembly is ultimately achieved, which can then easily be transformed into a mechanism, if necessary, in a designated later stage, the modeling stage (i.e. once the parts of the assembly have been defined and finalized): the Mechanism Stage. This also applies for an assembly achieved by importing a neutral STEP type format or similar, which only contains the information enabling the parts to be positioned correctly, but not which defines if they are mobile or not, and if the case, how. This option is a considerable benefit compared to other products which only provide the notion of constrained positioning, and which therefore do not allow a part designed on site to easily be made mobile, or whose positioning constraints have no relation to how it is supposed to move. Most of the commands to use to define and manipulate a mechanism are located in the Mechanism menu and it will also be very useful to use the contents of the Mechanism folder in the entities tree, which will contain all the relevant information on the composition of the mechanism being defined. Rigid Assembly You can create assemblies that are not mechanisms (this mode is used when creating a new assembly with a blank template). These assemblies do not have the Mechanism folder in the entity tree, nor do they have the Mechanism stage. They correspond to composite parts or rigid assemblies, such as, for example, fabricated chassis. It is possible to change this kind of assembly to a Mechanism with Mechanism ... command of Mechanism Menu. The same command allows you to perform the reverse operation if a mechanism assembly is applied (like a mode).

Rigid group Plane support Sphere on plane Point on profile

Merge rigid groups Ball joint Sphere on sphere Rigid Slot - Axis

Linear spring Torque force Scenario Export the measurements Angle measurement Angle weld Miter trim

Angular spring Translation velocity Kinematics simulation Trajectory

Distance measurement Groove weld

Slide

Pivot

Point on axis Screw

Axis on plane Rack and pinion Sphere on sphere Constraint

Sphere on plane Constrained configuration Linear damper Rotation velocity Dynamic Simulation Acceleration measurement Force measurement Weld definition

Angular damper Joint driving tasks View Angular velocity measurement Energy measurement Extruded bar

Cylindrical joint Point on plane Gear Sphere on surface Positioning Punctual force Force driving tasks View the measurements Angular acceleration measurement Velocity measurement Main trim

Configurations

When the rigid groups and the joints are defined, there is a mechanism in due form, and when the assembly is included in an assembly of a higher level, the articulations can be activated when positioned in relation to the other parts of this assembly. However, it can also be useful to visualize certain key positions of the mechanism locally, without having to include it in another assembly. This is done using the notion of configuration. A configuration of the mechanism is actually a position of the mechanism compatible with the constraints of its joints. The system automatically creates a configuration which cannot be deleted and which corresponds to the position of the parts at the end of the modeling stage, the configuration of design. You can create other configurations, for example configurations defined by constraints, using the Constraint Configuration command, such as if the mechanism was included in a higher level assembly: Rigid Groups are moved by taking into account the joint constraints to accommodate the positioning constraints that you can create using the various Mechanism menu commands (similar to the constrained positioning used when modeling an assembly by remounting). One of the different existing configurations is called the current configuration, its name displayed in the corresponding drop down list in the menu, and it can be changed by selecting another configuration.

When working in the Mechanism stage, parts can be seen in their position corresponding to the current configuration.

Mechanism

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This command allows you to create a mechanism. This stage is necessary to configure the kinematic or dynamic.

Creation stages / Use: Click the icon or select Mechanism > Mechanism... from the drop-down menu.

When an assembly with mechanism is included in a fixed main assembly which has also to be convert to a mechanism, it is possible to Inherit rigid groups, joints and forces from sub-assemblies already defined as mechanism. For a better readability, inherit elements are named with the name of the assembly document and name of the joint/rigid group/force in this assembly.

You can transform a mechanism rigid assembly (fabricated chassis or imported assembly) with this command. The same command allows you to perform the reverse operation if a mechanism assembly is applied. This operation destroys all mechanism created operations (scenario, constraint, ...). The Mechanism folder is deleted from the entity tree.

Convert positioning

This command converts the positions of the assembly in rigid sets and joints.

Creation stages / Use: Click the icon or select Mechanism > Convert Positioning from the drop-down menu.

Only one positioning is required before converting. To do this, simply open the operations tree and merge the positionings amongst themselves with the popup menu. Some over-complex conversions may only be done partially. In all cases, the user must verify and correct the result if required. The positioning must have some degrees of freedom ( parts must move with the mouse). If all is constrained, the result will be a rigid group. After this command has been used, it is no more possible to use it for this mechanism.

Additional information: To be able to use this command, you must first create a mechanism of the assembly by using the Mechanism command. Then the icon will be ungrayed.

Rigid group

This command creates rigid groups. A rigid group is a group of interdependent parts. When a joint is allocated to a rigid group, all the parts in this rigid group are involved.

Creation stages / Use: Click the Rigid group icon or select the Mechanism > Rigid group... command from the drop-down menu. 1. Click the different entities to be inserted in the rigid group.

A "ghost" rigid group can be created. This is a rigid set that contains only one point or frame, allowing you to make an intermediate joint. For example. A is a rigid group that must be moved linearly and around an axis in relation to a rigid set B. F is a "ghost" rigid set. You can place a prismatic joint between A and F, and a pivot joint between F and B.

When we use a in place assembly in a mechanism, if all its parts are in the same rigid group of the mechanism assembly, then the in place assembly is added to this rigid group. If one of the part is not in a rigid group or if some parts are not in the same rigid group, then the in place assembly is not added to any rigid group, and you have to add it manually.

Additional information: The system automatically creates a rigid group that cannot be deleted and will always be fixed while using the mechanism, which is the built rigid group. This can be empty if required.

Available Options: Hide: The box allows to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Not empty: The box allows to modify the behavior of a rigid group when it is empty. If the option is checked and if all entities of this group are deleted: If the Update heals is active, the rigid group is also deleted. If the Update heals is not active, the rigid group becomes invalid.

Physical properties: Possibility to assign physical properties to a rigid group. Values to define are the mass and principals moments (X, Y and Z) according to a principal frame.

Modification : To modify a rigid set, use the Edit popup menu in the entities tree, in the Groups folder.

Merge rigid groups

This command merges rigid groups. The contents of the 2 rigid groups will be put into the rigid group to be conserved.

Creation stages / Use: Click the Merge rigid groups icon or select the Mechanism > Merge rigid groups... command from the drop-down menu. 1. Click the rigid group to be conserved 2. Click the rigid group to absorb.

Modification : To modify a rigid set, use the Edit popup menu in the entities tree, in the Groups folder.

Moment of inertia of a rigid group

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This command provides information on the moment of inertia of a rigid group.

Creation stages / Use: Select Mechanism > Moment of Inertia of a Rigid Group... from the drop-down menu. 1. Select the rigid set. 2. Select the axis of the moment. 3. The result is displayed in the Moment of inertia box.

In order to turn on this command, the physical properties must be turned on.

Prismatic Joint

This command allows to create a prismatic joint between 2 rigid groups.

Creation stages / Use: Click the icon or select the Mechanism > Prismatic joint... command from the drop-down menu. 1. Select the first rigid group. 2. Select the second rigid group. 3. Select the direction of the translation. This direction indicates the positive value of the movement of the 2nd rigid group in relation to the 1st. 4. Enter the initial distance. This is the initial value of the joint, as represented in the design configuration. For example, if an actuator is designed with the rod half out and its initial value is 40mm, TopSolid considers that the rod is out by 40mm, if the maximum limit of the rod is 40mm, the rod cannot go in any further. 5. Check Limits to be able to fill in the minimum and maximum distances. 6. Viscous Friction can be taken into account by checking this option.

When the limits are filled in, limit stops are put in place during the manual displacement of the rigid sets. These limits have no impact when a scenario is used.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Revolute Joint

This command allows to create a revolute joint between 2 rigid groups.

Creation stages / Use: Click the icon or select the Mechanism > Revolute... command from the drop-down menu. 1. Select the first rigid group. 2. Select the second rigid group. 3. Select the rotation axis. The direction indicates the direction of positive rotation of the 2nd rigid group in relation to the first, if this joint is used in a task. 4. Select a center point. This optional possibility may be useful in dynamics. The point chosen for greater calculating precision will be projected to the axis selected previously. 5. Check the multi-turns angle if the revolute joint needs to turn more than 180°. The time required for calculating may be long. In the event of a geometrical change, the rigid set returns to its initial position, then the number of turns is recalculated. 6. Enter the initial angle. This is the initial value of the joint, as represented in the design configuration. For example, if a circular actuator is designed with the rod half out and its initial value is 40°, TopSolid considers that the rod is out by 40°, if the maximum limit of the rod is 40°, the rod cannot turn the other way any further. 7. Check Limits to be able to fill in the minimum and maximum angles.

8. Viscous Friction can be taken into account by checking this option. When the limits are filled in, limit stops are put in place during the manual displacement of the rigid sets. These limits have no impact when a scenario is used.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Cylindrical Joint

This command allows to create a cylindrical joint between 2 rigid groups.

Creation stages / Use: Click the icon or select the Mechanism > Cylindrical joint... command from the drop-down menu. 1. 2. 3. 4.

Select the first rigid group. Select the second rigid group. Select the rotation axis. Select a center point. This optional possibility may be useful in dynamics. The point chosen for greater calculating precision will be projected to the axis selected previously. 5. Enter the initial distance. This is the initial value of the joint, as represented in the design configuration. For example, if an actuator is designed with the rod half out and its initial value is 40mm, TopSolid considers that the rod is out by 40mm. If the maximum limit of the rod is 40mm, the rod cannot go in any further. 6. Check Limits to be able to fill in the minimum and maximum distances. 7. Friction can be taken into account by checking this option.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Spherical joint

This command allows to create a spherical joint between 2 rigid groups.

Creation stages / Use: Click the icon or select the Mechanism > Spherical... command from the drop-down menu. 1. 2. 3. 4.

Select the first rigid group. Select the second rigid group. Select the spherical point. Validate.

Available options: Limits: Allows to define an angular stop on a spherical joint. 1. Select the first rotation axis direction (first rigid group). 2. Select the second rotation axis direction (second rigid group). 3. Enter the maximum tilt angle between the 2 directions.

Friction: Viscous Friction can be taken into account by checking this option.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Planar Joint

This command allows to create a planar joint between 2 rigid groups.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Planar... command from the drop-down menu. 1. Select the first rigid group. 2. Select the second rigid group. 3. Select the sliding plane.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Point on Axis Joint

This command allows to create a point on axis joint between 2 rigid groups.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Point on axis... command from the drop-down menu. 1. 2. 3. 4.

Select the rigid group of the point. Select the rigid group of the axis. Select the point. Select the axis.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Axis on plane joint

This command allows to create an axis on plane joint between two rigid groups.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Axis on plane ... command from the drop-down menu. 1. 2. 3. 4.

Select the rigid group of the axis. Select the rigid group of the plane. Select the axis. Select the plane.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Point on Plane Joint

This command allows to create a point on plane joint between 2 rigid groups.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Point on plane... command from the drop-down menu. 1. 2. 3. 4.

Select the rigid group of the point. Select the rigid group of the plane. Select the point. Select the plane. The arrow reverses the contact side of the point on the plane. 5. Check or uncheck Unilateral. This option allows to have a nonpermanent contact between the point and the plane, from the side chosen when the plane was selected. If this option is checked, you will be able to move the point of the rigid group until it touches the plane of the rigid group. The rigid groups can be separated, but can't intersect themselves. 6. Friction can be taken into account by checking this option.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Sphere on plane joint

This command allows to create a sphere on plane joint between 2 rigid groups.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Sphere on plane... command from the drop-down menu. 1. Select the rigid group of the sphere. 2. Select the rigid group of the plane. 3. Select the center of the sphere, either by clicking the center point, or by clicking the sphere. 4. Enter the diameter of the sphere. 5. Select the plane. The arrow reverses the contact side of the sphere on the plane. 6. Check or uncheck Unileral. This option allows to have a nonpermanent contact between the sphere and the plane, from the side chosen when the plane was selected. If this option is checked, you will be able to move the sphere rigid group until it touches the plane rigid group. The rigid groups can be separated, but can't intersect themselves. 7. Check or uncheck No slipping. When No slide is checked, the sphere rolls in relation to the plane. Otherwise, it slides on the plane.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Sphere on sphere joint

This command allows to create a sphere on sphere joint between 2 rigid groups.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Sphere on sphere... command from the drop-down menu. 1. Select the first rigid group. 2. Select the second rigid group. 3. Select the center of the sphere of the first rigid group, either by clicking the center point, or by clicking the sphere. 4. Enter the diameter of the sphere of the first rigid group. 5. Select the center of the sphere of the second rigid group, either by clicking the center point, either by clicking the sphere. 6. Enter the diameter of the sphere of the second rigid group. 7. Check or uncheck Unilateral This option allows to have a nonpermanent contact between the 2 spheres, from the side chosen when the plane was selected. If this option is checked, you will be able to move the sphere rigid group until it touches the other one. The rigid groups can be separated, but can't intersect themselves. 8. Check or uncheck No slipping. When No slide is checked, the sphere rolls in relation to the other sphere. Otherwise, it slides.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Sphere on shape joint

This command allows to create a sphere on shape joint between 2 rigid groups.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Sphere on shape... command from the drop-down menu. 1. Select the rigid group of the sphere. 2. Select the rigid group of the shape. 3. Select the center of the sphere, either by clicking on the center point, or clicking the sphere. 4. Enter the diameter of the sphere. 5. Select the shape. The arrow reverses the contact side of the point on the plane. 6. Check or uncheck Unilateral. This option allows to have a nonpermanent contact between the sphere and the shape, from the side chosen when the plane was selected. If this option is checked, you will be able to move the sphere rigid group until it touches the shape rigid group. The rigid groups can be separated, but can't intersect themselves. 7. Check or uncheck No slipping. When No slide is checked, the sphere rolls in relation to the shape. Otherwise, it slides on the shape.

This joint works only when the contact between the sphere and the shape is a point contact. For example, it will not work between a sphere and a cone.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Screw Joint

This command creates a screw joint.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Screw... command from the drop-down menu. 1. 2. 3. 4. 5.

Select the first rigid group. Select the second rigid group. Select the rotation axis. Enter the thread. Check or uncheck for a left-hand thread.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information: The different rigid groups must also have a clindrical joint for the screw joint to work.

Rack and Pinion Joint

This command creates a rack and pinion joint.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Rack and pinion... command from the drop-down menu. 1. 2. 3. 4. 5.

Select the rigid group of the rack. Select the rigid group of the pinion. Select the direction of the rack. Click the arrow to reverse the direction of displacement. Select the axis of the pinion. Click the arrow to reverse the direction of rotation. Enter the primitive diameter of the pinion.

The direction displacement of the rack and the direction of rotation of the pinion must be coherent.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

The different rigid groups must also have a pivot and prismatic joint in order for the rack and pinion joint to work.

Gear Joint

This command creates a gear joint.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Gear... command from the dropdown menu. 1. 2. 3. 4.

Select the first rigid group. Select the second rigid group. Select the axis of the first rigid group. Click the arrow to reverse the direction of rotation. Select the axis of the second rigid group. Click the arrow to reverse the direction of rotation. 5. Enter the ratio.

The directions of rotation must be coherent.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information: The axes of the gear joint must not be coincident (they can be concurring, parallel or distinct). The different rigid groups must also have a pivot joint in order for the gear joint to work.

Belt Joint Links/Videos:

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This command allows you to create a belt joint between several pulleys.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Belt... command from the dropdown menu. 1. Enter the thickness of the belt. This thickness is important when the internal face and external face of the belt are in contact with the different pulleys. 2. Select the plane in which the belt is working (the axes of the pulleys must be perpendicular to this plane). 3. Indicate the number of pulleys. 4. Select the first rigid group. 5. Select the axis of the first rigid group. Click the arrow to reverse the direction of rotation. 6. Enter the diameter. 7. Do the same for the other pulleys.

The directions of rotation must be coherent.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information: The axes of the belt joint must not be coincident (they can be concurring, parallel or distinct). The different rigid groups must also have a pivot joint in order for the belt joint to work.

Slot and pin joint

This command allows to create a slot and pin joint between 2 rigid groups.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Slot and pin... command from the drop-down menu. 1. Select the first rigid group. 2. Select the second rigid group. 3. Select the direction of the slot. This direction indicates the positive value of the movement of the 2nd rigid group in relation to the 1st. 4. Select the axis. The part in the slot may turn in relation to this axis. When the limits are filled in, limit stops are put in place during the manual displacement of the rigid sets. These limits have no impact when a scenario is used.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

The 2 selected axes cannot be parallel.

Point on Profile Joint

This command allows to create a point on profile joint between 2 rigid groups. The rigid group of the point will follow the trajectory provided by the profile.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Point on profile... command from the drop-down menu. 1. 2. 3. 4. 5.

Select the rigid group of the point. Select the rigid group of the profile. Select the point. Select the profile. The Maintain tangent option allows you to always have the point rigid group tangent to the profile. For example, a cart (point rigid group) must follow a curve (profile rigid group) by keeping the tangency with this curve. To have the same result without this option, 2 points are needed on the profile.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Profile on Plane Joint

This command creates a profile on plane between 2 rigid sets.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Profile on plane... command from the drop-down menu. 1. 2. 3. 4.

Select the rigid group of the profile. Select the rigid group of the plane. Select the profile. Select the plane. The arrow reverses the contact side of the profile on plane. 5. Check or uncheck Unilateral. This option allows to have a nonpermanent contact between the profile and the plane, from the side chosen when the shape was selected. If this option is checked, you will be able to move the profile rigid group until it touches the plane rigid group. The rigid groups can be separated, but can't intersect themselves. 6. Check or uncheck No slipping. When No slide is checked, the profile rolls in relation to the plane. Otherwise, it slides on the plane.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Profile on profile

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This command allows to create a profile on profile joint between 2 rigid groups. For example, an ejector can move vertically until there is a contact with the mold, then slide along the wall.

Creation stages / Use: Click the icon or select the Mechanism > Other joints > Profile on profile... command from the drop-down menu. 1. Select the first rigid group. 2. Select the second rigid group. 3. Select the plane in which the 2 profiles are in contact on the same point. If profiles are not in the same plane, there will be projected following the normal direction to this plane. 4. Select the profile of the first rigid group. 5. Select the profile of the second rigid group. 6. Check or uncheck Unilateral. This option allows you to have a non-permanent contact between the 2 profiles. When 2 profiles are moved and touched together, the contact is done. It will be possible to separate profiles but not cross them. 7. Check or uncheck No slipping. This option, when it is checked, allows you to move a profile on another in case of contact, if other joints allow it. If the option is unchecked, the second profile will not move in case of displacement of the first one. 8. Validate by clicking .

The profile orientation should be such that the orange circle is into the matter. A line of a profile parallel to a line of another profile and in contact are considered as a contact point. The joint manages a contact between a non-collinear profile (no fillets between 2 lines) only if there is only one contact point at any time. The joint is compatible with opened profile, but all segments used in the joint must be created.

This joint can not be used when 2 profiles have 2 contact points like for example a cylinder in a "V".The trick is to cut the "V" in 2 parts, each profile of the "V" will have only one contact with the circle, the joint will be "unilateral".

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Point on shape Links/Videos:

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This command allows to create a point on shape joint between 2 rigid groups.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Point on shape... command from the drop-down menu. 1. 2. 3. 4. 5.

Select the rigid group of the point. Select the rigid group of the shape. Select the point. Select the shape. Check or uncheck Unilateral. This option allows to have a nonpermanent contact between the point and the shape, from the side chosen when the shape was selected. If this option is checked, you will be able to move the point rigid group until it touches the shape rigid group. The rigid groups can be separated, but can't intersect themselves.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Plane on shape

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This command allows to create a plane on shape joint between 2 rigid groups.

Creation stages / Use: Click the icon or select the Mechanism > Other joints > Plane on shape... command from the drop-down menu. 1. Select the rigid group of the plane. 2. Select the rigid group of the shape. 3. Select the plane. The arrow reverses the contact side of the plane on the shape. 4. Select the shape. 5. Check or uncheck Unilateral. This option allows to have a nonpermanent contact between the plane and the shape, from the side chosen when the plane was selected. If this option is checked, you will be able to move the plane rigid group until it touches the shape rigid group. The rigid groups can be separated, but can't intersect themselves. 6. Check or uncheck No slipping. When No slide is checked, the plane "rolls" in relation to the shape. Otherwise, it slides on the shape.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

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Smooth shape on shape joint

This command allows to manage the "shape-on-shape" punctual unilateral contact, in particular where one of the two shapes is smooth where contact occurs. This joint is useful with Mold mechanism regarding angular pins.

Creation stages / Use: Click the icon or select the Mechanism > Other joints > Smooth shape on shape... command from the drop-down menu. 1. 2. 3. 4.

Select the smooth shape rigid group. Select the other shape rigid group. Select the smooth shape offset shape. Select the offset distance between the smooth shape and the offset shape. 5. Select the shape of the other rigid group.

It must be possible to provide a parallel shape inside the smooth shape so that all points of this parallel shape at a certain distance is equal to the surface of the initial smooth shape. This is the offset distance. This offset distance must be as greater as possible so that the offset shape is never in contact with the other shape during calculation iterations. This offset shape is required to the displacements calculations:

Let d the offset distance specified between the smooth shape and the offset shape. During the calculation iterations, if d' is lower than d then TopSolid knows there is collision and it will move the grey shape in the same direction as the red vector until d' is equal to d.

Dimensions of offset shape must not exceed contact area while the movement of shapes. Otherwise there may be a loss of performance during shapes displacement because this shape move for each calculation iterations.

If the contact area between the pin and the other shape is equal to 30mm while shapes displacement, then the offset shape must be created with this same height.

Available options: Unilateral: This option allows to have a non-permanent contact between the smooth shape and the other shape. If this option is checked, you will be able to move the smooth shape rigid group until it touches the other shape rigid group. The rigid groups can be separated, but can't intersect themselves.

No slipping: When No slipping is checked, the smooth shape rolls on the other shape. Otherwise, it slides on it.

The Smooth Shape on Shape joint between the pink part and the blue part enables the blue part to move circularly

Normal to shape

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This command allows you to create a joint so that a part is normal to another.

Creation stages / Use: Click the

icon or select Mechanism > Normal to Shape... from the drop-down menu.

Example: The orange part must be normal to the blue part.

1. Select the rigid group of the axis (the orange part in the example below). 2. Select the rigid group of the shape (the blue part). 3. Select a point on the axis, outside the shape. This point must be on the axis of the orange part and will be projected onto the first face encountered of the blue part, depending on the direction defined in the following box. 4. Select the direction of the axis to the shape. In our case, the direction goes toward the bottom, but if the orange part is in a crown, the direction that defines the intersection point must be given. The orange part will be normal to blue in this point. 5. Select the shape (the blue part). 6. Validate.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Orientation

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This command allows you to create an orientation joint between 2 rigid groups.

Creation stages / Use: Click the icon or select the Mechanism > Other joints > Orientation... from the drop-down menu. 1. 2. 3. 4. 5.

Select the first rigid group. Select the second rigid group. Select the first direction. Select the second direction. Validate by clicking .

There is no angle to enter. It is deduced from the 2 chosen directions.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Equidistance joint

This command allows to link together three rigid groups by making sure that the distance between a point attached to the first rigid group and a point attached to the second rigid group remains the same as the distance between the point attached to the first rigid group and a point attached to the third rigid group.

Creation stages / Use: Click the icon or select the Mechanism > Other Joints > Equidistance... command from the drop-down menu. 1. 2. 3. 4. 5. 6.

Select the center rigid group. Select the second rigid group. Select the third rigid group. Select the center point (link with the center rigid group). Select the second point (link with the second rigid group). Select the third point (link with the third rigid group).

It is necessary to use an equidistant joint per pair of rigid groups to move symmetrically (i.e. one for a symmetrical vise and two for a three-jaw chuck).

The selected points can't be the same or combined. (neither during the selection nor during their movement). in the case of a three-jaw chuck, it is recommended to select a point on the outside edge of the jaw.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information: Example of equidistant joints (in yellow).

Rigid Joint

This command allows to create a rigid joint between 2 rigid groups. This joint allows you to make two rigid groups interdependent without merging them.

Creation stages / Use: Click the icon or select Mechanism > Other joints > Rigid... command from the drop-down menu. 1. Select the first rigid group. 2. Select the second rigid group.

To test the joint, either the sub-set can be inserted in an assembly, or a configuration can be created or reused.

Modifications / Additional information:

Constrained configuration

When the rigid groups and the joints are defined, there is a mechanism in due form, and when the assembly is included in an assembly of a higher level, the articulations can be activated when positioned in relation to the other parts of this assembly. However, it can also be useful to visualize certain key positions of the mechanism locally, without having to include it in another assembly. This is done using the configuration notion. A configuration of the mechanism is actually a position of the mechanism which is compatible with the constraints of its joints. The system automatically creates a configuration which cannot be deleted and which corresponds to the position of the parts at the end of the modeling stage, the configuration of design. Other configurations can be created, including, for example, configurations defined by positioning constraints by virtue of the 'Constrained configuration' command, as if the mechanism had been included in an assembly of a higher level: the rigid groups are displaced taking into account the constraints of the joints in order to meet the positioning constraints which can be creating using different commands from the Mechanism menu (in a similar way to the constrained positioning used during the modeling of an assembly by reassembly). One of the different existing configurations is called the current configuration , its name displayed in the corresponding drop down list of the menu, and it can be changed by selecting another configuration. When working in the Mechanism stage, the parts are in their position corresponding to the current configuration.

Creation stages / Use:

Click the icon or select the Mechanism > Constrained Configuration... command from the drop-down menu.

Modifications / Additional information: Configuration can be edited, renamed or deleted using the popup menu on the intended configuration in the Configurations sub-folder in the Mechanism folder in the entities tree. The Design configuration default configuration cannot be deleted or renamed.

Point on surface

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This command allows you to constraint a point of the part to include regarding a surface of the destination geometry.

Creation stages / Use:

Click the icon or select the Assembly > Other constraints > Point on surface... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Point on surface... command from the drop-down menu.

1. Select a point on the geometry to be included. 2. Select a surface on the destination geometry. 3 E t

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Axis on surface

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This command constrains an axis of the part to be included in relation to a surface of the destination geometry.

Creation stages / Use:

Click the icon or select the Assembly > Other constrains > Axis on surface... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. Select in this case the Mechanism > Other constrains > Axis on surface... command from the drop-down menu.

1. Select an axis on the geometry to be included. 2. Select a surface on the destination geometry. 3. Enter the offset.

Plane on surface

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This command constrains a plane of the part to be included in relation to a surface of the destination geometry.

Creation stages / Use:

Click the icon or select the Assembly > Other constraints > Plane on surface... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Plane on surface... command from the drop-down menu.

1. Select a plane on the geometry to be included. 2. Select a surface on the destination geometry. 3. Enter the offset.

Surface on point

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This command constrains the surface be included in relation to a point of the destination geometry.

Creation stages / Use:

Click the icon or select the Assembly > Other constraints > Surface on point... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Surface on point... command from the drop-down menu.

1. Select a surface on the geometry to be included. 2. Select a point on the destination geometry. 3 E t

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ff t

Surface on axis

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This command constrains the surface be included in relation to an axis of the destination geometry.

Creation stages / Use:

Click the icon or select the Assembly > Other constraints > Surface on axis... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Surface on axis... command from the drop-down menu.

1. Select a surface on the geometry to be included. 2. Select an axis on the destination geometry. 3 E

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ff

Surface on plane

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This command constrains the surface be included in relation to a plane of the destination geometry.

Creation stages / Use:

Click the icon or select the Assembly > Other constraints > Surface on plane... command from the drop-down menu. It is also possible to add constraints in a configuration of a mechanism. In this case, select the Mechanism > Other constraints > Surface on plane... command from the drop-down menu.

1. Select a surface on the geometry to be included. 2. Select a plane on the destination geometry. 3. Enter the offset.

Configuration Collision

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This command allows to

Creation stages / Use: Click the icon or select the Mechanism > Configuration Collision... command from the drop-down menu. 1. Select the collision updating mode when the Analysis stage of the document Checked: the collisions analysis operation is automatically updated as soon as the Analysis stage of the document becomes current. Unchecked: the collisions analysis operation is not automatically updated, it is necessary to click on the manual update icon (see below). Not managed: the drillings collisions operation is not computed.

1. 2. Choose the configuration to analyze. 3. Choose the representation to analyze.

4. Define the analysis options (see Available Options paragraph below). 5. Confirm with the button.

The collisions are saved in a sub folder (corresponding to the configuration's name) of the Mecanism > Collisions folder of the entities tree. For each analyzed configuration, A Collisions Management operation is created in the Analysis stage of the document.

Available options: Intersections: When 2 drillings are colliding, this option allows to highlight the collision with the creation of the intersection shape. When this option is unchecked, the collision is highlighted with a red cross at the collision location.

Threading-tapping: This option allows you to manage threadings/tappings. If a Ø8 screw is in a Ø8 tapped hole, there will be no collision (except if the screw is partially threaded and its non-threaded part is in the tapped hole). If the screw is bigger than the tapped hole, or if the option is unchecked, the collision will be detected and displayed.

Invalid if colliding: When this option is checked and one collision is detected, the document becomes invalid. In such case, you should repair this invalidity, by moving one of the drillings for example, in order to be able to continue the design of the document.

Modifications / Additional information: If you want to modify the analysis options you can run the command again or edit the Drillings Collisions Management operation of the operations tree when the Analysis stage of the document is activated.

Gravity Links/Videos:

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This command allows you to manage the direction and the value of the weight during dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Gravity... command from the drop-down menu. 1. Select the direction of the weight. 2. Enter the intensity of its acceleration.

The weight is global to the document and cannot be managed by a force driving task.

Modifications / Additional information: The force may be edited, renamed, deleted, activated or deactivated by using the popup menu in the Forces sub-folder in the Mechanisms folder in the entities tree.

To use this function in a dynamic simulation, the part must have a mass, a mass center, and moments of inertia. These parameters must also be checked in the assembly physical properties

Linear spring

This command adds a stress by simulating a linear spring between 2 rigid groups during the dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Linear spring... command from the drop-down menu. 1. 2. 3. 4.

Select the first rigid group. Select the second rigid group. Select the attachment point of the spring on the first rigid group. Select the attachment point of the spring on the second rigid group. 5. Enter the length of the unloaded spring or the force of the spring in the initial position of the mechanism. 6. Enter the stiffness of the spring.

The rest length corresponds to the vacuum length of the spring. Depending on this length, we can therefore have a traction or compression spring.

Available Options: Inheritable: This option allows you to operate this force in the higher level assembly. It is enabled by default.

Modifications / Additional information: The spring can be edited, renamed, deleted, activated or deactivated by using the popup menu in the Forces sub-folder of the Mechanisms folder of the entities tree.

To use this function in a dynamic simulation, the part must have a mass, a mass center, and moments of inertia. These parameters must also be checked in the assembly physical properties.

Angular spring

This command adds stress by simulating a torsion spring between 2 rigid groups during the dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Angular spring... command from the drop-down menu. 1. 2. 3. 4. 5.

Select the first rigid group. Select the second rigid group. Select the rotation axis. Enter the initial angle or the initial torque of the spring. Enter the stiffness of the spring.

The initial angle (or before working) corresponds to the unloaded angle of the spring.

Available Options: Multi-turns angle: Check this box to manage an angular variation higher than 360°. Inheritable: This option allows you to operate this force in the higher level assembly. It is enabled by default.

Modifications / Additional information: The spring can be edited, renamed, deleted, activated or deactivated by using the popup menu in the Forces sub-folder of the Mechanisms folder of the entities tree.

To use this function in a dynamic simulation, the part must have a mass, a mass center, and moments of inertia. These parameters must also be checked in the assembly physical properties.

Punctual damper Links/Videos:

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This command allows you to add a load simulating a punctual damping between 2 rigid groups during dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Punctual damper... command from the drop-down menu. 1. 2. 3. 4.

Select the first rigid group. Select the second rigid group. Select the damping point on the first rigid group. Enter the damping coefficient of the damper.

Available Options: Inheritable: This option allows you to operate this force in the higher level assembly. It is enabled by default.

Modifications / Additional information: The damper can be edited, renamed, deleted, activated or deactivated by using the popup menu in the Forces sub-folder in the Mechanisms folder of the entities tree.

To use this function in a dynamic simulation, the part must have a mass, a mass center, and moments of inertia. These parameters must also be checked in the assembl ph sical properties

Linear damper

This command adds strain by simulating a linear damper between 2 rigid groups during dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Linear damper... command from the drop-down menu. 1. 2. 3. 4.

Select the first rigid group. Select the second rigid group. Select the attachment point for the damper on the first rigid group. Select the attachment point for the damper on the second rigid group. 5. Enter the damping coefficient of the damper.

The damper can be used in traction or in compression.

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Available Options: Inheritable: This option allows you to operate this force in the higher level assembly. It is enabled by default.

Modifications / Additional information: The damper can be edited, renamed, deleted, activated or deactivated by using the popup menu in the Forces sub-folder of the

Mechanisms folder of the entities tree.

To use this function in a dynamic simulation, the part must have a mass, a mass center, and moments of inertia. These parameters must also be checked in the assembly physical properties

Angular damper

This command adds stress by simulating an angular damper between 2 rigid groups during the dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Angular damper... command from the drop-down menu. 1. 2. 3. 4.

Select the first rigid group. Select the second rigid group. Select the direction of the rotational axis of the damper. Enter the damping coefficient.

Available Options: Inheritable: This option allows you to operate this force in the higher level assembly. It is enabled by default.

Modifications / Additional information: The damper can be edited, renamed, deleted, activated or deactivated by using the popup menu in the Forces sub-folder in the Mechanisms folder of the entities tree.

To use this function in a dynamic simulation, the part must have a mass, a mass center, and moments of inertia. These parameters must also be checked in the assembly physical properties

Punctual force

This command adds a strain by simulating a punctual force on a rigid group during the dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Punctual force... command from the drop-down menu. 1. Select the rigid group on which the force will be applied. 2. Select the contact point of the punctual force. 3. Select the type of direction: Fixed: The direction chosen does not change based on the rigid group. It is defined based on the absolute frame. Joined to the rigid group: The direction chosen changes based on the rigid group. It is defined based on a frame of the rigid group. 4. Select the direction of the punctual force. 5. Enter the intensity of the force.

The punctual force may be used with different values in a force driving task.

Modifications / Additional information: The force may be edited, renamed, deleted, activated or deactivated by using the popup menu in the Forces sub-folder in the Mechanisms folder in the entities tree.

To use this function in a dynamic simulation, the part must have a mass, a mass center, and moments of inertia. These parameters must also be checked i th bl h i l ti

Torque force

This command adds stress simulating a torque force on a rigid group during dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Torque force... command from the drop-down menu. 1. Select the rigid group on which the force will be applied. 2. Select the type of direction: Fixed: The direction chosen does not change based on the rigid group. It is defined based on the absolute frame. Joined to the rigid group: The direction chosen changes based on the rigid group. It is defined based on a frame of the rigid group. 3. Select the direction of the torque force. 4. Enter the intensity of the force.

The torque force may be used with different values in a force driving task.

Modifications / Additional information: The force may be edited, renamed, deleted, activated or deactivated by using the popup menu in the Forces sub-folder in the Mechanisms folder in the entities tree.

To use this function in a dynamic simulation, the part must have a mass, a mass center, and moments of inertia. These parameters must also be checked in the assembly physical properties

Translation velocity

This command simulates an initial translation velocity on a rigid group during dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Translation Velocity... from the drop-down menu. 1. Select the rigid group to which the velocity will be applied. 2. Select the direction of the velocity. 3. Enter the value of the velocity.

The translation velocity can be used in the Initial velocity drop down window of the dynamic simulation.

Modifications / Additional information: The velocity can be edited, renamed, deleted, activated or deactivated using the popup menu in the Velocities sub-folder in the Mechanisms folder in the entities tree.

Rotation velocity

This command simulates an initial rotation velocity on a rigid group during dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Rotation Velocity... from the drop-down menu. 1. Select the rigid group to which the velocity will be applied. 2. Select the rotation velocity axis. 3. Enter the value of the velocity.

The rotation velocity can be used in the Initial velocity drop down window of the dynamic simulation.

Modifications / Additional information: The velocity can be edited, renamed, deleted, activated or deactivated using the popup menu in the Velocities sub-folder in the Mechanisms folder in the entities tree.

Joints driving task

This command defines the different joints driving tasks inserted in the scenario. Joints can be added in a task, a task is able to manage one or more tasks.

Creation stages / Use: Click the 1. 2. 3. 4.

icon or select Simulation > Joint Driving Task... from the drop-down menu.

Enter a new task name if required. Select the joint to drive from the drop down list, and click Add joint button. Enter the times and the values of desired movements by clicking in the relevant cells. Select the type of interpolation: 1. Constant velocity: The displacement movement is linear, the start and stop may be sudden. At each moment of the defined gap, the displacement value is strict. This interpolation is not realist. The acceleration is infinite when starting to have immediately the correct speed. 2. Constant acceleration: The acceleration is maximal, the velocity changes. It is often the case with small engines. 3. Variable acceleration: The movement is smoother at the start with a cushioned stop. It is often the case with big engines. Constant velocity

Constant acceleration

Variable acceleration

Each task is in relative time and can therefore start at 0 seconds. The time delay occurs at the scenario level. The benefit of this method is to be able to prepare driving sections and start them at the desired time. For example, the one-second movement of a part every 5 seconds on a conveyor in continuous operation. A first task will be the continuous movement of the conveyor, the 2nd task will be the movement of the part from 0 to 1 second. The start of the 2nd task will occur at 5 seconds in the scenario.

Only some joints can be driven. Non driven joints do not appear in the drop-down list. Driven joints are: The prismatic (length drive)

The pivot (angle drive) The cylindrical (length drive) The point on profile (length drive)

Forces driving task

This command defines the different force driving tasks inserted in the scenario. Each force (punctual, angular) may be added to a task, a task can contain one or more forces.

Creation stages / Use: Click the icon or select Simulation > Force Driving Task... from the drop-down menu. 1. Enter a new task name if required. 2. Select the force to drive in the drop-down list, and click on Add force button. 3. Enter the desired time and the intensities of the forces by clicking in the relevant cells. 4. Select the type of interpolation: 1. Constant: The force is constant during all the period of the time sequence. 2. Linear: The force is linear progressive and linear, it changes based on the time to arrive at the defined intensity. Constant interpolation

Linear interpolation

Each task is in relative time and can therefore start at 0 seconds. The time delay occurs at the scenario level. The benefit of this method is to be able to prepare driving sections and start them at the desired time. For example, a "stamp" task has been created. It may be implemented in the scenario at t=10 to start at the 10th second of the scenario.

Only forces can be driven. The weight, springs, dampers and velocities do not appear in the drop-down list.

Rigid group driving task

Links/Videos:

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This command allows to define a rigid group driving task without having defined all other joints. Displacements will be translations and rotations.

Creation stages / Use: Click the icon or select the Simulation > Rigid group driving task... command from the dropdown menu. 1. Enter a name, it will be proposed in the scenario. 2. Select a kind of driving (see explanations below). 3. Select a rigid group to drive and its driving frame.(All displacement values of the rigid group are regarding this frame). 4. Enter times, translation and rotation values regarding the different axes by clicking in corresponding cells. 5. Validate by clicking .

The vector defined by the X, Y and Z rotation is used as rotation axis, the norm of this vector is used as rotation angle around this axis. The task must be compatible with existing joints. For example, if a rigid group has a planar joint with another, the translation along Z will not be possible. If the rigid group has a rigid joint, no movement will be possible.

Available Options: Driving frame The driving frame is linked with the part. It is defined according to the part position in the design configuration. Consequently, if a part has a different position/orientation in another configuration, the relative position between the part and its driving frame is not the same. The resulting movement of the task may be different according to the current configuration.

It is possible to select a frame by clicking it directly in the graphic workspace.

Circular: Allows to create a circular displacement by adding a displacement and a rotation.

Bellow is an example with the Translation Y=20mm and a Rotation Z=90°:

Without Circular option

With Circular option

Driving: (example with the table below) The green part moves on a plate with the following task values: The task is added two times to the scenario with a waiting time of 1 second between the two tasks. Time 0s 2s 4s 6s

Translation X 0mm 50mm 0mm 0mm

Translation Y 0mm 0mm 20mm 30mm

Translation Z 0mm 0mm 0mm 0mm

Rotation X 0° 0° 0° 0°

Rotation Y 0° 0° 0° 0°

Rotation Z 0° 0° 90° 0°

Circular

Absolute: Entered values are regarding the initial position of the time 0s.At the end of the first task, the part comes back to the departure point and start the second task. A value of 0 indicates that the part comes back to the departure point of the direction.

Relative: The first task is done like with absolute mode, but after the second task continues where the first task has stopped. A value of 0 indicates that the part comes back to the departure point of the direction.

Incremental: Values are incremental regarding the previous position, the second task begins where the first has stopped. The position and the orientation of the part is kept. A value of 0 indicates that the part stays on the previous point of this direction.

It is recommended to use the incremental mode instead of the absolute one. In fact, with the absolute mode, you have to indicate the final position for each step, which can be complicate if the group has turned.

Visibility Change Task Links/Videos:

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This command allows to define a task to hide or show rigid groups.

Creation stages / Use: Click the icon or select Simulation > Visibility Change Task... from the drop-down menu. 1. 2. 3. 4.

Enter a name for this task. Select the action to perform (Hide or Show). Enter the rigid groups. Validate with the button.

To hide or show rigid groups during simulation, 2 tasks must be created, one to hide and the other to show. The visibility change task lasts as long as there are no other visibility change tasks for the same rigid groups. Just like joint driving tasks, visibility change tasks must be integrated with the simulation scenario.

Grip Change Task Links/Videos:

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This task allows you to "capture" and "release" rigid groups in the scenario.

Creation stages / Use: Click the icon or select Simulation > Grip Change Task... from the drop-down menu. 1. 2. 3. 4. 5.

Enter a name for this task. Select the action to perform (Take or Drop). Enter the taking rigid group. Select taken or dropped rigid groups. Validate with the button.

To take or drop rigid groups during simulation, 2 tasks must be created, one to take and the other to drop. The grip change task lasts for as long as there are no other contrary grip change tasks for the same rigid groups. Just like joint driving tasks, grip change tasks must be integrated into the simulation scenario.

Scenario This command allows you to create a scenario in which several tasks can be inserted and by defining the moment when these tasks must be launched.

Creation stages / Use: Click the icon or select the Simulation > Scenario... command from the drop-down list. 1. Enter the name for the scenario. 2. Drag the tasks from the left column to the timing chart. You can move tasks by dragging them with the mouse in the track and from one track to another. 3. Validate. Click the image below for further information.

This command creates a Scenarios sub-folder in the Mechanisms folder in the

entity tree.

Modifications / Additional information: For all modifications regarding the scenario, use the contextual menu from the Scenarios sub-folder in the Mechanisms folder in the entity tree. To add tasks, drop the relative tasks in the desired scenario. Using the popup menu, rename, edit or delete a scenario or tasks To modify the start date of a task, expand the scenario by clicking "+" and edit the task with the popup menu or use the Modify Start Instant popup command directly from the timing chart.

The joint driver tasks and the force driver tasks can be grouped together in the same scenario. In this case, only the dynamic simulation is possible. Grip change tasks, Visibility change tasks and rigid group driving tasks can also be used in the scenario.

The scenario still depends on the assembly in modeling mode.

Kinematics simulation

This command calculates the simulation before viewing.

Creation stages / Use: Click the icon or select the Simulation > Kinematics simulation.. command from the drop-down menu. 1. Check or uncheck Auto refresh. The slightest modification (joints, tasks, etc.) restarts the simulation calculation, which can slow things down considerably. 2. Select the starting configuration in the drop down list. Several configurations may be available, with different part positions. 3. Select the scenario in the drop-down list. 4. Enter the number The trajectory points are pre-calculated. The greater the number of positions, the more accurate the trajectory. Conversely, too few positions will create a segmented trajectory. 5. Enter the calculation pitch per position. When the displacement is too large in relation to the number of positions calculated, the calculation can be fine-tuned by modifying the pitch. It represents the interval between two position calculations of the mechanism. The lower the calculation, the more accurate the trajectories. 6. Check the Viewer option to be able to play the simulation when exporting the assembly as visualization format, or in case of opening it with TopSolid'Pdm Explorer. 7. Validate.

Increasing the number of positions per second and/or the steps by position gives a more precise result but on the other hand it takes more time to calculate.

For reasons of performance, you are advised not to activate Auto refresh. If this option is checked, editing, deleting, adding a joint or task causes a new simulation calculation. This calculation time may be long, depending on the complexity of the assembly and the accuracy of the calculation required.

Available Options: Collisions: Check this option in order to manage them. 1. Select the type of representation on which to verify the collisions. 2. Select the parts. 3. If you check Invalid if Collision, the simulation will be invalid when it is recalculated, if there are collisions. Otherwise, you will only know if there are collisions when viewing the simulation.

The calculation of collisions is very intensive on system resources. For this reason, it is recommended that you only select parts that can enter into collision. In a mechanism, only collisions between rigid groups are detected. If there are collisions between parts of a same rigid group, they will not be calculated. They will have to be detecte in static mode (Design stage instead of Mechanism stage).

Modifications / Additional information: Using the popup menu, Auto refresh can be edited, deleted and checked or unchecked.

When the simulation is not updated, it is colored cyan in the entities tree. It must be refreshed (popup menu) before using.

The force driving tasks are not taken into account in the scenario for

the Kinematics simulation. CAUTION: The results of the simulations are given for your information and can be tainted with errors (for example, because it is outside the validation domain of the achieved approximations). Critical mechanisms must always be verified with another software (it is probably good that both give the same result). Furthermore, even if the result is exact, perhaps the simplifications achieved once the mechanism has been modeled are not verified in reality (friction, tolerance of parts, ...), therefore the final product must still be tested in an actual condition (verily extreme) before making it available to the user without risk.

Dynamics Simulation

This command calculates the simulation before viewing.

Creation stages / Use: Click the icon or select the Simulation > Dynamic simulation.. command from the drop-down menu. 1. Check or uncheck Auto refresh. The slightest modification (joints, tasks, forces, dampers, velocity, etc.) restarts the calculation of the simulation, which can slow things down considerably. 2. Select the start configuration in the drop down list. Several configurations may be available, with different part positions. 3. In the drop down list, select the linear or angular start velocity, if it is defined. 4. Select the scenario in the drop-down list. 5. Enter the duration of the simulation. If a scenario has been selected, the duration of the simulation does not need to be entered, it is defined by the scenario. 6. Enter the number of positions calculated per second. The trajectory points are pre-calculated. The greater the number of positions, the more accurate the trajectory. Conversely, too few positions will create a segmented trajectory. 7. Enter the calculation steps per position. When the displacement is too large in relation to the number of positions calculated, the calculation can be fine-tuned by modifying the pitch. It represents the interval between two position calculations of the mechanism. The lower the calculation, the more accurate the trajectories. 8. Enter the damping factor which provides a damper notion to the mechanism (frictions, energy loss...). Globally, the damping factor applies to the whole mechanism.

9. Check or uncheck Overconstrained. (please read the warning below). 10. Check or uncheck Unknown physical properties. If this option is unchecked, all parts must have a material and their physical properties activated (mass, ...) if not, the simulation will be invalid. If the option is checked, the simulation can be ran even if some parts have no mass, for example to create a static analysis when mass effects are negligible regarding the applied efforts or when movements are very slow. 11. Check the Viewer option to be able to play the simulation when exporting the assembly as visualization format, or in case of opening it with TopSolid'Pdm Explorer. 12. Validate.

Increasing the number of positions per second and/or the steps by position gives a more precise result but on the other hand it takes more time to calculate. For reasons of performance, you are advised not to activate Auto refresh. If this option is checked, editing, deleting, adding a joint or task causes a new simulation calculation. This calculation time may be long, depending on the complexity of the assembly and the accuracy of the calculation required.

Available Options: Collisions: Check this option in order to manage them. 1. Select the type of representation on which to verify the collisions. 2. Select the parts. 3. If you check Invalid if Collision, the simulation will be invalid when it is recalculated, if there are collisions. Otherwise, you will only know if there are collisions when viewing the simulation.

The calculation of collisions is very intensive on system resources. For this reason, it is recommended that you only

select parts that can enter into collision. In a mechanism, only collisions between rigid groups are detected. If there are collisions between parts of a same rigid group, they will not be calculated. They will have to be detecte in static mode (Design stage instead of Mechanism stage).

Modifications / Additional information: Using the popup menu, Auto refresh can be edited, deleted and checked or unchecked.

When the simulation is not updated, it is colored cyan in the entities tree. It must be refreshed (popup menu) before using.

The density, the center of density, moments of inertia must be attributed to the parts and assembly for the dynamic simulation to function. Overconstrained: Calculating an overconstrained simulation is prohibited by default. But you can calculate it by checking this option, recognizing that the result of this overconstrained simulation could be corrupt. It is highly recommended to modify the assembly to no longer be overconstrained. CAUTION: The results of the simulations are given for your information and can be tainted with errors (for example, because it is outside the validation domain of the achieved approximations). Critical mechanisms must always be verified with another software (it is probably good that both give the same result). Furthermore, even if the result is exact, perhaps the simplifications achieved once the mechanism has been modeled are not verified in reality (friction, tolerance of parts, ...), therefore the final product must still be tested in an actual condition (verily extreme) before making it available to the user without risk.

Play simulation

This command allows you to play the kinematic and dynamic simulations.

Creation stages / Use: Click the icon or select Simulation > Play Simulation... from the drop-down menu. 1. Select the simulation to visualize in the drop-down list. 2. Click Refresh if the button is not grayed out. The button is grayed out when the simulation is updated. Refreshes can also be run from the entities tree. 3. If a traveling is linked to the simulation it can be activated by checking the Traveling option. If several travelings exist, select the one to use by the simulation. 4. Roll over the cursor to view the simulation manually. Next Collision: Allows you to move the simulation forward to the next collision. This command is only available if collision search is on in kinematic or dynamic simulation. Fast backward: Plays the simulation in reverse, and quickly.

Play Backward: Plays the simulation in reverse.

Pause: Stops the simulation.

Play: Plays the simulation as defined.

Fast Forward: Plays the simulation quicker.

Loop Play: Loop plays the simulation, indefinitely, until another command is used.

To record the simulation, use the Record Simulation command.

Available Options: Settings: Speed: Select the slow motion value. 1 is normal speed; a higher value slows down simulation, a lower value accelerates it. Negative values are not allowed. Time: Enter the time. The simulation will start at the time indicated. For example if 2s is entered, the simulation will start directly at 2 seconds. The total time is given during the simulation creation. Stop at collision: By checking this option, the simulation will stop every time a collision is detected. This command is only available if collision search is on in kinematic or dynamic simulation.

If the Auto refresh mode is active on the kinematics or dynamic

simulations, the Update button is grayed out.

Collision detection is only available if the collision search is on in kinematic or dynamic simulation.

Record Simulation

Links/Videos:

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This command allows you to record a simulation.

Creation stages / Use: Click the icon or select Simulation > Record Simulation... from the drop-down menu. 1. Select the simulation to record. 2. Click Refresh if the button is not grayed out. The button is grayed out when the simulation is updated. Refreshes can also be run from the entities tree. 3. If a traveling is linked to the simulation it can be activated by checking the Traveling option. If several travelings exist, select the one to use by the simulation. 4. Enter the Start time. To start at the beginning of the simulation enter 0s (default proposed value). 5. Enter the End time. The proposed time is the total time of the scenario (default proposed value). 6. Enter the speed value. 1 is normal speed; a higher value slows down simulation, a lower value accelerates it. Negative values are not allowed. 7. Select the View to record. This choice is useful only if the document is displayed in several views. 8. Increase or decrease the frame in the graphic area by moving its vertexes. 9. Move the frame in the graphic area by moving its edges. 10. Validate by clicking on .

Available Options:

Video setup: 1. Enter the width and height of the video to record. These values are in pixels. 2. Enter the number of images per second. For videos, generally this value is between 25 and 30. If below, the video will be smaller, but jerky. 3. Enter the Key-frame rate if needed. 4. Select one of the installed codecs. The same codes are necessary on the station that will playback the video. If you use Uncompressed, a video of a couple of seconds will take several hundreds of Mb on your hard disk. 5. Modify the quality of the video by moving the cursor (grayed out for some codecs). An increase in quality increases the size of the video. 6. Configure the codec (for advanced users). Refer to the documentation of the codec). 7. Select the render mode from the drop down list. The render mode has a lot of influence on the calculation time and the generation of the video. 8. Select the background of the video. The screen background can be displayed in your video as well as a black or a white background. 9. Check Open Video to automatically open the video in the viewer defined in Windows after it has been created. 10. Validate. 11. Select a destination directory.

Several options improve video quality, but also increase size and calculation time. For example, a rendering with effects takes much lo to calculate because for 25 images/second, 25 times the effects mus calculated. The most frequent video playback problem is the absence of the cod the station trying to play the video.

Realistic rendering:

Antialiasing: this cursor allows to smooth elements edges.

Lighting accuracy: This cursor allows you to improve rendering qualit produced by extended lights and materials reflects. The improvement is increasing antialiasing, but it is much faster. This setting is only on if th that is likely to be adjusted (radiosity, sky light, extended lights).

Simplified Rendering: This option turns off all "costly" calculation tim lights, material with imperfect reflection, ...

Global Illumination: This option allows you to accurately simulate the scene itself, and no longer only the direct light from luminous sources. In a classic image calculation, an area that is not directly lit by light is b light re emitted by the walls and scene objects. Global illumination take avoids obtaining unlit areas. This option is particularly useful for implementation and architecture im

Global illumination accuracy: This option allows you to improve glob taking in account scene little details. Generally, default value (15%) is e

Recursion depth: Allows to setup of shadows depth, of reflection and r For example, if you have several mirrors reflecting themselves one othe will be reflected only in the first mirror. With a value of 2, this reflection mirror. This setting is only for beamed shadows.

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Simulation Configuration Links/Videos:

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This command allows you to create a configuration of a given simulation, at a t instant.

Creation stages / Use: Click the icon or select the Simulation > Simulation configuration... command from the drop-down menu. 1. Select a simulation from the drop down list. 2. Enter a time. 3. Validate.

When validating, a new configuration is created that can be used and modified from the Configurations folder in the entity tree.

Rigid Traveling

Links / Videos :

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This command allows to define a movement of a camera fixed on a rigid group. This traveling can be linked to a mechanism simulation.

Creation stages / Use: Click the 1. 2. 3. 4. 5.

icon or select the Simulation > Rigid Traveling... command from the drop-down menu.

Select the rigid group where to fix the camera. Select an hook point on this rigid group. Select the vertical direction of this camera. Select the target direction by the camera. Validate by clicking .

The target direction can't be parallel to the vertical direction.

If the rigid group, the hook point and the target direction are on the same mobile rigid group, the traveling will follow the mobile rigd group during the simulation. (like a board camera). Example of board camera.

The travelling can also be a tracking which allows to have a camera following a mobile rigid group.

Different travelings can be cumulated in a variable traveling.

Available options: Perspective projection: If the option is not checked, enter the vision field height. If the option is checked, it is the vision field angle to be entered. In this case, the camera will be conical.

Modifications / Additional information:

The traveling is created in the Travelings sub folder of the Mechanism folder from the entities tree. To use a traveling in a simulation, just drag it in the simulation via the entities tree. It is also possible to cumulated several travelings in a variable traveling.

Tracking Traveling

Links / Videos :

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This command allows to define a camera fixed on a rigid group and following a mobile rigid group. This traveling can be linked to a mechanism simulation.

Creation stages / Use: Click the

icon or select the Simulation > Tracking Traveling... command from the drop-down menu.

1. 2. 3. 4. 5.

Select the rigid group where to fix the camera. Select the mobile rigid group to follow. Select an hook point of the camera. Select the vertical direction of this camera. Select the target point of the camera. This point has to be selected on the mobile rigid group to follow. 6. Validate by clicking . Example of a fixed camera following the yellow fork

The traveling can also be a rigid one which allows to have a camera on the mobile rigid group. Different travelings can be cumulated in a variable traveling.

Available options: Perspective projection: If the option is not checked, enter the vision field height. If the option is checked, it is the vision field angle to be entered. In this case, the camera will be conical.

Modifications / Additional information:

The traveling is created in the Travelings sub folder of the Mechanism folder from the entities tree. To use a traveling in a simulation, just drag it in the simulation via the entities tree. It is also possible to cumulated several travelings in a variable traveling.

Variable Traveling

Links / Videos :

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This command allows to cumulate several travelings and to define the moment when they have to be started. This traveling can be linked to a mechanism simulation.

Creation stages / Use: Click the icon or select the Simulation > Variable Traveling... command from the drop-down menu. 1. Enter the start time of the traveling. 2. Select the traveling to use in the drop-down list. 3. Validate by clicking .

Rigid and Tracking travelings can be selected.

Available options: Interpolation: If the first traveling starts at 0s and a second at 10s, the interpolation allows to progressively move from the first traveling to the second during the complete time of the first (in our case 10s). If the option is unchecked, the transition between the 2 travelings will be immediate

until the first is finished. This option can have strange behaviors by interpolating 2 different types of traveling (rigid to tracking or vice versa).

Modifications / Additional information:

The traveling is created in the Travelings sub folder of the Mechanism folder from the entities tree. To use a traveling in a simulation, just drag it in the simulation via the entities tree

Distance measurement

This command measures the evolution of a distance during the simulation.

Creation stages / Use: Click the icon or select Simulation > Measurements > Distance Measurement... command from the drop-down menu. 1. 2. 3. 4. 5. 6. 7.

Select the first rigid group. Select the second rigid group. Select the type of first geometry (axis, plane, point). Select this geometry. Select the type of the second geometry (axis, plane, point). Select this geometry. Drop the measurement created in the entities tree in the desired simulation(s).

Several measurements can be used by a same simulation. The same measurement can be used in several simulations. To know the measurement value, use the View measurements command.

Angle measurement

This command measures the evolution of an angle during the simulation.

Creation stages / Use: Click the icon or select Simulation > Measurements > Angle Measurement... command from the drop-down menu. 1. 2. 3. 4. 5. 6. 7.

Select the first rigid group. Select the second rigid group. Select the normal direction at the angle to be measured. Select the first direction of the angle to be measured. Select the second direction of the angle to be measured. Check Multi-turns if the angle can be higher than 180° Drop the measurement created in the entities tree in the desired simulation(s).

The direction of selected axes/edges is important to define the initial angle value.

Several measurements can be used by a same simulation. The same measurement can be used in several simulations. To know the measurement value, use the View measurements command.

Velocity measurement

This command measures the velocity between 2 points, during the simulation.

Creation stages / Use: Click the icon or select Simulation > Measurements > Velocity Measurement... command from the drop-down menu. 1. Select the mobile rigid group. 2. Select a point of this rigid group. 3. Select Amplitude or Projection. Projection allows you to fill in a direction. The measure value will be regarding this direction (positive or negative). 4. If Projection is selected, select the direction of projection. 5. Also select if the projection is absolute or relative. The measurement in relative projection is the measurement in relation to the rigid group which can also have a velocity. The measurement in absolute projection will be in relation to the absolute direction selected. 6. Drop the measurement created in the entities tree in the desired simulation(s).

Several measurements can be used by a same simulation. The same measurement can be used in several simulations. To know the measurement value, use the View measurements command.

Angular velocity measurement

This command measures the angular velocity of a rigid group based on its joints during the simulation.

Creation stages / Use: Click the icon or select Simulation > Measurements > Angular Velocity Measurement... command from the drop-down menu. 1. Select the mobile rigid group. 2. Select Amplitude or Projection. Projection allows you to fill in a direction. The measure value will be regarding this direction (positive or negative). 3. If Projection is selected, select the direction of projection. 4. Also select if the projection if absolute or relative. The measurement in relative projection is the measurement in relation to the rigid group which can also have a velocity. The measurement in absolute projection will be in relation to the absolute direction chosen. 5. Drop the measurement created in the entities tree in the desired simulation(s).

Several measurements can be used by a same simulation. The same measurement can be used in several simulations. To know the measurement value, use the View measurements command.

Acceleration measurement

This command measures the acceleration of a rigid group based on its joints during the simulation.

Creation stages / Use: Click the icon or select Simulation > Measurements > Acceleration Measurement... command from the drop-down menu. 1. Select the mobile rigid group. 2. Select Amplitude or Projection. Projection allows you to fill in a direction. The measure value will be regarding this direction (positive or negative). 3. If Projection is selected, select the direction of projection. 4. Also select if the projection is absolute or relative. The measurement in relative projection is the measurement in relation to the rigid group which can also have an acceleration. The measurement in absolute projection will be in relation to the absolute direction selected. 5. Drop the measurement created in the entities tree in the desired simulation(s).

Several measurements can be used by a same simulation. The same measurement can be used in several simulations. To know the measurement value, use the View measurements command.

Angular acceleration measurement

This command measures the angular acceleration of a rigid group based on its joints during the simulation.

Creation stages / Use: Click the icon or select Simulation > Measurements > Angular Acceleration Measurement... command from the drop-down menu. 1. Select the mobile rigid group. 2. Select Amplitude or Projection. Projection allows you to add a direction. The measure value will be regarding this direction (positive or negative). 3. If Projection is selected, select the direction of projection. 4. Also select if the projection is absolute or relative. The measurement in relative projection is the measurement in relation to the rigid group which can also have an acceleration. The measurement in absolute projection will be in relation to the absolute direction selected. 5. Drop the measurement created in the entities tree in the desired simulation(s).

Several measurements can be used by a same simulation. The same measurement can be used in several simulations. To know the measurement value, use the View measurements command.

Force measurement

This command measure the force of a rigid group based on its joints during the simulation.

Creation stages / Use: Click the icon or select Simulation > Measurements > Force Measurement... command from the drop-down menu. 1. Select the mobile rigid group. 2. Select a source from the proposed forces or joints in the drop down list. 3. Select Amplitude or Projection. Projection allows you to fill in a direction. The measure value will be regarding this direction (positive or negative). 4. If Projection is selected, select the direction of projection. 5. Also select if the projection is absolute or relative. The measurement in relative projection is the measurement in relation to the rigid group which can also have a force. The measurement in absolute projection will be in relation to the absolute direction selected. 6. Drop the measurement created in the entities tree in the desired simulation(s).

Several measurements can be used by a same simulation. The same measurement can be used in several simulations. To know the measurement value, use the View measurements command.

Moment of Force Measurement Links/Videos:

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This command allows you to measure the moment of a rigid group based on its joints during simulation.

Creation stages / Use: Click the icon or select Simulation > Measurements > Moment of Force Measurement... command from the drop-down menu. 1. Select the mobile rigid group. 2. Select a source from the proposed forces or joints in the drop down list. 3. Select the rotation point. 4. Select Amplitude or Projection. Projection allows you to fill in a direction. The measure value will be regarding this direction (positive or negative). 5. If Projection is selected, select the direction of projection. 6. Also select if the projection is absolute or relative. The measurement in relative projection is the measurement in relation to the rigid group which can also have a force. The measurement in absolute projection will be in relation to the absolute direction selected. 7. Drop the measurement created in the entities tree in the desired simulation(s).

Several measurements can be used by a same simulation. The same measurement can be used in several simulations. To know the measurement value, use the View measurements command.

Energy measurement

This command measures the kinetic or potential energy during the simulation.

Creation stages / Use: Click the icon or select Simulation > Measurements > Energy Measurement... command from the drop-down menu. 1. Check Kinetic or Potential or both. In the event both types of energy are checked, it is the sum of both which will be displayed. 2. Drop the measurement created in the entities tree in the desired simulation(s).

Several measurements can be used by a same simulation. The same measurement can be used in several simulations. To know the measurement value, use the View measurements command.

View measurements

This command allows you to view the different measurements dropped in the simulation(s) from the entities tree.

Creation stages / Use: Click the icon or select Simulation > View Measurements... from the drop-down menu. 1. If several simulations are available, select the desired simulation in the drop down list. 2. Click Refresh if the button is not grayed out. The button is grayed out when the simulation is updated. Refreshes can also be run from the entities tree. 3. Use the vertical and horizontal sliders to increase or decrease the precision of the table and move your cursor along the curve. The coordinates will display in the dynamic text area situated under the cursor.

When several curves are displayed on the table, their color may be modified in the Measurements folder in the entities tree by right-clicking on the desired measurement and by selecting attributes. Several different measurements can be displayed at the same time in the measurements window. Measurements can be added/removed by drag and a contextual menu allows to access to the scale factor and the unit of this measure. The measurements must be drag in the simulation since the folder of entities tree.

Turn your mouse wheel to increase or decrease the accuracy of the table. Each graph has its own cursor allowing to animate the mechanism directly from the graph. By moving the cursor on the curve, the value is displayed when clicking.

Available Options: It is possible to export measurements by clicking the Export measurements button.

Export measurements

This command exports the measurements taken to a csv file during a kinematics or dynamic simulation.

Creation stages / Use: Select the Simulation > Export measurements... command from the drop-down menu, with the contextual menu from the simulation in the entities tree or from the Export measurements button from the View measurements command. 1. Select the simulation to which the measurement should be exported. 2. Click Refresh if the button is not grayed out. The button is grayed out when the simulation is updated. Refreshes can also be run from the entities tree. 3. Enter the number of measurements to be taken per second. 4. Select the values separator for the exported .csv file. Each cell is separated by this separator. During this file import, this separator has to be indicated. 5. Select the decimal separator. Automatic keeps the TopSolid parameters, Period or ANSI allows to force this separator in the exported file. 6. Select encoding. Unicode allows to not have trouble with special characters (for example Japanese or Chinese characters) if the file is opened in another language. With ANSI, these characters may be lost. 7. Indicate the name and the path of the exported file by clicking on Scroll.

If the Auto refresh mode is active on the kinematics or dynamic simulations, the Update button is grayed out. The number of lines in the exported file shall depend on the duration of the simulation and the number of measurements to be carried out per second.

Trajectory

This command allows you to view the trajectory from a point linked to a rigid group in relation to another rigid group.

Creation stages / Use: Click the

icon or select Simulation > Trajectory... from the drop-down menu.

1. Select the simulation. 2. Click Refresh if the button is not grayed out. The button is grayed out when the simulation is updated. Refreshes can also be run from the entities tree. 3. Select the mobile rigid group. 4. Select the trajectory origin of the mobile rigid group. 5. Select the type of sketch to generate. If this is a planar sketch, select its plane. If this is a spatial sketch, there is no plane to select.

You cannot modify the trajectory type (basified or not) after the validation. An associative trajectory is only visible in the mechanism stage. In the modeling stage, it is grayed out. When selecting the origin of the trajectory, the design configuration is updated up to the validation of the command. When displaying the trajectory, the chosen configuration is updated again.

A trajectory is a polyline. The number of points is defined in the simulation, by the number of points per second. The greater the number of points, the more exact the trajectory, but the calculation time will also be longer.

Available Options: Basify: The trajectory can be either associative, and therefore recalculated when the mechanism is changed, or by checking Basify, produce an editable sketch at the modeling stage that may be used.

Advanced options:

Fixed Rigid Group: Select a rigid group in relation to where the mobile rigid group will move. If no group is selected, the built rigid group is taken into account. Filtering: Filtering allows you to delete merged and aligned points on the trajectory. Angle: TopSolid will create 2 lines with 3 successive points. If the angle between these 2 lines is less than the angle entered, TopSolid considers that the points are aligned and deletes the intermediate points in order to create one line instead of different segments. Distance: If the distance between the points is less than the distance entered, TopSolid considers that the points are merged and deletes useless points. During simulation, the point used to create the trajectory cannot move for a moment, in this case points will overlap. Smoothing: If the points can be registered on a curve, the polyline will be replaced by arcs or splines. Angle: Smoothing can be done under this angle. Above, TopSolid considers it as an acute angle. Distance: If the distance between the points is registered on an arc, TopSolid can replace the polyline with an arc. Tolerance: The polyline is smoothed by interpolation for the given tolerance. (arcs and lines). Splines: Allows TopSolid to replace arcs and lines by splines. Cleaning: If 2 colinear segments and end to end, with each a length lower than the entered value , then these 2 segments will be replace by one with the length of both. "Raw" Trajectory: Obtained result without filtering or smoothing.

Trajectory with Angle Filtering: If angle "a" between the 2 lines is less than the angle entered, the polyline will be replace by a line.

Trajectory with Distance Filtering: If distance "d" is less than the distance entered, the points are considered as merged and deleted (in yellow on the image).

Trajectory with Angular Smoothing: If the points of the polyline are registered on a curve and that angle "a" between 2 lines is less than the angle entered, the polyline will be smoothed. (On the image, the section with the yellow points is smoothed).

Trajectory with Distance Smoothing: If the distance between the points is registered on an arc, the polyline will be replaced by an arc. (On the image, the section with the yellow points is replaced by an arc).

Trajectory with Tolerance Smoothing: The polyline is converted to spline by interpolation regarding to the entered tolerance.

These options are as useful for planar sketches as for spatial sketches.

Center of Mass Trajectory

Links / Videos :

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This command allows to calculate and visualize by a 2D or 3D sketch, the center of mass trajectory of several rigid groups during a simulation. This command specially allows to see if a simulation center of mass is limited in its supports.....

Creation stages / Use: Click the icon or select the Simulation > Center of Mass Trajectory... command from the drop-down menu. 1. Select the simulation. 2. Click Refresh if the button is not grayed out. The button is grayed out when the simulation is updated. Refreshes can also be run from the entities tree. 3. Select rigid groups to take into account. 4. Select the type of sketch to generate. If this is a planar sketch, select its plane. If this is a spatial sketch, there is no plane to select. 5. Validate by clicking .

You cannot modify the trajectory type (basified or not) after the validation. An associative trajectory is only visible in the mechanism stage. In the modeling stage, it is grayed out. When selecting the origin of the trajectory, the design configuration is updated up to the validation of the command. When displaying the trajectory, the chosen configuration is updated again.

A trajectory is a polyline. The number of points is defined in the simulation, by the number of points per second. The greater the number of points, the more exact the trajectory, but the calculation time will also be longer.

Available Options: Basify: The trajectory can be either associative, and therefore recalculated when the mechanism is changed, or by checking Basify, produce an editable sketch at the modeling stage that may be used.

Advanced options: Filtering: Filtering allows you to delete merged and aligned points on the trajectory. Angle: TopSolid will create 2 lines with 3 successive points. If the angle between these 2 lines is less than the angle entered, TopSolid considers that the points are aligned and deletes the intermediate points in order to create one line instead of different segments. Distance: If the distance between the points is less than the distance entered, TopSolid considers that the points are merged and deletes useless points. During simulation, the point used to create the trajectory cannot move for a moment, in this case points will overlap. Smoothing: If the points can be registered on a curve, the polyline will be replaced by arcs or splines. Angle: Smoothing can be done under this angle. Above, TopSolid considers it as an acute angle. Distance: If the distance between the points is registered on an arc, TopSolid can replace the polyline with an arc. Tolerance: The polyline is smoothed by interpolation for the given tolerance. (arcs and lines). Splines: Allows TopSolid to replace arcs and lines by splines. Cleaning: If 2 colinear segments and end to end, with each a length lower than the entered value , then these 2 segments will be replace by one with the length of both.

"Raw" Trajectory: Obtained result without filtering or smoothing.

Trajectory with Angle Filtering: If angle "a" between the 2 lines is less than the angle entered, the polyline will be replace by a line.

Trajectory with Distance Filtering: If distance "d" is less than the distance entered, the points are considered as merged and deleted (in yellow on the image).

Trajectory with Angular Smoothing: If the points of the polyline are registered on a curve and that angle "a" between 2 lines is less than the angle entered, the polyline will be smoothed. (On the image, the section with the yellow points is smoothed).

Trajectory with Distance Smoothing: If the distance between the points is registered on an arc, the polyline will be replaced by an arc. (On the image, the section with the yellow points is replaced by an arc).

Trajectory with Tolerance Smoothing: The polyline is converted to spline by interpolation regarding to the entered tolerance.

These options are as useful for planar sketches as for spatial sketches.

Simulation Pattern

Links / Videos :

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This command allows to define a pattern corresponding to a rigid group displacement during a simulation.

Creation stages / Use: Click the icon or select the Simulation > Simulation Pattern... command from the drop-down menu. 1. Select the simulation. 2. Click Refresh if the button is not grayed out. The button is grayed out when the simulation is updated. Refreshes can also be run from the entities tree. 3. Select the mobile rigid group. 4. Select the total number of points representing the simulation of this mobile rigid group. 5. Validate by clicking .

You cannot modify the pattern type (basified or not) after the validation. An associative pattern is only visible in the mechanism stage. In the modeling stage, it is grayed out.

A pattern is a repetition of points. The greater the number of points,

the more exact the pattern, but the calculation time will also be longer.

Available Options: Basify: The pattern can be either associative, and therefore recalculated when the mechanism is changed, or by checking Basify, produce an editable sketch at the modeling stage that may be used .

Display: The Display section allows you to redefine the position of the visualization of the pattern. 1. Select the starting point and/or 2. Select the starting frame.

Advanced options: Select a rigid group in relation to where the mobile rigid group will move. If no group is selected, the built rigid group is taken into account.

Exploded Links/Videos:

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This command allows you to create an explosion from an assembly.

Creation stages / Use: Select Explosion... from the popup menu of an assembly, in the project tree. 1. Select the explosion template to use. 2. Select the assembly representation to use. 3. If the assembly has several configurations, select the configuration to use. 4. Validate by clicking on .

This command is only available on assemblies.

This command can also be used from the assembly by using the contextual menu on its tab.

Include assembly

This command allows you to include an assembly in an Exploded document.

Use: Click the icon or select the Explosion > Include... command from the drop-down menu. 1. 2. 3. 4.

Select the assembly document to include. Select the assembly representation to use. Select the configuration to use (if several). Validate.

Only the open assembly documents will be proposed in the list of the documents to include.

Modifications: Right-clicking on the components of the assembly allows you to edit the inclusion with the objective of changing the included document and/or configuration.

Explosion group

This command creates explosion groups. The objective here is to displace all the components of the same group in the same operation.

Creation stages: Click the icon or select the Explosion > Group... command from the drop-down menu. 1. Provide a name for the group being created 2. Select the entities to group. By using Entities to ignore, the group will consist of the entire assembly, without the selected entities. 3. Validate the command.

When an explosion group is being created, the assembly structure is presented in a tree. Items at every level of the tree can be selected, the selection of a node will select all the branches which follow. This allows a rapid selection of the subsets. The rotating selection allows you to move up or down the tree from the selected entity. This selection is modifiable via the Assembly to Part and Part to Assembly modes. The part mode allows you to only select parts.

Available Options: Hide:

The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Modifications: In the entities tree, an Explosion groups folder contains all the created groups. Simply edit one of these groups to modify its content (add or remove items).

Include existing explosions

If some sub-sets of the assembly have an exploded belonging to a current explosion group, they can be inserted in the current document.

Use: Click the icon or select Explosion > Include Existing Explosions...from the drop-down menu. 1. Select the reference part, which is the fixed part of this group. The explosion will be included with respect to this reference part. 2. Select the explosion group to be accounted for. 3. Select the sub-set with an exploded. 4. Select the exploded document to include 5. Validate the command.

Available Options: Explosion lines: This cell (checked by default) also includes the explosion lines being inserted.

Modifications: To modify an "include existing explosion" operation, open the operations tree and unfold the explosion of the group to modify.

Then select the desired Displacement operation the edit it by rightclicking it.

Translation Links/Videos:

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This command explodes the selected entities by translation.

Creation stages / Use: Click the icon or select Explosion > Translation... from the drop-down menu. 1. Specify the translation direction. 2. Specify the distance of this translation. 3. Select the group or the entities to translate.

The displacement angle is taken between the origin point and the center of the part to move. The double-click on a moved entity or its explosion line to display the moving dimension and modify the value.

You can move an exploded entity by selecting it with the left mouse button and moving the mouse with the button held down.

Available Options: Hide:

The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Reference Part: You are able to use a reference part for your displacement. If, as a result, the reference part is moved, exploded entities that use this item as reference will also be moved. To remove an entity in this filed, just click an empty place of the graphic area when this field is active.

Ignore Dependencies: If the item moved is used as reference by another displacement, selecting this cell will turn off this reference. The item is therefore moved without moving items using it as reference.

Explosion lines: - One line (for Translation and Rotation only): If several entities are moved, this cell allows you to display one line for all the entities and not one line per entity. - Construction mode: Shortest: The line uses the shortest route between the initial position and the displaced entity.

Rotation Links/Videos:

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This command explodes the selected entities by rotation.

Creation stages / Use: Click the icon or select Explosion > Rotation... from the dropdown menu. 1. Specify the rotation axis. 2. Specify the angle of this rotation. 3. Select the group or entities to move.

The displacement angle is taken between the origin point and the center of the part to move. The double-click on a moved entity or its explosion line to display the moving dimension and modify the value. You can move an exploded entity by selecting it with the left mouse button and moving the mouse with the button held down.

Available Options: Hide: The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Reference Part: You are able to use a reference part for your displacement. If, as a result, the reference part is moved, exploded entities that use this item as reference will also be moved. To remove an entity in this filed, just click an empty place of the graphic area when this field is active.

Ignore Dependencies: If the item moved is used as reference by another displacement, selecting this cell will turn off this reference. The item is therefore moved without moving items using it as reference.

Explosion lines: - One line (for Translation and Rotation only): If several entities are moved, this cell allows you to display one line for all the entities and not one line per entity. - Construction mode: Shortest: The line uses the shortest route between the initial position and the displaced entity.

Axial displacement

This command explodes the selected entities based on a given axis.

Creation stages: Click the icon or select Explosion > Axial displacement... from the drop-down menu. 1. 2. 3. 4.

Select the displacement direction. Select the origin point of the displacement. Specify the coefficient or the displacement distance. Select the group or entities to move.

The move distance is the result of the length between the point of origin and the center of the part to move multiplied by the coefficient.

Available Options: Hide: The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Reference Part - You can use one reference for your move: If, as a result, the reference part is moved, exploded entities that use this item as reference will also be moved.

- To remove an entity from this field, when the field is active, click in the empty space in the graphic area.

Ignore Dependencies: If the item moved is used as reference by another displacement, selecting this cell will turn off this reference. The item is therefore moved without moving items using it as reference.

Selection of entities to displace: If the explosion group is a subset, the rotary picking on the screen allows you to go up or down in the tree from the picked entity. This selection logic is modifiable by the Part, Assembly to Part and Part to Assembly modes.

Local displacements: When a group is moved, all entities belonging to the group will move by the same value (distance or coefficient), however you can locally modify these values for given parts by selecting them from the list and entering the desired value.

Explosion lines: - One line (for Translation and Rotation only): If several entities are moved, this cell allows you to display one line for all the entities and not one line per entity. - Construction mode: Shortest: The line uses the shortest route between the initial position and the displaced entity

Modifications:

To modify an existing axial displacement, open the operations tree and unfold the explosion of the group to be modified. Then select the desired Displacement operation the edit it by right-clicking it.

Example:

Spherical displacement

This command explodes the entities selected by a spherical rotation movement of three degrees of freedom around a fixed point (origin point of the displacement).

Creation stages: Click the icon or select Explosion > Spherical Displacement ... from the drop-down menu. 1. Select the origin point of the displacement. 2. Specify the displacement coefficient. 3. Select the group or entities to move.

The displacement distance is the result of the length between the origin point and the center of the part to displace multiplied by the coefficient.

Available Options: Hide: The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

Reference Part: - You can use one reference for your move:

If, as a result, the reference part is moved, exploded entities that use this item as reference will also be moved. - To remove an entity from this field, when the field is active, click in the empty space in the graphic area.

Ignore Dependencies: If the item moved is used as reference by another displacement, selecting this cell will turn off this reference. The item is therefore moved without moving items using it as reference.

Selection of entities to displace: If the explosion group is a subset, the rotary picking on the screen allows you to go up and own the tree from the picked entity. This selection logic is modifiable by the Part, Assembly to Part and Part to Assembly modes.

Explosion lines: - One line (for Translation and Rotation only): If several entities are moved, this cell allows you to display one line for all the entities and not one line per entity. - Construction mode: Shortest: The line uses the shortest route between the initial

Modifications: To modify an existing spherical displacement, open the operations tree and unfold the explosion of the group to modify. Then select the Displacement operation then edit it by right-clicking.

Example:

Radial displacement

This command explodes the entities selected by a radial movement.

Creation stages: Click the icon or select Explosion > Radial Displacement ... from the drop-down menu. 1. Select the origin point of the displacement. 2. Select the axis (this axis provides the rotation axis and the move direction of the entities). 3. Specify the radial coefficient. 4. Specify the coefficient along the axis. 5. Select the group or entities to move.

The displacement distance is the result of the length between the origin point and the center of the part to displace multiplied by the coefficient. Radial coefficient: used for the entities radial displacement. Coefficient along the axis: used for the displacement of the entities along the axis.

Available Options: Hide: The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially

those who were behind.

Reference Part: - You can use one reference for your move: If, as a result, the reference part is moved, exploded entities that use this item as reference will also be moved. - To remove an entity from this field, when the field is active, click in the empty space in the graphic area.

Ignore Dependencies: If the item moved is used as reference by another displacement, selecting this cell will turn off this reference. The item is therefore moved without moving items using it as reference.

Selection of entities to displace: If the explosion group is a subset, the rotary picking on the screen allows you to go up and own the tree from the picked entity. This selection logic is modifiable by the Part, Assembly to Part and Part to Assembly modes.

Explosion lines: - One line (for Translation and Rotation only): If several entities are moved, this cell allows you to display one line for all the entities and not one line per entity. - Construction mode: Shortest: The line uses the shortest route between the initial position and the displaced entity.

Modifications:

To modify an existing radial displacement, open the operations tree and unfold the explosion of the group to modify. Then select the Displacement operation then edit it by right-clicking.

Example:

Explosion line

This command creates an explosion line between two points.

Creation stages: Click the icon or select Explosion > Explosion Line... from the drop-down menu. 1. Select the starting point. 2. Select the arrival point. 3. Validate.

Available Options: Indent: This option allows you to indent explosion lines from the start or end. The length of the line will therefore be reduced from the value of these indents.

Construction mode: Shortest: The line uses the shortest route between the initial position and the displaced entity. Parallel to Axes: The line is parallel to the axes of the selected reference frame.

Style: This zone selects the explosion line style to use. Attributes: If select the Attributes cell, you will be able to configure the type of line, its thickness and its color (the button

allows to remove the selected color). The half tone cell allows to use the half tone of the color.(gray for back for example).

Modifications: To modify an existing explosion line, open the operations tree and select the explosion line to modify. Right-clicking allows you to edit in order to modify.

Auto Animation Links/Videos:

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This command allows to create a mounting/dismounting animation rapidly regarding defined movements (translations and rotations).

Creation stages / Use: Click the icon or select Mounting > Auto Animation... from the drop-down menu. 1. Enter the number of positions per second. The trajectory points are pre-calculated. The greater the number of positions, the more accurate the trajectory. Conversely, too few positions will create a segmented trajectory. 2. Enter the duration of the animation. 3. Validate.

The different movements will be equally split over the entire duration of the animation. If certain movements must have different durations, use the Animation command.

Available Options: Viewer: By checking this option, the animation will be visualized if this

document is exported as package and opened with TopSolid'Viewer.

Animation Links/Videos:

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This command allows to create an animation of mounting/dismounting in which several displacements (translations and rotations) can be included. It also allows to define when these displacements must be executed. This animation can be played and/or recorded.

Creation stages / Use: Click the

icon or select Mounting > Animation... from the drop-down menu.

1. Enter a name for the animation. 2. All movements are placed in the timing chart with the same duration. You can move them by dragging them with the mouse in the track and from one track to another. 3. Validate. Click the image below for further information.

This command creates an Animations sub-folder in the entities tree.

You can quickly create an animation by using the Auto Animation command.

Modifications / Additional information: For all modifications with regard to the animation, use the popup menu, from the entities tree in the Animations folder: Using the popup menu in the entity tree, rename, edit or delete an animation or movements. To modify the start time, duration or to rename a movement, use the contextual menu on the task. To modify the start date and duration, you can also move the rectangle that represents the movement. Removed movements from the timing chart appear in the task column, which can then be dragged again in the timing chart.

Play animation Links/Videos:

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This command allows you to view an ascending or descending animation.

Creation stages / Use: Click the icon or select Mounting > Play Animation... from the drop-down menu. 1. Select the animation to view from the drop down list. If there is only one animation, it is selected by default. 2. Use the cursor to manually view the animation. Rewind: Goes back to the start of the animation at any time.

Quick Reverse: Plays the animation in reverse, and quickly. Play Backwards: Plays the animation in reverse. If the animation is a mounting, it is the dismounting which will be played. Pause: Stops the animation. Play: Plays the animation as defined. Quick Advance: Plays the animation quicker.

Play loop: Loop plays the animation, until another command is used.

To record the animation, use the Record Animation command.

Available Options: Slowing: Select the slow motion value. 1 is normal speed; a higher value slows down simulation, a lower value accelerates it. Negative values are not allowed.

Time: Enter the time. The animation will start at the time indicated. For example, if 2s is entered, the animation will start directly at 2 seconds. The total time is given when creating the animation.

Record Animation Links/Videos:

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This command allows you to record an ascending or descending animation.

Creation stages / Use: Click the icon or select Mounting > Record Animation... from the dropdown menu. 1. Select the animation to record. 2. Enter the start time. To start at the beginning of the simulation, enter 0s (default proposed value). 3. Enter the end time. The proposed time is the total time of the animation (value proposed by default). 4. Enter the slow motion value. 1 is normal speed; a higher value slows down simulation, a lower value accelerates it. Negative values are not allowed. 5. Select the view to save. This choice is useful only if the document is displayed in several views. 6. Increase or decrease the frame size in the graphic area by moving its vertex. 7. Move the frame in the graphic area by moving one side. 8. Validate by clicking on .

Available Options: Video setup: 1. Enter the Width and Height of the video to save. These values are in pixels. 2. Enter the number of images per second. For videos, generally this value is between 25 and 30. If below, the video will be smaller, but jerky. 3. Enter the key-frame rate if needed.

4. Select one of the installed Codecs. The same codes are necessary on the station that will playback the video. If you use Uncompressed option, a video of a couple of secondes may take several hundreds of Mb on your hard disk. 5. Modify the quality of the video by moving the cursor (grayed out for some codecs). An increase in quality increases the size of the video. 6. Configure the codec (for advanced users). Refer to the documentation of the codec). 7. Select the render mode from the drop-down list. The render mode has a lot of influence on the calculation time and the generation of the video. 8. Select the Background of the video. The screen background can be displayed in the video, or a black background, or a white one. 9. Check Open Video to automatically open the video in the viewer defined in Windows after it has been created. 10. Validate. 11. Select a destination directory.

Several options improve video quality, but also increase size and calculation time. For example, a rendering with effects takes much lo to calculate because for 25 images/second, 25 times the effects mus calculated. The most frequent video playback problem is the absence of the cod the station trying to play the video.

Realistic rendering:

Antialiasing: this cursor allows to smooth elements edges.

Lighting accuracy: This cursor allows you to improve rendering qualit produced by extended lights and materials reflects. The improvement is increasing antialiasing, but it is much faster. This setting is only on if th that is likely to be adjusted (radiosity, sky light, extended lights).

Simplified Rendering: This option turns off all "costly" calculation tim lights, material with imperfect reflection, ...

Global Illumination: This option allows you to accurately simulate the scene itself, and no longer only the direct light from luminous sources. In a classic image calculation, an area that is not directly lit by light is b light re emitted by the walls and scene objects. Global illumination take avoids obtaining unlit areas. This option is particularly useful for implementation and architecture im

Global illumination accuracy: This option allows you to improve glob taking in account scene little details. Generally, default value (15%) is e

Recursion depth: Allows to setup of shadows depth, of reflection and r For example, if you have several mirrors reflecting themselves one othe will be reflected only in the first mirror. With a value of 2, this reflection mirror. This setting is only for beamed shadows.

Auto Mounting Stages Links/Videos:

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This command allows you to automatically create different mounting stages by basing them on translations or rotations. These stages can then be used in mounting notices.

Creation stages / Use: Click the menu.

icon or select Mounting > Auto Mounting Stages... from the drop-down

1. If Make Displacement is checked, the parts and assemblies of the mounting step will be exploded in the mounting notice. If it is unchecked, parts and assemblies of the mounting stage will ascend non exploded.

Mounting Notice 1

Mounting Notice 2

Mounting Notice 3

The parts are exploded.

The Make displacement option of this mounting stage is unchecked. The part comes installed.

The option Make displacement is checked for the mounting step. The part is displayed exploded.

2. Enter a prefix for the name of the stages. If no prefix is entered, the stages will be called 1, 2, ... 3. Select the numbering direction (ascending or descending). 4. Check First Stage to create a first stage that contains only the start part, on which all others will gather. 5. Check Last Stage to create a stage that includes the final mounted assembly. 6. Validate.

The direction of numbering is important. Conditions the order of steps in the mounting notice.

Steps are created based on the selected operation and must be defined from the bottom to the top of the chronology of the explosion. An Mounting line is created in the operations tree, above the selected displacement. An Mounting Stages folder is created in the entities tree.

You can manually create mounting stages by using the Mounting Stages command.

Modifications / Additional information: The steps can be contextually edited and modified from the Mounting Stages folder of the entity tree. You can see the effects of the defined ascending steps with the Mounting > View mounting stages... command. By default, the title of the first mounting stage created is numbered "1", which in fact corresponds to the case of descending: at the start everything is up, it's the start of the chronology of the explosion. If it is not the case, you can change titles by editing operations or use the Mounting > Rename mounting stages... command.

View mounting stages Links/Videos:

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This command allows you to view the different mounting stages.

Creation stages / Use: Click the icon or select Mounting > View Mounting Stages... from the drop-down menu. 1. Select the mounting stage to view by selecting it from the list. 2. If Make displacement is checked, the parts and assemblies of the mounting step will be exploded when viewed. If it is unchecked, the parts and assemblies of the mounting stage will be shown unexploded.

The option Make displacement is unchecked for the mounting stage. The part is shown installed.

The option Make displacement is checked for the mounting step. The part is displayed exploded.

It is possible to check or uncheck the Make displacement option in order to see the result and select at which stage to check it.

Rename Mounting Stages Links/Videos:

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By default, the title of the first mounting stage created is numbered "1", which in fact corresponds to the case of descending: at the start everything is up, it's the start of the chronology of the explosion. When you would like to create an mounting notice, you must rename the stages to put them in reverse chronological order.

Creation stages / Use: Click the icon or select Mounting > Rename Mounting Stages... from the drop-down menu. 1. Enter a prefix. The prefix of the mounting stage is proposed by default. 2. Select the numbering direction (ascending or descending).

The direction of numbering is important. Conditions the order of steps in the mounting notice.

Assembly Links:

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This command creates the BOM of an assembly document.

Creation stages / Use: Select the BOM > Assembly... command from the drop-down menu. 1. Select the source assembly document. 2. Choose if you want to use the representation or a set defined into the assembly document. It is not possible to use both at the same time for the same bom. 3. Validate the command.

The use of the option "set" is memorized same as the sets names. As a result, you can change the reference assembly document afterwards and if the new one contains as well the same sets, the bill of material will be properly updated. This allows to create predefined bill of material template document for specific assembly set (as casing, motor...)

Available Options: Representation: This option lists all representations of the assembly and allows to

select the one to use to display the bom.

Sets: If sets have been defined in the assembly, one of them can be used to display the bom.

Group by property: This checked option will group on the same BOM line different parts having all identical properties. If 4 M6x20 hexagonal screws are used in the same subset, there will only be one line whether the option is checked on not. However, if a cubical part and a cylindrical part are both called "end stops" and all properties in their respective columns are identical, they can be grouped.

Compare parts geometry: This option allows you to make a topological comparison between parts. It allows you to distinguish parts with the same properties (Description, Material,...), the same dimensions (Length, Width,...) but different machinings.

Filters: This option allows to filter your bill of material to be able to exclude/keep an elements selection. You just have to check the filter to use to activate it. There are 2 types of filters in this dialog: Source Document: this area lists filters created in the source document (Entities Filter and Filter by Properties). Filter Documents: this area lists the existing filter documents in the source project or in the project referenced by the source document. If the Activate cell is selected, only elements matching with this filter will be kept in the bill of material ( and consequently, all other elements will be excluded).

Modifications: The modification of a BOM template used in an existing BOM will not update the existing BOM.

To modify the properties displayed in an existing BOM, use the Columns command.

Columns

Links:

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This command modifies the properties used in the current BOM.

Use: Click the

icon or select the BOM > Columns... command from the drop-down menu.

The Template box is then displayed on the screen, showing the properties used in the Selected properties column. You can: Add and/or delete properties. Modify the organization of the properties.

The display unit of the properties corresponds to the units of the document. These units can be accessed via the options tree (to display the options tree, select the TopSolid button then in the Display menu, select Options).

Additional information: This command is only available if the document contains a BOM.

Columns window: (click different areas for explanations).

Available Properties: The section lists all available properties. To create one or more bill of material columns, select the needed properties (by keeping the CTRL key for multi-selection) and click the green arrow to switch in the Selected Properties section. The Image property allow to display the preview of parts into the column of the BOM.

Selected Properties: This section lists all selected properties for additional column creation in the bill of material. To remove one or several bill of material columns, select properties (by keeping the CTRL key for the multi-selection) and click the red arrow to switch them in the Available Properties section. Blue arrows on the right allow to define the properties sort. The upper property will be in the left column and so on.

Selected properties for sorting (ordered): This section allows to define properties to sort. If 2 parts have "Axis" as description, the 2 parts will by grouped in one bill of material line and the quantity will display 2, If the sort is also done with the "Mass" property, the both parts will be on a different line and the quantity will be 1 for each of these 2 lines. The transfer of the selected properties to the Selected Properties for sorting area is done with the green vertical arrow To remove them, click the red vertical arrow. Vertical blue arrows on the right allow to define the properties order for the sort. The upper property will be the first to be used. If the value is the same, the second property will be used.

Forced Column Title: This field allows to enter manually the column name for the selected property.

Column width: In the draft document, the size of each column will be automatically adjusted to the table’s positioning points. To do this, the column size must not be defined; if the size of each column is defined, the table size will be forced and the table’s positioning points will not be considered. When using the Image property, the column width has to be field to adjust the image size. The preview is then displayed as a thumbnail either in the BOM document, or in the BOM table of the draft document.

Visible: By default, columns are visible. By unchecking this option, the column will not be displayed, but will be taken in account for the result of the bill of material (see for example Selected Properties for Sorting ).

Property use: The section allows to define how will be numerical values processed. If for example 3 parts have the same name, but their mass are different and the sort is done with the name: Sort: there will be 3 lines with, for each of them the corresponding mass. Make sum: there will be only one line, the mass column will display the sum of the 3 masses. Make average: there will be only one line, the mass column will display the average of the 3 masses. Don't forget to check the Groups by properties option in the Assembly command.

Format: This section allows to modify the display of numerical values, by modifying the number of decimals, by changing the unit which can be displayed or not.

Alignment: The section allows to choose the result alignment in the column.(Left, Center, right).

Indented: This option, when it is checked, allows to have a gap on the right in the bill of material (in the

draft) for parts/assemblies of lower levels.

Without Indented option for the description property.

With Indented option for the description property.

Sorting: This section allows to choose how to sort the property. The choice is done regarding the type of properties. From A to Z or from Z to A for alphanumeric results (name, description, ...) from the smallest to the greatest or from the greatest to the smallest for numeric results (mass, length, ....) and from the oldest to the most recent or from the most recent to the oldest for dates.

Empty values sorting: This section allows to choose if an empty result of a column has to be displayed first or last.

Columns as This command uses the definition of columns in an existing BOM in a new BOM.

Creation stages / Use: Click the icon or select BOM > Columns as... from the dropdown menu. 1. Select the BOM document to use. 2. Validate.

Only the open BOM documents will be proposed in the drop-down menu of this command.

Additional information: If the current BOM already contains columns, they will be deleted and replaced by those of the BOM used by this command.

Reset Bill of Material Frames Links/Videos:

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This command allows you to renumber the BOM indexes.

Creation stages / Use: Click the icon or select BOM > Reset BOM Indexes... from the drop-down menu. Launching the command automatically renumbers the BOM indexes starting with the first item of the BOM.

Indexes may have to be reset if you add parts to your assembly and/or if you modify the BOM display mode (First Level, Multilevel or Flat).

Modifications / Additional information: This command doesn't allow to force a bill of material index.

Index Rules Links / Videos :

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This command allows to predefine the indexes of the bill of material’s elements. All documents that provide the function used into the rules will be indexed in the same way. This allows for example to index all screws Sxx, all extruded bars EBxx, etc...

Creation stages / Use: Click the icon or select the Bill of Material > Index Rules... command from the drop-down menu. 1. Click the Add button to select the function document to use. 2. You can link a rule with one family document. Otherwise, select in the bottom of the drop-down list. 3. Click the Index to customize it. 4. Validate.

An Index rules folder will be created in the entities tree with the number of rules in brackets. Right click on this folder allows to edit again the Index rules dialog box to modify them. They can be editing running the Index rules command too.

If a rule is modified, existing indexes won't be updated. User must run the Reinitialize Bill of Material indexes command to update them. All indexes will be modified with initial value of counters. As for standard indexes, hole won't be filled. Indexes can go from 3 to 5 if the index 4 had existing but it is not available anymore because the part has been deleted in the assembly and no reinitialization done.

Available options: Add string: Allows you to enter characters (or separators).

Add counter: The counter increments for each new creation. It can be numerical or alphabetical. Indicate the initial value of the counter. Indicate the number of counter characters. Enter the fill character (see result in above example). Validate. There can be only one counter per rule.

Modifications / Additional information: You can change, delete or re-order the part numbering using the Modify, Delete, Up or Down buttons.

Manufacturing Index

This command allows to apply automatically the manufacturing indexes property to the part of a bill of material. The command is only available if the bill of material uses the Flat or Assembly Only modes.

Creation stages / Use: Select the Bill of Material > Manufacturing Index... command from the drop-down menu.

What the command does: If the occurrence property "Manufacturing Index" already exists on the part/sub-assembly occurrence in the source assembly, its value is displayed in the column. If the occurrence property "Manufacturing Index" does not exist, TopSolid creates and applies this property to the part/sub-assembly occurrence and then displays it in the column. The system parameter "Bill of material type" is set as Part Manufacturing if the bill of material uses the Flat mode. Assembly Manufacturing if the bill of material uses the Assembly Only mode. This parameter is used by the bill of material tables in draft documents.

Modifications / Additional information: The manufacturing indexes are displayed in a specific column. Thus in order to visualize this values, you need to add the column "Manufacturing Index". The color of this column indicates that the displayed value comes from an occurrence property. This color can be configured in "Tools > Options > Bill of material" If the occurrence property "Manufacturing Index" is modified manually in the assembly, its new value is updated in the bill of material. Vice versa, if the value is defined manually in the bill of material, the value is applied on the corresponding occurrence in the assembly. It is possible to delete all the manufacturing index at once by using the command Clear Manufacturing Index.

Clear Manufacturing Index

This command allows to delete all the manufacturing indexes on the parts from a bill of material document.

Creation stages / Use: Select the Bill of Material > Clear Manufacturing Index... command from the drop-down menu. As the command is selected, all the indexes are automatically deleted.

Warning : using this command deletes all the manufacturing indexes occurrence properties applied on the parts and sub-assemblies from the source document. So it is important to use this command with caution if this occurrence property is also used in the assembly for the design ( Part marking for example) Actually, if the part is marked with its manufacturing index and this command is used, the mounting index information is lost for the marking. And there is no guaranty that the new index that will be created afterward will have the same value.

Mounting Index

This command allows to apply automatically the mounting indexes property to the part and sub-assembly of a bill of material. The command is only available if the bill of material uses the Multilevels mode.

Creation stages / Use: Select the Bill of Material > Mounting Index... command from the drop-down menu.

What the command does: If the occurrence property "Mounting Index" already exists on the part/sub-assembly occurrence in the source assembly, its value is displayed in the column. If the occurrence property "Mounting Index" does not exist, TopSolid creates and applies this property to the part/subassembly occurrence and then displays it in the column. The system parameter "Bill of material type" is set as "Mounting". This parameter is used by the bill of material tables in draft documents.

Modifications / Additional information:

The mounting indexes are displayed in a specific column. Thus in order to visualize this values, you need to add the column "Mounting Index". The color of this column indicates that the displayed value comes from an occurrence property. This color can be configured in "Tools > Options > Bill of material" If the occurrence property "Mounting Index" is modified manually in the assembly, its new value is updated in the bill of material. Vice versa, if the value is defined manually in the bill of material, the value is applied on the corresponding occurrence in the assembly. It is possible to delete all the mounting index at once by using the command Clear Mounting Index.

Clear Mounting Index

This command allows to delete all the mounting indexes on the parts and sub-assemblies from a bill of material document.

Creation stages / Use: Select the Bill of Material > Clear Mounting Index... command from the drop-down menu. As the command is selected, all the indexes are automatically deleted.

Warning : using this command deletes all the mounting indexes occurrence properties applied on the parts and subassemblies from the source document. So it is important to use this command with caution if this occurrence property is also used in the assembly for the design ( Part marking for example) Actually, if the part is marked with its mounting index and this command is used, the mounting index information is lost for the marking. And there is no guaranty that the new index that will be created afterward will have the same value.

Multiple Draftings (Bill of materials)

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This command allows you to draft several documents from a bill of material document. This command is also available from the popup menu of the assembly tab.

Creation stages / Use: Select the contextual command after selecting the bill of material where are parts/assemblies to draft or from a bill of material document. 1. 2. 3. 4.

Select the selection mode in the drop down list (see "available options" for details) Check the parts and/or sets to draft. Double-click in the templates cell to change the template to use. Validate.

Only BOMs can turn on this command. To use this command from an assembly, use the Multiple Draftings function from the popup menu of an assembly. Option Deleted useless drafting is available only if there are draft in the Specified Folder.

Available options: "Selection" tab: Selection: All: all assemblies/parts are selected. None: nothing is selected. Manual: select parts and/or assemblies to be drafted. Assembly: all the assembly type documents are automatically selected. Part:all the part type documents are automatically selected. Criteria: Allows to selected parts/assembly documents according to personalized criterias Drafting template: By left-clicking in this column on the required line, you can specify the drafting template to use for this part. By right-clicking, you have access to the following contextual commands: Apply the template to this type Apply the template to all documents Apply the template to checked documents

"Options" tab:

Parts / Components: The directory choice of created drafts is splitted in two parts: Parts: allows to define the directory for selected parts and/or sub-assemblies to be projected. Component: allows to define the directory for drafts created with a predefined draft. You can choose between: Source Folder: each created draft will be created in the same folder than the part or the assembly. Specified Folder: all drafts will be created in the specified folder. Check the option Delete useless drafting in order to delete the drafts already generated if the part is not anymore in the bill of material. Options: Open after creation: Check this option if all drafts must stay opened. If Open After Creation is checked, the display could be slowed down or blocked depending on th number of documents open and the performance of the graphic card.

Update existing draftings: Check this option to update previously created draftings of assemblies/parts. Project the occurrences: All occurrences : Allows to draft all the occurrences that are in the assembly (families and others). Occurrences of the instance families : Allows to draft the occurrences of the instance families that a in the assembly and not the instance that is in the family. Example : Modification of code in the assembly, after generation of multiple drafting.

In the assembly, Generation of multiple component is drafting. inserted with the code Ht200.

In the assembly, after drafting, modification of code with the code Ht100.

Example : Modification locally in the assembly.

Result with the option Result with the checked : the part unchecked : projected is updated projected is no because it correspond to updated beca the occurrence of correspond to instance family that is in instance famil the assembly.

Instance families. Occurrence of instance Result with option families modified locally unchecked : projection in the assembly (not of instance families. derived part)

Result with option checked : projection of occurrence of instance families that is in the assembly.

Nest draftings: Create drafting bundle: Check this option in order to create automatically a bundle that contains all the create draft. You have to select a bundle template with nesting. You can also specify the destination folder for the bundle document. Update existing drafting bundle: If a bundle with nesting based on the same bill of material already exists, you can activate this option to upd it

Multiple Unfoldings Links/Videos:

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This command allows you to create or update the sheet metal unfoldings of an assembly document.

Creation stages / Use: Click the icon or select BOM > Multiple Unfoldings... from the drop-down menu.

1. Set the multiple unfoldings options in the dialog box. 2. Validate the creation of documents with the button.

For a given line, a double-click in the template column allows to select an unfolding template for this part. TopSolid searches for the biggest flat face. It is defined by default as reference face for the unfolding. To define another reference face, you have to define the origin face of the unfolding positioning command and, if needed, the alignment direction which will be aligned with the X axis of the destination frame of the unfolding.

Available Options:

With draftings : This field allows to generate Drafting with the same choices than the Unfolding (destination folder, drafting options). Three news columns appears : Existing Draftings : if drafting is already generated. Creation : allows to choose the draft to generate. Drafting template : allows to choose the template of drafting.

Selection: This field proposes different quick selection types.

Create in: By default, the unfoldings are created in the source folder. The Specified Folder button allows you to customize the location of documents.

Open After Creation: This option, checked by default, automatically opens newly created unfoldings.

Update Existing Unfoldings: If, among the selected parts for the unfolding, an unfolding document already exists in the destination folder, this document will be updated.

When the multi drafting is created, by default the part projected is the result of unfolding in detailed representation. In the drafting, an additional option is proposed on the Main Set (Other > Unfolding Projection... ) which allows to project the part before the unfolding.

Selecting a document from the dialog list will create a new unfolding even if an unfolding already exists. If you only want to update an existing unfolding, select the appropriate cell without selecting the part in the dialog.

Refresh PDM properties Links / Videos :

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This command allows to refresh bill of material datas that stem from PDM properties.

Creation stages / Use: Click the icon or select the Bill of Material > Refresh PDM properties... command from the drop-down menu.

This command is only enable if the bill of material contains a column with a PDM property.

Additional information: It is possible to display in the bill of material an information called PDM properties. These are properties that come from minor revision status of the reference document, but that are not included in the file itself. In this type of properties, you can find the ERP properties (Published to ERP, Imported in ERP, ERP State) but also properties linked with the Life Cycle of the document (Life Cycle Sub State).

As these properties are not included in the reference documents, the bill of material cannot know if it is up to date or not. So this command allows to refresh this data.

Export BOM (csv or text)

This command allows to export a BOM to csv file or text file.

Creation stages / Use: 1. Right-click the BOM file to export and select Import / Export > 2. 3. 4. 5. 6.

Export document with conversion... Select the destination path in the window and the desired file type (csv or text). Click Save. Select the values separator for the exported file. Select the encoding type. Validate by clicking .

Available Options: Separator: 3 separators are available as default: Tabulation, Semicolon and Comma. Possibility to customize the separator with the Other button.

Encoding: Unicode allows to not have trouble with special characters (for example Japanese or Chinese characters) if the file is opened in another language. ANSI, these characters may be lost.

Export bill of material to TopSolid'Quote Links/Videos:

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This command allows you to export a bill of material document for use with the TopSolid'Quote quote software.

Creation stages / Use: Click the icon or select Bill of material > Export bill of material to TopSolid'Quote... from the drop-down menu. The Import/Export > Export bill of material to TopSolid'Quote...command is also available with the contextual menu on a bill of material document tab. TopSolid'Quote is launched if it isn't already.

TopSolid'Quote is a TopSolid quote software. It requires a license in order to use it and must definitely be installed in order to use this command.

OptiCut Export Links / Videos :

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This command allows to export all extruded bars in a specific CSV format for OptiCut.

Creation stages / Use: Click the icon or select the Bill of Material > OptiCut Export... command from the drop-down menu. 1. Give the file name and the destination folder. 2. Validate by clicking .

This format is also available by calling up the Export Document with Conversion command on a BOM document.

The trimming angle management mode must have been set to Angles and Orientations. For documents created before version 7.9 SP7, you need to change the measure mode by opening the extruded bar document, and then launching the Trimming Angles Measure contextual command on the Trimming Angles Management operation available in the Analysis stage.

Scraping Links / Videos :

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This command allows to enable or disable manual modification of the bill of material content. When it is activated, the cell content modification does not affect the template document. When it is disabled, the cell content modifications are transmitted to the template file which is also updated with these new values.

Creation stages / Use: Click the icon or select the Bill of material > Scraping... command from the drop-down menu.

When a cell content is modified, it background becomes yellow. This help to know which cell are not linked anymore with the template document information. On the tab document, the icon next modified cell on the table

allows you to move down to the

Modifications / Additional information: You can reset the initial value of a modified cell by using the contextual command Restore Value.

When creating a bill of material table into a draft document, all the modified cells of the bill of material document are also displayed with the yellow background on the draft.

Top Level Links/Videos:

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This mode lists the subsets and parts contained in the assembly without detailing the constituents of the subsets.

Creation stages / Use: Click the menu.

icon or select BOM > Top Level... from the drop-down

This command does not require any interaction from the user. The BOM is recalculated as soon as the mode is activated.

Multi-levels Links / Videos:

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This mode allows you to select the level of detail of each sub-set comprising the assembly. It is the default mode for a new BOM.

Creation stages / Use: Click the icon or select BOM > Multi-levels... from the dropdown menu.

This command does not require any interaction from the user. The BOM is recalculated as soon as the mode is activated.

Flat Links/Videos:

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The Flat BOM lists all parts of the assembly without taking into account the organization of subsets.

Creation stages / Use: Click the

icon or select BOM > Flat... from the drop-down menu.

This command does not require any interaction from the user. The BOM is recalculated as soon as the mode is activated.

Overview of Visualization commands During the creation of a project, in particular the designing of a part or assembly, it is often necessary to modify the graphic zone to improve user friendliness and to meet all needs. The Visualization menu contains all of the tools necessary for these display modifications (lights, zoom, render mode, view sharing, etc.). Layers Configure camera from a view Configure a visualization from a view Create lights: Point light Directional light by 2 points Beam light by 2 points Spot light by 2 points

Save a realistic image Pan view Revolve view Pivot view Cameras:

Top camera Front camera Perspective camera

Zooms: Global zoom Zoom by box

Define render mode Views: Split view Delete view

Graphic cross-section

Show

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This command allows to show hidden entities.

Creation stages / Use: Click the icon or select the Visualization > Show... command from the drop-down menu or hit the S key of your keyboard. Launching the command allows you to temporary invert the display, its shows the hidden entities and hides the visibles ones, you can pick an entity in order to hide it. Generally, this command is used with the Visualization > Hide... command which allows you to hide several entities.

In addition, the Show all, Hide all and Invert visibility (which allows you to hide the visible entities and shows the hidden ones) commands are available from the entities tree.

Hide

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This command allows to hide several entities.

Creation stages / Use: Click the icon or select the Visualization > Hide... command from the drop-down menu or hit the H key of your keyboard. Pick the entity to hide. Generally, this command is used with the Visualization > Show... command which allows you to hide several entities.

In addition, the Show all, Hide all and Invert visibility (which allows you to hide the visible entities and shows the hidden ones) commands are available from the entities tree.

Layer

This command allows you to create different layers in your document.

Creation Stages: Click the icon or select Visualization > Layer... from the dropdown menu. 1. Give a name to your new layer. 2. Enter a identifier to use

All the elements are created on the level 0 layer. It is possible to change this default value by defining it in the attributes by default command.

Additional information: You can change an element via the editing of its attributes.

Visualization from a view

This command saves the configuration of a current view for the purpose of calling it up later.

Creation Stages: Click the icon or select Visualization > Visualizations > Visualization from a view... from the drop-down menu. 1. Select the view to save (left button in the display area of the view) 2. Validate the command This preview could be used at any time by a right button in the display area, then by selection of the preview via the Visualizations sub-menu.

You are able to save as many views as necessary. The visualization keeps the exact configuration of the view (graphical cuts and filters activated or not, ...)

Top camera

This command allows you to modify the orientation of a view in order to switch it into a top view.

Use: Click the icon or select the Visualization > Cameras > Top Camera command from the drop-down menu.

This command does not require any interaction from the user. The top view is calculated upon activation of the command. This command is also available by contextual menu on the background.

Additional information: This top view is calculated from the absolute frame. To orient the view in Top View from any face, use the right button on this face and select the See According to Normal command.

Bottom camera

This command allows you to modify the orientation of a view in order to switch it into bottom view.

Use: Click the icon or select the Visualization > Cameras > Bottom camera command from the drop-down menu.

This command does not require any interaction from the user. The bottom view is calculated upon activation of the command. This command is also available by contextual menu on the background.

Additional information: This bottom view is calculated regarding the absolute frame.

Front camera

This command allows you to modify the orientation of a view in order to switch it into front view.

Use: Click the icon or select the Visualization > Cameras > Front Camera command from the drop-down menu.

This command does not require any interaction by the user. The front view is calculated upon activation of the command. This command is also available by contextual menu on the background.

Additional information: This front view is calculated from the absolute frame.

Back camera

This command allows you to modify the orientation of a view in order to switch it into a back view.

Use: Click the icon or select the Visualization > Cameras > Back camera command from the drop-down menu.

This command does not require any interaction from the user. The back view is calculated upon activation of the command. This command is also available by contextual menu on the background.

Additional information: This back view is calculated from the absolute frame.

Left camera This command allows you to modify the orientation of a view in order to switch it into a perspective view.

Use: Select Visualization > Cameras > Left camera command from the drop-down menu.

This command does not require an interaction by the user. The left view is calculated upon activation of the command. This command is also available by contextual menu on the background.

Additional information: This view is computed from the absolute frame.

Right camera

This command allows you to modify the orientation of a view in order to switch it into right view.

Use: Select the Visualization > Cameras > Right Camera command from the drop-down menu.

This command does not require any interaction from the user. The right view is calculated upon activation of the command. This command is also available by contextual menu on the background.

Additional information: This right view is computed from the absolute frame.

Perspective camera

This command allows you to modify the orientation of a view to switch it into a perspective view.

Use: Click icon or select the Visualization > Cameras > Perspective Camera command from the drop-down menu.

This command does not require any interaction from the user. The perspective view is calculated upon activation of the command. This command is also available by contextual menu on the background.

Additional information: This perspective view is computed from the absolute frame.

Isometric camera Links/Videos:

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This command allows you to modify view orientation to switch to an isometric view.

Use: Select the Visualization > Cameras > Isometric Camera command from the drop-down menu.

This command does not require any interaction from the user. The isometric view is calculated upon activation of the command. This command is also available by contextual menu on the background.

Additional information: This isometric view is computed from the absolute frame.

Conical Camera Links/Videos:

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This command allows you to modify view orientation by switching to Conical view.

Use: Select the Visualization > Cameras > Conical Camera command from the drop-down menu.

This command does not require any interaction from the user. The conical view is calculated upon activation of the command. This command is also available by contextual menu on the background.

Additional information: This conical view is computed from the absolute frame.

Camera by 2 points

This command allows you to create a camera by 2 points.

Creation Stages / Use: Click the icon or select the Visualization > Cameras > Camera by 2 points... command from the drop-down menu. Origin: Camera origin. Select a point.

Target: Camera's viewpoint. Select a point.

Vertical direction: Allows to define the camera orientation around the axis origin/viewpoint. Select a axis.

Field of view angle: Field of view angle of the Perspective Projection. You must select a "Perspective projection" cell to access this data.

A right click on the camera allows to replace it by a camera from view.

Camera from a view

This command allows you to create and parameterize a camera from the current view.

Creation Stages: Click the icon or select Visualization > Cameras > Camera from a view ... from the drop-down menu. 1. Select the reference view (left button in the view's display zone) 2. Validate the command This camera will be able to be used at any time by a right button in the display zone then selection of the camera via the Cameras submenu.

A right click on the camera allows to replace it by a camera by 2 points.

Point light

This command allows a point light to be created in your document. A point light lights in all directions from the source center.

Creation Stages: Click the icon or select Visualization > Lights > Point Light... from the drop-down menu.

Position: Select a point defining the light's position Color: Select the color diffused by the light. The pipet allows to have the Intensity: The light reflected at a point at the same intensity in all directions.

Types of shadows: None: No shadow will be given to the scene. Shadow map: This method is faster, but less precise. It can blur it without any consequence on the processing time. Ray-traced: It is an accurate method but takes more time to process. It is set by default. It can be blurred by defining a geometry for the light source, but the processing time is the much higher.

Shadow color: Allows to define the shadow color Attenuation: A light other than directional cannot light to an infinite distance. TopSolid allows attenuation factors to be added to take this reality into account. This is how this attenuation is managed:

From the popup menu of a light (via the Lights folder in the entity tree or directly on the light in the graphic area) you can: Switch a light on/off. Edit and therefore modify the settings of a non basic light. Basify a non basic light.

A document without user light is lit by work lights. These lights cannot be modified or deleted. When a user light is created, it is not active by default. The display can be switched between work light and user light via the command Realistic light.

Spot light

This command allows a spot type light to be created in your document. A spot light is like a cone of light.

Creation Stages: Click the icon or select Visualization > Lights > Spot Light... from the drop-down menu. Position: Target: Cutoff angle: This is the half angle of opening of your cone of light. On the boundary of this angle, the obscurity is total.

Half intensity angle: Allows the half light zone to be defined. At the boundary of this zone, the light intensity is divided by two then decreases until it is zero at the boundary of the cutting angle.

Color: Intensity: The light reflected at a point at the same intensity in all directions.

Light geometry: Allows coming closer to the actual geometry of the source. E

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From the popup menu of a light (via the Lights folder in the entity tree or directly on the light in the graphic area) you can: Switch a light on/off. Edit and therefore modify the settings of a non basic light. Basify a non basic light.

A document without user light is lit by work lights. These lights cannot be modified or deleted. When a user light is created, it is not active by default. The display can be switched between work light and user light via the

Additional information: The Exponent parameter (exponential factor) allows getting as close as possible to a spot lighting. It allows a uniform lighting to be avoided and to decrease the aliasing at the boundary of the light.

IES Light

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This command allows an IES type light to be created in your document. An IES light is a light file provided by some manufacturers. This file includes all light information (geometry, intensity,...)

Creation stages / Use: Click the icon or select Visualization > Lights > IES Light... from the drop-down menu.

1. Select a point defining the light's position. 2. Select a target point which will be sighted by the light. 3. Enter the IES file path. 4. Enter the Cutoff angle. This is the half angle of opening of your cone of light. On the boundary of this angle, the obscurity is total. this option can be empty if the light is multi directional. 5. Select the color diffused by the light. The pipet allows to have the same color than a shape, another light, ... 6. Select the intensity (see below for explanation). 7. Validate by clicking .

Available options: Intensity:

The light reflected at a point at the same intensity in all directions. Enter the value of the luminous flux or the power of the light. Also select the type of lamp (LED, halogen, incandescent, ...) If the From IES file option is checked, the luminous flux,the power of the light and the type of lamp are field by the IES file. they can't be changed.

Light geometry: Allows coming closer to the actual geometry of the source. Example: if you want to simulate a fluorescent tube, it is preferable to choose cylindrical geometry. It is recommended to use the geometry defined in the IES file by selecting IES in the drop-down list. The visible geometry option allows to show the lamp. It can also be hidden or shown with the contextual menu.

From the popup menu of a light (via the Lights folder in the entity tree or directly on the light in the graphic area) you can: Switch a light on/off. Edit and therefore modify the settings of a non basic light. Basify a non basic light.

A document without user light is lit by work lights. These lights cannot be modified or deleted. When a user light is created, it is not active by default. The display can be switched between work light and user light via IES files can be downloaded on light manufacturers website.

Sky light

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This command simulated both direct sunlight and ambient lighting from the sky. This radiation is much more diffuse than other light, providing much softer lighting.

Creation Stages / Use: Click the icon or select Visualization > Lights > Sky Light... from the drop-down menu. Sky light: Defines the various sky parameters. 1. Select the turbidity of the sky: a value near 0 indicates a clear sky, a vue near 10, a sky very polluting. 2. Specify the factor of albedo. It is the fraction of sun energy which is reflected by the floor. The more the surface is reflecting, the higher is albedo. 3. Specify the factor of saturation. This factor allows to modulate the sky color. A value of 100% corresponds to the color of a clear sky, a value near 0 corresponds to a grey sky. 4. Select the intensity by dragging the cursor or entering the value. A value of 100% corresponds to the intensity of a clear sky. A lower value allows to simulate a cloudy sky. 5. Indicate the direction of north. 6. Indicate the direction of the zenith. 7. Choose whether to enable shadows.

Sun: Defines the various sun parameters (position, color, and intensity). 1. Enter the azimuth and altitude, or click the Position calculator button. 2. Select the intensity by dragging the cursor or entering the value. A value of 100% corresponds to the intensity of sun with a clear weather. A lower value allows to simulate the sun veiled by clouds. Clouds: Defines the various clouds parameters. 1. Cumulus/Stratus: Density: percentage defining the density of clouds (compact, thick and tight). Opacity: percentage defining the opposition to the passage of light. 2. Cirrus: Type: cirrus type to use (5 types available). Opacity: percentage defining the opposition to the passage of light. 2. Luminosity: percentage of light emission. 3. Random seed: integer between 1 and 10000 to simulate a random position of clouds in the sky.

Colors of the sky and the sun are automatically defined regarding the sun position (orange in the morning or evening, blue during the day, ....) Clouds: position the mouse cursor on the Cumulus/Stratus button or on the Type field of Cirrus to see a preview of clouds.

Openings: If the sky light can pass through faces (windows, or others, ...), select them to reduce rendering calculations.

Environment

This command loads the environment to be reflected on your parts.

Use: Click the

icon or select the Visualization > Environment... command from the drop-down menu.

1. Select the environment to use from the drop down list. 2. Select the vertical direction of the environment. If the environment is a building, it is the ceiling direction. 3. Enter a tilt angle regarding this vertical, if needed. 4. Select the direction of the reference front direction. 5. Enter an azimuth angle regarding this direction, if needed. 6. Enter an intensity factor, if needed. Near 0, the environment will be dark, near 1, it will be bright. 7. Validate by clicking .

Example of an environment settings with the graphic handles.

An environment can only be reflected on the parts in a material which has a reflection coefficient.

Available Options: Activate the environment: This option, checked by default, activates the environment from its creation.

Overview: Field of view angle: This option allows to modify the conicity angle. As long as this command is active, the part or the assembly is displayed with a conical camera which takes in account this conicity. The minimum value is 30°

Additional information: Only opened Environment documents and those checked-in in a referenced library are available in the Environment document drop-down menu.

Background

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This command makes it possible to set the background for a Part or Assembly document from an image file (bmp, jpeg, png, tif,...).

Creation stages / Use: Select the Visualization > Background... command from the drop-down menu. 1. Enter the name of the background. 2. Select the background image file. 3. Validate the background creation by clicking the

button.

The active screen background image will only be displayed with realistic rendering types. The selected image file is included in the Part or Assembly document. Unlike the background environment, The background image is fixed regardless the camera orientation. The background image can be taken in account when calculating as realistic rendering by selecting the Activate background option: Screen background.

Available Options: The Enable Background option allows a default background to be set.

Modifications / Additional information:

Defined backgrounds are stored in the Background folder in the entity tree. The popup menu for the background allows the background to be enabled, edited, or deleted.

Rendering with background image

Realistic rendering

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This command saves your scene in the image format. This backup takes into account the materials and the coatings associated with the items as well as the shadows made by the lights.

Use: Click the

icon or select Visualization > Realistic Rendering... from the drop-down menu.

1. Select the view to save. 2. Validate the dialog. 3. Specify a destination directory and a file name.

You can stop a backup in progress by using the Esc key.

Available Options: Image: View to calculate: the view to calculate is the current view. Preset: Allows to quickly define all settings for the image calculation. Tree presets are delivered, and you can save your own settings . View size: The current view dimensions are used. The width and height can't be changed. Width / Height: Image size. The units used are pixels. Background: This option, when on, allows you generate an image with a transparent background (the backg the image will not hide the background of the page). Background can be: white Screen background: Actual screen background is used (degraded or background image) black environnement : The background environment is displayed as background. transparent: the image background is defined as transparent for all save formats which manage it (all ex Antialiasing: this cursor allows to smooth the elements border. Lighting accuracy: this cursor allows you to improve rendering quality by reducing the « noise » produced b lights and materials reflects. Improvement is similar to the one obtained by increasing antialiasing, but it is mu setting is only on if the scene includes complex lighting that is likely to be adjusted (radiosity, sky light, extend

Light accuracy with 10%

Light accuracy with 100%

Fast skylight: This parameter only calculates the indirect rays of the sky. This produces a smoothed rende

quickly, but this calcula on is approximate.

Example of an image computed in the scene with same settings Fast skylight = YES

Fast skylight = NO (it takes about 2 mor

Global Illumination: This option allows you to accurately simulate the ambient light reflected by the scene it longer only the direct light from luminous sources. In a classic image calculation, an area that is not directly lit by light is black. In reality, this area receives light walls and scene objects. Global illumination takes this effect into account and avoids obtaining unlit areas. This option is particularly useful for implementation and architecture images. (see images below). Global illumination accuracy: This option allows you to improve global illumination calculation by taking in little details. Generally, default value (15%) is enough. Post-processing: This option allows to apply a treatment to the calculated image. To complete the list, you m calculate the image with preview, in which the post-processing can be defined and saved. Then it is proposed image calculation (as background task for example).

Preview without Tone mapping

Preview with Tone mapping and intensity correction

Without Global Illumination

With Global Illumination

Overview: Scale: allows you to generate a preview smaller than final image (for example 50% for a preview half smaller, which allows you to faster calculate the preview). Right-clicking in the preview window allows you to save the calculated image in another format.

Display the rendering: Display a preview of the rendering.

Save: Format: Select the extension of the backup file, BMP, PNG, JPEG, TIFF, Radiance HDR and OpenEXR. Quality: Influences the overall quality of the image (set at 90 by default). Only available with the format .JPEG Background job: This option allows you to calculate rendering by a Rendering server running as background job. You can continue to work with TopSolid. The rendering server allows you to calculate photorealistic rendering by allowing the user to continue working with TopSolid. The rendering server is automatically launched when a image calculation is validated with «Background job» saved option. When the rendering server is running, its icon is displayed in Windows task bar (near clock) . When moving your mouse cursor on this icon, the server status is displayed. Particularly, if this image is under calculation, its progress status is indicated. When an image calculation finished, a tooltip is displayed on the rendering server icon .A click on this tooltip allows you to open this calculated image. A right click on this icon allows you to suspend or resume calculation in progress and to configure the rendering server. A double click on this icon allows you to display the in progress calculation list, to be able to reorder them or to cancel them. It also allows you to display calculated image history to be able to open them by double-click. Open image: If this option is activated, the resulting image will open automatically when the backup is complete.

Advanced: Recursion depth: Allows to set the shadow, the reflection and the refraction depths together. For example, if several mirrors reflect one in the other, with a value of 1, the shadow will be reflect in only one mirror. With a value of 2, this reflection can also be reflected in another mirror. This setting is only for beamed shadows. Ray cutoff: When a beam is reflected or refracted, part of its intensity is lost. When the intensity of a beam goes under the bottom value, this beam is no longer considered in the calculation of the image. This setting allows you to balance the duration and the accuracy of the calculation in scenes rich in reflection and/or refraction. Caustics: A caustic is the envelope of light rays reflected or refracted by a curved surface or object, or the projection of that envelope of rays on another surface Example of a caustic through a glass of water:

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This command allows to compute an image in 360° realistic rendering. This image can be visualized with a specific viewer (FSPViewer,...) or included in a web site.

Creation stages / Use: Select the Visualization > Panoram Rendering... command from the drop-down menu. This command use the same options than the Realistic Rendering command.

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This command allows to create a basic picture file with the render displayed on screen, without option and without using the realistic rendering command which needs a paid license but which is much more efficient and has a lot of rendering options.

Creation stages / Use: Click the icon or select the Visualization > Screenshot... command from the drop-down menu. 1. Select the view to calculate. 2. Uncheck View size and enter the width and the height of the selection rectangle to calculate only the selected area.This rectangle can be re sized and moved by selecting by its edges or its frame.The units used are pixels. 3. Select the background: This option, when on, allows you to generate a picture with a transparent background (the background color of the image will not hide the background of the page). Background can be: white Screen background: Actual screen background is used (degraded or background image) black environment: the background environment is displayed in the background. transparent : background image is defined as transparent for supported saved formats (all of them except JPEG).

4. Select the output: a file can be created by checking this option or by checking clipboard, the image will be copied automatically, then you are able to open any image editing software and paste this image. 5. If file is selected upper, select the picture format and also the compression quality for JEPG format. 6. Check the Open image option to open the calculated file with the Windows image viewer. 7. Validate to calculate the image by clicking on . 8. Enter the file destination path by clicking on Browse.

The generated file isn't linked to the view from which it is calculated

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Cette command allows to do a virtual visit inside an assembly document as if the user is walking inside it.

Creation Stages / Use: In an assembly document, click on the icon or select the command Visualization > Walk-through... from the drop-down menu. 1. Click a point into the graphic area to define the start position of the observer. 2. Click a second point to define the initial direction the observer is looking at. 3. Use the keyboard keys to move the observer (see the Available Options chapter for more details on the keys settings).

While moving with the keyboard, it is possible to use the middle button of the mouse to rotate the view ( looking up, down, ...).

Available options: View from top:

While selection the Origin and target points, you can tick this option to see the scene from the top.

Options: Character height: Allows to set the camera height according to the selected origin point (the origin point represents the feet position and the height gives the eye position). Field of view: Allow to define the angle of the conic view. This represents the angular field of view. To get a visualization similar to a human eye, you must set this value to 60°. Step length: Represents the distance traveled each time you press the "Forward" key. Max step height: Represent the maximal height that can be get over when using the "Forward" key without using the "Jump" key. Jump height: Represent the height that can be reached when using the "Jump' key. A jump apply a forward displacement (using the step length value) combined with a vertical displacement. Speed: This option allows to set the displacement speed while using the "Run" key. Detect collisions: If you untick this option, it will be possible to cross over obstacle. But it is still possible to climb up obstacle if they are smaller that the step height.

Displacement control settings: The displacement is made with the keyboard. The key setting is defined in "Tools > Options > Walk-through". Forward, backward, Left and Right: Each click apply a displacement equal to the step length. You can keep the key down to string steps together. Run : When clicking on this key, the "observer" keep moving forward at the defined speed. The displacement stops if an obstacle is met. Jump: Allows to jump on or over an obstacle if it is smaller than the jump height.

Selection by curve

This mode allows you to select all the items intersected by a curve.

Use: Click the icon or select Visualization > Selections > Selection by Curve... from the dropdown menu. Free hand draw the selection curve.

Point type items cannot be selected with this mode. Unlike the selection by area, all elements touch by this curve are selected.

A click in the graphic area followed by a cursor displacement (by keeping the button pressed) allows to create a rectangular selection. The frame creation direction is important. It allows to have a strict selection (all elements completely inside the selection frame are selected) or non strict (all element in contact or inside the frame are selected).These 2 modes are differentiated by the frame color and type of line. (blue and solid line for the strict mode, green and doted for the non strict mode).

Strict mode: only the circle is selected

Non strict mode: The 2 segments, the fillet and the circle are selected

Selection by area

This mode allows you to select all the items included in an area.

Use: Click the icon or select Visualization > Selections > Selection by area... from the dropdown menu. Free hand draw the selection area

Only the items included in the zone will be selected. Unlike the selection by curve, elements which are intersected by this area aren't taken into account.

A click in the graphic area followed by a cursor displacement (by keeping the CTRL key pressed) allows to create a rectangular selection. The frame creation direction is important. It allows to have a strict selection (all elements completely inside the selection frame are selected) or non strict (all element in contact or inside the frame are selected).These 2 modes are differentiated by the frame color and type of line. (blue and solid line for the strict mode, green and doted for the non strict mode).

Strict mode: only the circle is selected

Non strict mode: The 2 segments, the fillet and the circle are selected

Select by Attributes

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This command allows to select entities of the document based on their attributes (color, linetype, transparency, layer and rendering type).

Creation stages / Use: Click the icon or select the Visualization > Selections > Selection by Attributes... command from the drop-down menu. 1. Choose the selection mode of the attributes : this mode allows you to browse the tree structure of the entity. Entities: the attributes are searched at the top level of the entity. Parts of entities: the attributes are searched in the structure tree of the entity. Parts of an entity: the attributes are searched in the structure tree of one entity that you have to select. Example: Let's take a part made of are red shape included twice in an assembly document, if you make a selection with the red color: - The Entities mode allows to select the both shapes. - The Parts of entities mode allows to select the faces of the both shapes.

- The Parts of an entity mode allows to select the faces of one of the both shapes. 2. Choose the attributes to select (color, linetype, transparency, layer and rendering type). 3. Confirm the selection with the button, this selection can be saved thanks to the Selection... command.

Modifications / Additional information: The Wireframe rendering option is applied on shapes only, it can have 3 states: Unchecked: shapes in shading rendering can be selected only. Checked (tick): shapes in wireframe rendering can be selected only. Checked (square): shapes in shading and wireframe rendering can be selected.

Select by Type

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This command allows to select the different types of entities available in the document.

Creation stages / Use: Click the icon or select the Visualization > Selections > Selection by Type... command from the drop-down menu. Choose the entity type in the drop-down list (entities available in the document are displayed only). Confirm the selection with the button, this selection can be saved thanks to the Selection... command.

Selection of Shapes

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This command allows to select the different shapes of a document.

Creation stages / Use: Click the icon or select the Visualization > Selections > Selection of Shapes... command from the drop-down menu. Check the Topology type option if you want to select either solid shapes or surfacic shapes of the document. Check the Geometry type option if you want to select either exact shapes or faceted shapes of the document. Confirm the selection with the button, this selection can be saved thanks to the Selection... command.

Modifications / Additional information: Faceted shapes are made of triangular faces. Generally, they are coming from STL or IFC import, they can also be created with the Surfaces > Other > Conversion into Faceted Shape... command.

Existing Selections

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This command allows to display the selections list and choose one of them.

Creation stages / Use: Click the icon or select the Visualization > Selections > Existing Selection... command from the drop-down menu. Choose a selection in the drop-down list. The elements of this selection can be used when launching a new command.

In the entities tree, a selection can be chosen from the Selections folder and then the Select contextual command can be executed from the contextual menu.

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This command allows to define selections of elements and save them. These selections can be used in different commands where the Select contextual is available.

Creation stages / Use: Click the icon or select the Visualization > Selections > Selection... command from the drop-down menu. 1. Type the selection's name 2. Choose the elements in the graphic area or in the entities tree. 3. Confirm with the button.

The Ctrl key allows you to select several entities. The Shift key allows you to go upward in the entity structure (segment through sketch, edge or face through shape, etc...). The selections are saved into the Selections folder of the entities tree.

Modifications / Additional information:

When a command is launched, you can choose one of the selections with a right click in the graphical area, it displays the Selections contextual sub-menu. When no command is launched, you can choose a selection with 3 different ways: From the Selections contextual sub-menu displayed when you make a right click in the graphical area. From the Selections folder of the entities tree using the Select contextual command. From the Visualization icon bar when you launch the Existing Selections... command. For example, it allows to select all the red surfaces of a document and launch the sewing command. Example of access to the Selections menu when no command is launched:

Filter faces This mode allows to filter using automatic detection, the faces of the shapes when the cursor of the mouse intersects the latter. By activating this mode, faces are no longer selectable, it is easier to select other entities (points, edges, sketch, ...)

Use: Click the icon or select Visualization > Selection Filters > Filter Faces... from the drop-down menu.

This filter can be cumulated with the Edges filter, Unsafe items filter and with one of these 3: Filter by color, Filter by properties, Filter by entities.

Filter edges This mode allows to filter using automatic detection, the edges of the shapes when the cursor of the mouse intersects the latter. By activating this mode, the edges are no longer selectable, it is easier to select other entities (points, faces, sketch, ...)

Use: Click the icon or select Visualization > Selection Filters > Filter Edges... from the drop-down menu.

This filter can be cumulated with the faces filter, Unsafe items filter and with one of these 3: Filter by color, Filter by properties, Filter by entities.

Facetted Shape Vertex Selection

This command activate the option that allows to Selection Facetted shape vertex.

Creation stages / Use: Select the Visualization > Picking filter > Facetted shape vertex selection... command from the drop-down menu.

This option is only available for the dimension. It is not available for the annotations.

Filter unsafe items

This mode allows to filter automatic detection of faces whose hooking could not be assured throughout the part life cycle.

Creation stages / Use: Click the icon or select the Visualization > Picking filters > Filter Unsafe Items command from the drop-down menu.

This filter can be cumulated with the Faces filter, Edges filter and with one of these 3: Filter by color, Filter by properties, Filter by entities.

Modifications / Additional information: Example of use: When a geometry is split into two, with a groove operation, an operation may not hook to one of the resulting faces if the groove is changed or deleted, which may lead to an invalid operation. Activating this filter we make sure to not use these faces.

In the above example, all the yellow faces cannot be selected when the Filter Unsafe Items mode is enabled

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When you select an element from the entities or operations tree, this mode allows you to display an arrow that point out the element in the graphical area.

Creation stages / Use: Select the Visualization > Picking Filters > Echo Arrow in Trees command from the drop-down menu. This command is a mode, if this mode is activated, an echo arrow is displayed in the graphical area when an element with a graphical representation is selected in a tree (entities or operations).

This mode is not available in a Drafting or a Drawing document as well as documents without Visualization menu.

Modifications / Additional information: The origin of the arrow is always located at the center of the graphical area.

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When you select an element from the dialog of a command, this mode allows you to display an arrow that point out the element in the graphical area.

Creation stages / Use: Select the Visualization > Picking Filters > Echo Arrow in Dialogs command from the drop-down menu. This command is a mode, if this mode is activated, an echo arrow is displayed in the graphical area when an element with a graphical representation is selected from the graphical area or from the entities tree.

This mode is not available in a Drafting or a Drawing document as well as documents without Visualization menu.

Modifications / Additional information: The origin of the arrow is always located at the center of the graphical area.

Filter by color This command allows you to create a visualization filter according to a color. This filter allows to show or hide only entities with this color.

Creation Stages / Use: Click the icon or select Visualization > Filters > Filter by Color... from the drop-down menu. 1. Select the color of the filter. 2. Validate. When a filter is active, the icon appears on the upper right of the graphic area. To deactivate all filters, click this icon.

You can accumulate several filters You can turn off a filter by right-clicking - Remove a filter in the graphic area. You can turn off all filters with one right-click - Remove all filters in the graphic area.

Several filters can be created. They are listed in the Filters folder of the entities tree. To use them, just drag them in the graphic area. It is also very easy to create a BOM of some parts or of an assembly by defining before a filter for these parts.

Available Options:

Entities to remove: Selected entities: With is option, all selected entities will be removed by the filter. Unselected entities: With is option, all unselected entities will be removed by the filter.

Filter color: Select the filter color. All entities with this color will be filtered.

Additional information: Only the elements matching the filter will be visible in the graphic area.

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This command allows you to create a visualization filter on entities. The selection mode allows you to refine the rotating selection.

Creation stages / Use: Click the icon or select the Visualization > Filters > Filter by entities... command from the drop-down menu. 1. Enter the filter name. 2. Activate or don't activate the filter. 3. Select if entities to take in account in the filter are those selected or those non selected. 4. In the drop down list, you can also directly select parts and assemblies to consider. 5. Validate by clicking .

You can accumulate several filters You can turn off a filter by right-clicking - Remove a filter in the graphic area. You can turn off all filters with one right-click - Remove all filters in the graphic area. From the entities tree, drag the filter into the graphic area to activate it. Entities can be selected from the graphic area or by checking them in the drop-down list.

Available Options: Entities to remove: Selected entities: With this option, selected entities will be removed from the filter. No selected entities: With this option, no selected entities will be removed from the filter.

Hide: The box allow to hide selected entities during the use of the command, to be able to select other entities more easily, especially those who were behind.

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This command allows you to use a filter document. This Filter document is a document which allows to filter by searching properties and conditions. For example, it is possible to filter all hexagonal head screws with a diameter lower than 6mm.

Creation stages / Use: Click the icon or select Visualization > Filters > Filter by properties... from the drop-down menu. 1. 2. 3. 4.

Enter the filter name. Activate or don't activate the filter. In the drop-down list, select the filter document to use. Validate by clicking .

When a filter is activated, the icon appears upper right of the graphic area. To deactivate the filters, click this icon.

You can accumulate several filters You can turn off a filter by right-clicking - Remove a filter in the graphic area. You can turn off all filters with one right-click - Remove all filters in the graphic area. From the entities tree, drag the filter into the graphic area to activate it.

Several filters can be created, they are listed in the Filters folder of the entities tree. To use them, just drag them in the graphic area. It is also very easy to create a BOM of some parts or of an assembly by defining before a filter for these parts.

Available Options: Entities to remove: Selected entities: With this option, the selected entities (the entities which have the property) will be removed by the filter. No selected entities: With this option, the none selected entities (the entities which don't have the property) will be removed by the filter.

Cut by Planes

This command allows you to make a graphical cut of the entities by one (or several) planes.

Creation Stages / Use: Click the

icon or select Visualization > Cut by planes... from the drop-down menu.

1. Select the reference plane. 2. Enter an offset or select a passing point. In this case, this point will indicate the offset of the cut plane. 3. Modify the options if necessary. 4. Validate the dialog.

The graphic cut is not possible when realistic rendering is activated.

In case of offset or passing point, the offset plane used for cut will be parallel to the reference plane.

Available Options: X Rotation: Allows rotating, the cut plane around the X axis by the value given.

Y Rotation: Allows rotating, the cut plane around the Y axis by the value given.

Cut color: Should the closure display option be active, the cut plane will be in the color specified by the user.

Cut hatches: Type: Allows to select hatches to be displayed of the cut faces. Orientation: Allows to enter the hatch orientation.

Entities: This dialog allows you to select the entities concerned by the cut. All entities: All the entities are cut (default mode), this option is useful when the other modes have been used. Selected entities: All the selected entities are cut, the other ones are not cut. Unselected entities: All the selected entities are not cut, the other ones are cut. Hide: This option allows you to temporary mask the selected entities in order to be able to select the ones located behind them.

Second and third cut:

Allows to define a second and a third cut plane on the same cut, with the same kind of settings (plane, offset, rotation, color, hatches, ...) as upper.

Display cut: If this option is unchecked, the parallel faces behind the cut plane are not displayed. The parts are hollowed like if they were surfaces. If this option is checked, the 2 options below are ungrayed, and the cut will be displayed with the selected color and hatches. Use shapes color: If this option is checked, the cut planes color defines upper will not be used. The cut faces color will be the part color. Automatic hatching: If this option is checked, the hatch orientation defined upper will not be taken in account. Hatches will be oriented ramdomly (very useful in an assembly).

Display cut edges: When the command is validated, the cut faces edges are thickened to visualize them properly.

Preview cut edges: During the dynamic preview, the cut faces edges are thickened to visualize them properly.

Enable cut: If this option is unchecked, by validating this command, the Cuts folder and the cut are created in the entities tree but will not be activated in the graphical area. In this case, to show cut parts, you have to double-click the Cut icon in the Cuts folder of the entities tree.

When we have a big assembly, it is recommanded to uncheck the option : Preview cut edges. This option can slow the system.

To edit the current cut and modify it, use the Edit current cut command by clicking the icon in the graphic area. It is possible to deactivate a cut by using the Delete contextual menu or by using the icon. in the graphic area. It is not possible to accumulate several cuts. Activation of a second cut will automatically cause the deactivation of the current cut. To activate an existing cut, drag it from the cuts folder of the entities tree to the graphic area.

Example with a blue cut color:

Cut by Profile

This command allows to make a graphical cut on a 3d document with an open sketch.

Creation stages / Use: Select the Vizualisation > Cut by profile... command from the dropdown menu. 1. 2. 3. 4.

Select the profile Modify the direction of cut if necessary. Modify the options if necessary. Validate the dialog.

The graphic cut is not possible when realistic rendering is activated.

The profile must be open to make the cut.

Available options: Cut color: Should the closure display option be active, the cut plane will be in the color specified by the user.

Cut hatches: Type: Allows to select hatches to be displayed of the cut faces. Orientation: Allows to enter the hatch orientation.

Display cut: If this option is unchecked, the parallel faces behind the cut plane are not displayed. The parts are hollowed like if they were surfaces. If this option is checked, the 2 options below are ungrayed, and the cut will be displayed with the selected color and hatches. Use shapes color: If this option is checked, the cut planes color defines upper will not be used. The cut faces color will be the part color. Automatic hatching: If this option is checked, the hatch orientation defined upper will not be taken in account. Hatches will be oriented ramdomly (very useful in an assembly).

Display cut edges: When this option is checked, cut faces edges are thickened to visualize them properly.

Enable cut: If this option is unchecked, by validating this command, the Cuts folder and the cut are created in the entities tree but will not be activated in the graphical area. In this case, to show cut parts, you have to double-click the Cut icon in the Cuts folder of the entities tree.

For big assemblies, it is recommended to not check the Display cut edges option. This option might slow down the performance of the system.

To edit the current cut and modify it, use the Edit current cut command by clicking the

icon in the graphic area.

It is possible to deactivate a cut by using the Delete contextual menu or by using the icon. in the graphic area. It is not possible to accumulate several cuts. Activation of a second cut will automatically cause the deactivation of the current cut. To activate an existing cut, drag it from the cuts folder of the entities tree to the graphic area.

One view This command allows you to quickly switch your graphic zone into a view. Useful when the graphic zone consists of multiple views. done with the Two views, Three views, Four views or Split view commands.

Use: Click the icon or select the Visualization > Views > One view... command from the drop-down menu.

Two views This command allows to split into two views, the current document display. It is then possible to have simultaneously a 3d view and a top view of the same document.

Creation Stages / Use: Click the icon or select the Visualization > Views > Two views... command from the drop-down menu.

It is possible to resize the views by dragging the separator. To have again only one vue, use the Visualization > Views > One view...command.

Three views This command allows to split into three views, the current document display. It is then possible to have simultaneously a 3d view a left and a top view of the same document.

Use: Click the icon or select the Visualization > Views > Three views... command from the drop-down menu.

It is possible to resize the views by dragging the separator. To have again only one vue, use the Visualization > Views > One view...command.

Four views This command allows to split into four views, the current document display. It is then possible to have simultaneously a 3d, a left, a front and a top view of the same document.

Use: Click the icon or select the Visualization > Views > Four views... command from the drop-down menu.

It is possible to re size the views by dragging the separator. To have again only one vue, use the Visualization > Views > One view...command.

Split view

This command splits a view horizontally or vertically into two.

Use: Click the icon or select the Visualization > Views > Split view... command from the drop-down menu. A dashed line appears dynamically. Click the area where you wish to make the separation.

By moving the mouse cursor on the vertical boundaries of the view, the dashed line is horizontal. By moving the mouse cursor on the horizontal boundaries of the view, the dashed line is vertical. If your document is split into two views, only the current view has a black framing around it To delete the split view, use the Delete view command.

Delete views

When your graphic area has several views done with the Two views, Three views, Four views or Split view commands, this command allows to delete one of them.

Use: Click the icon or select the Visualization > Views > Delete view... command from the drop-down menu. Select the view to delete. The view that will be deleted is symbolized by a red cross.

When only one view is remaining on the screen, this command is not available.

Pan view

This command allows you to dynamically move your view into translation.

Use: Click the icon or select the Visualization > Views > Pan view... command from the drop-down menu. Keep the left button pushed down and pan your view. To leave this command after the displacement, right click Ok, or use the Esc key.

The right mouse button also allows to use this command regardless the current command.

Rotate view

This command allows you to dynamically rotate your view around a point.

Use: Click the icon or select the Visualization > Views > Rotate view... command from the drop-down menu. Keep the left button pushed down and revolve your view. To leave this command after the displacement, right click on Ok, or use the Esc key.

The middle button also allows you to use this same command regardless of the function currently in use.

Additional information: The center of rotation corresponds to the center point of the view.

Spin view

This command allows you to dynamically rotate your view around an axis.

Use: Click the icon or select the Visualization > Views > Spin view... command from the drop-down menu. Keep the left button pushed down and pivot your view. To leave this command after the displacement, right click on Ok, or use the Esc key.

Additional information: The rotation in made around the normal axis of the center of the view.

Lock view

This command allows you to lock a view. A locked view can not be subject to any movement (zoom, rotation, translation, etc.).

Creation Stages / Use: Click the icon or select the Visualization > Views > Lock view... command from the drop-down menu.

When a view is locked, zoom, orientations and cameras icons are grayed. To unlock a view, you just need to re-select the Lock view command.

Zoom to fit

This zoom allows you to resize a screen view so as to fully visualize all the project items.

Use: Click the icon or select Visualization > Zoom to Fit from the drop-down menu.

This command does not require any interaction from the user. The zoom to fit is calculated on the current view upon activating the command. This command can also be used with the CTRL+MAJ+Z shortcut.

It is possible also possible to double-click the mouse wheel to zoom to fit.

Zoom by box

This zoom allows you to focus on a zone of the current view by enclosing the area to zoom on.

Use: Click the icon or select Visualization > Zoom by Box... from the drop-down menu. Press your mouse's left button to define the framing borders which will be the limits of the view after zooming. Release the left button to display this zoom.

Define render mode

This command defines the type of render mode to apply to the view.

Use: Click the Render modes icons on the right of the graphic area or select the Visualization > Render modes > ... commands from the drop-down menu. Shaded renderings Shade render mode allows you to visualize the scene with the item faces filled in, thus providing a realistic type of visualization (using what is called the "Gouraud" method). Name

Shadow rendering with edges

Shadow rendering with dotted hidden edges

Shadow rendering

Shadow rendering with hidden wireframe

Constant shadow rendering

Description Fill in faces. The edges are displayed. If sketches are visible, they cross the geometry.

E

Fill in faces. The edges are displayed. Hidden edges are visualized with dashes. If sketches are visible, they cross the geometry. Only the filling of the faces is displayed. The edges are not displayed. If sketches are visible, they cross the geometry.

Only the filling of the faces is displayed. The edges are not displayed. If sketches are visible, they are interrupted by the geometry. Calculate a unique illumination value for each facet. The edges are not displayed. If sketches are visible, they cross the geometry.

Realistic renderings Name

Description

E

Realistic rendering with edges

The materials and the coatings associated with the items are taken into account. The edges are displayed.

The materials and the coatings associated with the items are taken into account. Realistic rendering

Realistic rendering with effects

The materials and the coatings associated with the items are taken into account as well as the shadows made by the lights.

Realistic rendering with effects and edges

The materials and the coatings associated with the items are taken into account as well as the shadows made by the lights. The edges are displayed.

Progressive Ray Tracing

The Progressive Ray Tracing mode allows to calculate an image on the whole document’s graphics area without blocking the use of the software commands. The rendering parameter settings are available via an icon on the top right of the graphics area. These settings are retained when calculating an image using the Visualization > Realistic Rendering … command.

Wireframe renderings Name

Description Visualization of the items by their edges. All the edges are visualized.

Wireframe rendering Visualization of the items by their edges. The hidden edges are not visualized. Wireframe rendering without hidden lines Visualization of the items by their edges. Hidden edges are visualized with dashes.

E

Wireframe rendering with hidden lines as dashes

Zebra rendering Name

Zebra rendering

Description Visual verification of the continuity and the tangency of surfaces.

E

Display shapes only Links / Videos :

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This mode allows to display shapes entities only (solid or surface). The wireframe entities (sketch, points, axes,…) will be automatically hided.

Creation stages / Use: Click the icon or select the Visualization > Display shapes only... command from the drop-down menu.

When this mode is active, the icon background is orange.

Display lateral faces

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With a sheet metal part, this mode allows to visualize faces following the thickness (a specific color is applied to these lateral faces). This mode only functions with shaded renderings.

Creation stages / Use: Click the icon or select the Visualization > Display lateral faces... command from the drop-down menu.

When this mode is active, the icon background is orange.

Display lateral faces Active mode

Non-active mode

Realistic lighting Links / Videos:

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This command automatically activates the user lights and at the same time deactivates default.

Use: Click the icon or select the Visualization > Realistic lighting... command from the drop-down menu.

To visualize the realistic lighting in your part or assembly document, you must be with the realistic rendering, with a conical perspective and the document must have an environment. To deactivate the realistic lighting, just click again the same icon.

Background nvironment Links/ Videos:

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This mode allows you to view the environment as screen background.

Creation Stages / Use: Select the Visualization > Background environment... mode from the drop-down menu.

To view the environment in a screen background on the part or assembly document, you must absolutely be in realistic rendering mode so that the document has an environment and is in conical perspective.

To hide the environment, simply click a second time on this mode. Unlike the background image, the environment "follows" the camera orientation. This environment can be taken in account during the realistic rendering calculation.

Rendering with environment background

High-quality shadows Links / Videos :

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This mode allows to display shadows very accurately.

Creation stages / Use: Click the icon or select the Visualization > High-quality shadows... command from the drop-down menu.

When this mode is active, the icon background is orange.

Image in realistic rendering without high-quality shadows

Image in realistic rendering with high-quality shadows

Realistic reflections Links/Videos:

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This mode allows to display reflects a bit more realistic during your work and the visualization in the document. It is not an image calculation, but a mode of work. Reflects are more realistic by calculating the image.

Creation stages / Use: Click the icon or select the Visualization > Realistic reflections.... command from the dropdown menu.

To visualize the realistic reflections in your part or assembly document, you must be with the realistic rendering. An environment can be displayed or not.

Realistic reflections activated.

Realistic reflections deactivated.

Analyze Links / Videos :

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This command allows to analyze an element by picking or when moving the cursor over the elements.

Creation stages / Use: This command can be launched by clicking on the icon, or by hitting the F8 key, or by selecting the Analyze > Analyze... command from the drop-down menu. 1. Select an element or check the Dynamic option to display the analyze in a tooltip. 2. In the Categories area, choose the information to display in the Result area.

For more complex entities, you can use the Shift key to analyze the higher-level elements (segment -> sketch, edge -> shape, face -> shape…)

Available options: Dynamic: This options allows to make the analysis when moving the cursor over

the elements and display the result in a tooltip. However, when this mode is checked, you can pick an element in order to display its information in the Result area.

Categories: Function: allows to display the parameter of a function provided by the element. Property: when a part has been selected, it allows to display the author, the material characteristics, the physical properties of the element. Information : allows to display the description and the comment entered with the Information command. Attribute: allows to display the color (RVB), the linetype, the layer, the transparency et the rendering type of the element. Topology: allows to display the element type (vertex, edge, face,...) of the element and its characteristics (number of vertex, loops, edges,...). Geometry: allows to display the geometry type of the element and its dimensions (coordinates, length, radius, diameter, aperture angle,...). Extent: allows to display the size of the enclosing box of the element.

By default, dimensions are indicated according to the absolute frame. If you want to make an analysis according to a specific frame, you have to hook the compass on this frame.

Advanced Options: Accuracy: allow to define the number of digit to display, enter a value between 0 to 10. Display length unit: allows to display or hide the lenght unit in the Geometry and Extent categories.

Modifications / Additional information:

You can copy the information from the Result area in order to paste them into another application. During the analysis of a shape (solid or surface), the number of shells corresponds to the internal and external area of the shape. Then, a simple solid block have contains 2 shells whereas a surface have one shell only. The number of facets corresponds to the number of graphical facets, these facets are triangular facets. For example, during the facettisation of a simple block, the rectangular facets are made of 2 triangular faces, so it has 12 facets.

Analyze geometry Links/Videos:

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This command measures the entities in order to obtain the