Introduction To Pre Processing With ANSA [PDF]

Zitiervorschau

Introduction to pre processing with ANSA Training handouts

www.beta-cae.com www.beta-cae.com

2

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

About this document This course introduces participants to the basics of pre processing with ANSA. The covered topics include CAD translation and import, geometry handling, surface and volume mesh generation and improvement, model assembly, basic solver entities and an introduction to EPILYSIS solver. Upon course completion, the participant will become familiar with the ANSA interface and able to accomplish the essential steps needed to deliver a meshed file that can be used for structural analysis applications.

Who is this guide for? This guide is ideal for the user that encounters ANSA for the first time. For the engineer who is familiar with CAE terminology, but not familiar with ANSA interface. If you want to find your way around ANSA interface, but don't know quite where to start, this guide will familiarize you with the basic window panels of ANSA interface.

3

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Overview Main terms and GUI • Reading CAD data • Geometry healing • Middle surface extraction • Model browser • Surface Mesh • Batch Mesh • Handling non-geometry mesh • Improving the result of middle surface extraction • Depenetration • Volume Mesh • Assembly • Model Management – Introduction to pre processing decks • EPILYSIS: set up and run a model for static analysis in ANSA •

4

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Main terms and GUI

www.beta-cae.com www.beta-cae.com

ANSA GUI overview Modules 1. Main pull down menus

2. Toolbars 10. Search engine

8. Database browser

5. Hidden buttons pop-up

11. Hidden window 4. Module buttons group

9. Status bar 6. ANSA info

3. Module buttons

7. Command line

6

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

View control using mouse Rotate perpendicular to mouse track Ctrl

Rotate perpendicular to the screen

+

Ctrl

+

Rotation axis

Zoom with mouse wheel or

Translate OUT

Ctrl

Ctrl

+

+ IN

Ctrl

+

Shift

View control is faster when both Ctrl and Shift are pressed, as certain items are not drawn during the movement (dynamic view)

7

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

View control using the keyboard Standard views

Step rotations

Pan

8

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

The use of mouse buttons

The LEFT mouse button is used to:

The MIDDLE mouse button is used to:

The RIGHT mouse button is used to:

➢Activate

➢Declare

➢Perform

module/menu buttons

➢Select/define

entities

function

the opposite action of left mouse (e.g. select/de-select or insert/delete).

➢Zoom

➢Reapply

➢Cancel

the end of selections

the currently activated

in/out (in case of wheel

the last action

mouse)

➢Deactivate

➢Move

➢Pick

color bars, color legend, elements index on the drawing area (requires to keep the button pressed for a while)

a function

closest position

➢Access

right click menu in lists

➢Activate

hidden windows, select buttons to place them on desktop

9

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Color view modes From a switch button in the Drawing Styles toolbar, choose how to draw the items of the model.

The most usual color view modes are:

ENT: According to orientation

PID: According to property. Note for LS-DYNA: The property corresponds to *PART and *SECTION

MID: According to material

The colors of properties and materials are listed and controlled from the corresponding lists. PIDs and Mats lists can be quickly accessed from the Containers toolbar

10

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Entities visibility: detail on demand effect By default, some details of a model become invisible as the user zooms out of the model (e.g. hot-points or dense mesh disappear). Graphics performance when handling large models is thus improved. Zoom-out

Zoom-in

In order to adjust the level of detail that is displayed, press F11 or the Quality Criteria button from Utilities toolbar and switch to the Presentation Parameters tab of the window that opens. Moving the slider of Detail on Demand effect to the left, more detail is displayed (recommended for new users). F11

Moving the slider of Detail on Demand effect to the left, more detail is displayed (recommended for new users).

or

11

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Selecting items Single selection: To select, press the left mouse button over or close to each entity. Selected entities become highlighted. To deselect a selected entity, use the right mouse button. Confirm the end of selection with the middle mouse button.

Box selection: For functions that support box selection, press and hold the left mouse button. Drag the mouse in order to define a rectangle. Entities that lie inside the rectangle are selected. Box deselection is done in the same manner, using the right mouse button. Confirm the end of selection with the middle mouse button.

Ctrl

+

A

: Select all the visible entities in the screen

Ctrl

+

L

: Deselect all the visible entities in the screen

12

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Feature selection tools When activating a function that requires selection of entities (e.g. nodes, elements etc.) a toolbar with feature selection tools opens. When picking of entities with single or box selection is not convenient, one of the available tools can be deployed. Toolbar for elements selection

Toolbar for nodes selection

The most important selection methods are: Feature Area: It is the area of elements between whom the angle that is formed at their common edge is less than the given feature angle. Picking a single element, the whole feature area gets selected.

Feat. Angle

PID region: Picking an element with a particular PID, all the connected visible elements of the same PID get selected.

13

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Feature selection tools (2) Poly Area: Picking individual elements, all the elements enclosed in the path that is formed among the picked elements get selected. Confirmation with middle click is needed.

Poly Line: Picking individual elements, all the elements along their connecting path become selected. Confirmation with middle click is needed.

Feature Line: It is the line of consecutive edges, whose corner angle is less than the specified one. Picking a single edge, the whole feature line of edges or of their nodes gets selected. The direction of the feature line, depends on which end of the edge is picked.

Corner Angle

14

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Feature selection tools (3) Path: Picking two edges or nodes, the shortest path of edges/nodes that connects them gets selected. Confirmation with middle click is needed.

Loop: Picking a single node of an internal opening, all the nodes of the opening get selected. The Loop tool is applicable not only for openings, but for any kind of closed chain of entities.

Nodes/Entity nodes: Whenever it is needed to select nodes, the user can select them either directly or by selecting elements that use them (Entity nodes option). Switching to Entity nodes, the feature selection tools for elements becomes available. Confirmation with middle mouse button is necessary

15

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Focusing on items - Or

The Focus toolbar, located at the bottom area of ANSA main window, provides functions to isolate regions of the model. These functions can be applied on single entities (e.g. faces), on items with the same PID or MID etc., according to the status of the respective Feature Selection toolbar selected button (ENT-PID-MID etc.). ! This aforementioned switch button is similar to the switch button of the color view modes. Do not confuse the use of these two buttons. E.g. drawing per PID color can be combined by focusing per entity without any problem.

Or: Logical operation for the selection of items to remain visible. No selection confirmation is necessary. Result of the application depends on the selection. E.g. If a yellow CONs is selected, only the 2 faces that have this CONs as boundary remain visible.

16

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Focusing on items: And - Not And: Makes the neighbors of the selected entities visible. Result of the application depends on the selection. E.g. If yellow Cons are selected, only their neighboring faces become visible.

Not: Hides the selected entities. Result of the application depends on the selection. E.g. If a yellow CONs is selected, only the 2 faces that have this CONs as boundary are removed from visibility.

17

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Focusing on items: !Not !Not: Logical operation for the selection of multiple items to remain visible. 1-2: Select first with left mouse button 3: The selected items are hidden. Confirm end of selection with middle mouse button. 4: Only the selected items become visible.

1

3

2

4

Using the right mouse button in Or, And, Not and !Not, the opposite action is performed:

In GUI settings>Mouse/Keyboard window, if the option “Double click for PID selection (focus Group))is active, then by selecting with double click in Or, And, Not and !Not, whole properties get selected, even if focusing is set to be done by ENTs.

18

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Focusing on items: Neighb Neighb>1st Level: Brings to visible the first neighboring items connected to the already visible ones.

Neighb>All: Brings to visible all the neighboring items connected to the already visible ones (equivalent to pressing repeatedly the Neighb [1st Level] function until no more entities are brought to visible).

19

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Focusing on items: Near Near: Brings to visible all items near the nodes/points of the selected visible entities, that lie within a specified distance no matter if they are connected or not. The default search distance is 10.

The search distance can be modified from the Radius field in the Options List window.

If the Dense search option is active, function searches not only near the nodes/points but through the whole surface of the selected faces

20

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Focusing on items: Invert – All Invert: Visible items are hidden and vice-versa.

All: Brings everything to visible.

21

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Focusing on items: Lock If Lock is activated, then, when pressing All, only the entities that were visible at the time when Lock was activated remain visible.

Disabling Lock, the information of the previously locked entities is lost In order to keep one or more locked views in memory, use Store Lock: 1: Isolate entities in the screen. 2: Apply Lock>Store Lock 3: Specify a name for the locked view. 4: After changing the visible entities on the screen, at any moment invoke Lock>Manage Locks. 5: In the list that opens, select the previously created view and press Show Only. 3 1 2 4

5

While the Lock flag is activated, all the stored locks, appear also under the All function as sub-options

22

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Resolution The appearance of Cons and Curves depends on the Resolution values [1,2]. Big resolution => Curved lines are depicted with few straight segments. The curvature is not obvious. Resolution values are specified in the Options window invoked by Windows>Settings [3]. They affect all the visible entities. 1

2

CONS Resolution Length = 20

CONS Resolution Length= 2

3

The resolution of individual Cons or Curves can be changed, activating Auxiliaries>Fine from TOPO menu. Leftclicking on a Cons increases its resolution, while right-clicking decreases it. Clicking on a crosshatch of a face, all its Cons are affected: Fine

Fine

The resolution corresponds to the initial node density for mesh generation. Small resolution gives a more clear view of the model and is convenient for new users when working in TOPO. Nevertheless, when switching to MESH menu, the resolution should be set equal to the target element length. 23

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Topology tolerances If a CAD file that is opened in ANSA doesn't contain any information about connectivity of the part's faces, a model consisting of unconnected faces (red Cons only) is obtained. Applying TOPO>Faces>Topo, the faces get connected based on proximity, resulting in a model containing also yellow and, in some cases, cyan Cons.

How does ANSA decide if two Cons or Hot points lie close enough to consider them connected? There are two tolerance values: Hot points matching distance and CONS matching distance. These distances are depicted with two white lines at the lower left corner of the graphics area. As these values are usually small, zoom in a lot in order to see the white lines [1]. The tolerance values are specified in Tools>Settings>Resolution/Tolerances/Units [2]. 1 2

24

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Measurements 1. The Measure tool is invoked from the respective toolbar button in the Utilities toolbar. 2-3. Pick two nodes. In the Results section of the Measure window, the user can select among the available measurements. By default the distance is displayed. 4. Picking one more node, other measurements become available. By default, the angle is displayed. 5. Confirm the end of selection for one measurement with middle click. After this, selection of entities for a new measurement can be done. ! Exiting the window (with Esc or with another middle click), the measurements are discarded, unless Store has been pressed in the Measure window [6]. Stored measurements are listed in the Database Browser. Measurements between entities of different type: E.g. to measure the distance from a node to a CONS: 1. Pick a node 2. In the Selection section of the Measure window, switch the radio button to CONS/Curves 3. Pick a CONS. The minimum distance between the node and the CONS is displayed.

1 4

2 3

6

5

2

1 3

25

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Hidden buttons and menus

When an arrow is displayed next to the name of a group of functions, this means that it contains hidden buttons.

Left click on the group name, to acquire quick access to the hidden buttons

Right click on the group name, to open a menu with the hidden buttons.

Having opened the hidden menu, right click on a button to move it from the main menu to the hidden menu and vice-versa.

26

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Search Engine The Search Engine can work as a function finder, providing an easy way to activate a function without searching its button among the numerous menu buttons. Just type some letters that are related to the function and choose among the given suggestions:

There is no need for literal match between the characters that are typed and the name of the ANSA function. In the example, the function that creates ELEMENT_DISCRETE for LS-Dyna is suggested by typing the word “bush”.

In order to access the history of the last applied functions, click on the arrow at the right side of the search engine widget.

27

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Dock - Tab windows In order to dock a window drag it from its header to one side of the ANSA GUI and wait a couple of seconds till a preview of the location where the window will be docked is displayed. Drop the window.

Preview

Drag

Drop

After docking a window once, double click on its header to un-dock or re-dock it in the last position. In order to tab a window in another window that is docked, drag it from its header to header of the target window. Wait till a preview of the tab is given. Drop the window. In order to un-tab the window, right click on its tab and choose the respective option. Alternatively, drag the tab out of the window.

Drag

Drop Preview

28

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Tips for windows handling Expand: A window that has a scroll bar can be temporarily expanded. Press and hold the Shift key, middle click anywhere inside the window and drag the mouse towards the required expansion direction:

Shift

+

Roll-up: Middle click on the header of a window, in order to leave only its header visible, without closing it:

Box selection of checkboxes: Checkboxes of any window can be massively enabled/disabled with box selection/deselection:

Switch radio buttons with the “1” key:

1

29

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

ANSA settings and configuration files All the settings of ANSA can be accessed from the Settings window which is invoked from Windows>Settings or using the shortcut Ctrl+I. All settings concerning the graphic interface and many options related to ANSA functionality can be found here. All the settings that are related to the GUI are saved in a file with the name ANSA.xml. E.g. the arrangement of buttons and windows, contents of hidden menus, toolbars, fonts etc are saved in ANSA.xml. When ANSA is launched, the ANSA.xml file is searched under /.BETA/ANSA/version_X.X.X/ANSA.defaults 3. /ANSA.defaults_vX.X.X

All the settings that are related to the Translators are saved in a file with the name translators.defaults. Eg. reading attributes annotations, publications etc. from a CAD file are saved in translators.defaults When ANSA is launched, settings are searched sequentially under the same locations with the ANSA.defaults. Thus: 1. /config/translators.defaults 2. Help

window

31

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reading CAD data

www.beta-cae.com www.beta-cae.com

Reading CAD data - General  How can CAD files be translated to ANSA databases? 1. Direct translation from within ANSA using File>Open 2. GUI driven translation through the CAD to ANSA translator. It can be invoked through: • /ansa_transl_gui.sh • or /ansa_transl_gui.bat (for windows)  What kind of file formats can be translated?

1. Neutral CAD files (Iges, VDA-FS, Step) 2. Files in native CAD format: • CATIA v4 and v5 • NX • Parasolid • PTC Creo Parametric (ex Pro/Engineer)

• Solidworks • Inventor • Core Technologie • JT Open  Where are the translation options? 1. For direct translation from ANSA Tools>Settings>Translators 2. For GUI driven translation, inside the CAD translator swindow  Where can these translation option be saved? In the translators.defaults_vx.x.x file either from ANSA through Tools>Settings> or from CAD translator through Tools>Preferences 33

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reading CAD data – translation options in ANSA Invoked through Tools>Settings 1. All formats: expanding this option, user can find the translation options according to the format of the CAD file 2. General: common options for translation regardless the format of the CAD file. The option Open settings before translation enables the Translators window every time the user selects to open or merge a CAD file. 3. Resolution/Tolerance/Units: options that control the resolution, tolerance values and units during translation ! Save the translators options in the translator.defaults_vx.x.x file

34

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reading CAD data – translation options in ANSA Some of the translation options are explained below: • Preview assemblies: for assemblies create a single file containing only hierarchy • Force single part: crate a single part database even for a ssemblies • Read free geometry: option to read free geometry • Read attributes: option to read attributes contained in geometric entities(part attributes are always read) • Include/Exclude layers: option to include/exclude specified layers • Geometry mode: specify what type of bodies to read • Perform ANSA topology: option to perform topology during CAD file reading • Topology between PIDs: option to perform topology between different CAD layers • Topology between parts: option to perform topology between different parts

• Clean geometry: option to perform automatic geometry clean up in addition to topology • Write log: create a log file for the translation • Open settings before translation: open the settings card before translation (after File>Open)

35

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reading CAD data – translation of a single neutral CAD file The folder /CAD_TRANSLATION/step_assembly/ contains files in neutral CAD format, that will be translated to ANSA files. In this example, the CAD format is STEP. Nevertheless, the procedure is the same for IGES or VDA files as well.

•Translate a single file: - From Tools>Settings>Translators>Resolution/Tolerance/Units: 1. specify a CONS perimeter length of 10 and Distortion distance of 20%. 2. make sure that the tolerances are set to middle. - From Tools>Settings>Translators>Neutral files with ANSA, make sure that Perform ANSA topology is enabled. However, mind having Clean geometry disabled, in order to proceed later to manual healing of geometry, for the purposes of the training. - Apply File>Open and choose a STEP file - Apply File>Save as and save the translated file as ANSA database. 1

2

3

36

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reading CAD data – translation of multiple neutral CAD files The folder /CAD_TRANSLATION/step_assembly/ contains files in neutral CAD format, that will be translated to ANSA files.

•Translate multiple files creating a single ANSA file: - Open a new, empty ANSA database, by applying File>New. In the confirmation window that opens, choose Discard so as not to save the current database again. - Apply File>Merge and select all the 8 STEP files. Keep the default options in the Merge Parameters window that opens. - File>Save as the database of the whole assembly with the name FR_RT_assembly.ansa.

•Translate multiple files creating a separate ANSA file for each one: 1. To avoid repeating the process of opening and saving each file one by one, use the File>Auto function. 2. Select all the rest STEP files and press Open. 3. Choose to Write ANSA DB. 4. An ANSA file with the name .step.ansa will be written for each selected CAD file, under the same directory. 2

3

4

37

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reading CAD data – direct translation of a single file File>Open file: ../CAD_TRANSLATION/jt_small_assembly/Assy00/Part01_SOLIDS.jt The translators window opens with the options of the JT format active. From Geometry mode, select to read Geometry only and press OK. ! In the same way you can directly translate an assembly

38

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

GUI driven translation: assembly translation Sample file: /CAD_TRANSLATION/jt_small_assembly/Assy00.jt The GUI provides an integrated environment for the translation of CAD or neutral data files. It integrates all translation modes along with their respective translation options into a single environment. Open the CAD translator and select the file to be translated. There are two important options when translating assemblies: 1.Flatten assemblies enabled: Creates a single ANSA database, containing the geometry of the parts and their hierarchy. 2.The hierarchy of the assembly can be seen in the Model browser of ANSA, that is invoked from the Parts toolbar button. 1

2

! Flatten assemblies options is not available for direct translation within ANSA

39

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

GUI driven translation: assembly translation 2. Flatten assemblies disabled: Creates one ANSA database containing only the hierarchy of the parts and one database for each part, containing the geometry. 1. To facilitate the work, from Tools>Preferences>Destination output specify an Output directory where all the ANSA files will be saved. 2. Open the Assy00.ansa and invoke the Model browser. It contains empty parts and groups. 3. In order to bring the geometry in the database, apply File>Merge. Select all the ANSA files of the individual parts that have been saved in the Output directory. 4. In the Merge Parameters window, have the options Merge Parts and Autoposition Parts enabled. 2 3

1

4

40

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Command line driven CAD Translation It is not necessary to translate CAD files directly to ANSA or using the translators GUI. Translation can be performed by running the appropriate executable file and specifying the required options from a command shell/prompt. For example, the translation of a single JT open file can be done with the command: ansa_jt.sh -i Part01_SOLIDS.jt -o /home/user/test.ansa -read_mode_geometry -notperf_topo

-i is the input CAD file. -o is the name of the ANSA database to save. -read_mode_geometry is the command argument that corresponds to Read Mode: Geometry only. -perf_topo is the command argument that corresponds to Perform ANSA topology. For CATIA files, the command would be: ansa_cad.sh -i my_file.CATPart -o /home/user/test.ansa -read_mode_geometry -notperf_topo

In order to see a list of the arguments, type: ansa_jt.sh -help

...or refer to the document CAD to ANSA Translator's User's Guide.

For every applicable option that is not specified in the command, a default value is considered. Default values for CAD translation are saved in the translator.defaults_vx.x.x file.

41

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Geometry healing

www.beta-cae.com www.beta-cae.com

Healing geometry automatically – file: /TOPO/demo0_simplified.igs The first thing to do after importing a CAD file is to check the tolerance values and apply the desirable-target perimeter length from Settings>Resolution/Tolerances/Units. 1. From the Tools toolbar -located on the top area of ANSA main window- apply, Checks>Geometry. Note that the same can be activated from Tools pull-down menu. 2. For shell descriptions of sheet steel components, mind having enabled all the Check Geometry Options, except Unmeshed Macros and Single Cons. 3. The Checks Manager window opens, listing the identified problems. Selecting an entry in the list, the involved faces, it becomes highlighted. 2 1

3

4. Right-clicking on one or more entries, opens a context menu. The involved entities can be isolated by applying Show Only. Auto fix column indicates in which problems automatic fix is available. Nevertheless, Check>Geometry cannot locate problems that need engineering judgement. E.g. a big gap could exist because of a missing face (i.e. a geometry error) or because of the existence of an internal opening (...no geometry error). In this example, the problems will be located and fixed manually, for training purposes.

4

43

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors – saving visibility status Display styles tool, located in the Drawing Styles toolbar, provides the ability to save the status of the visibility buttons and the Presentation Parameters tab options of the F11 card, under a specific style. Thus, different styles can be stored for respective needs and reused later, in order to instantly switch massively the visibility status of the database. In order to create a new style select New option from the sub-menu, In the window that opens edit the name and confirm. The style is created by storing the current status of visibility buttons and Presentation Parameters. Create the default style and the check geo 1. The created styles can be seen in the sub-menu. The active one is the checked 2. To activate another, select it from the list 3. Or select List from the sub-menu and in the Display styles window press right mouse button and Apply 1

2

3 or

44

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors 1. 2. 3. 4. 5. 6. 7. 8.

The orientation of the faces (grey-yellow side) is currently random Apply Faces>Orient>Visible to obtain uniform orientation of all the visible faces Applying Faces>Orient>Visible again, the orientation of the visible faces is inverted A shell component is considered clean if it contains single Cons only at the free edges and if it has no triple Cons. So, for visual inspection, disable visibility of Double CONS and disable Shadow. From Focus toolbar apply Or to isolate one of the areas, where the red Cons denote a topological problem. Enable Double, Shadow and Crosh. Lock the view. Focus toolbar ---> Not to hide a face. The problem is that the hidden face covers the underlying gap, but its boundaries are not common with the boundaries of the gap. The face needs to be trimmed.

4

3

2

1

Shadow

6

Lock

7

Double

5

45

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors – Trim a face 1. Focus toolbar ---> All to make all the locked entities visible 2. Cons>Project, in order to create Cons on the untrimmed face, at the projection of the gap boundaries. Select the Cons of the gap 3. Confirm with middle 4. Select the target face 5. Confirm with middle 6. The target face has been cut appropriately. Faces>Delete to delete the excessive face, clicking on a Cons of the face 7. An interface to inspect the faces that use the selected Cons opens. Choose to Delete the face ! If a Crosshatch had been picked, instead of a Cons, the face would be deleted without confirmation 8. The neighboring faces still have single Cons. Apply Faces>Topo and select the involved Cons to automatically connect them, based on the tolerances 9. The Cons appear yellow, indicating proper connectivity. Deactivate Lock, to proceed with fixing another region. 2

4

7

8

6

9

46

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors – Gaps (1) 1. Focus toolbar ---> All to make everything visible 2. Apply Surfs>Info at the depicted face. The face and the underlying surface are not big enough to cover the gap. A way to handle this is to delete the face and create a new one that covers it 3. UseFaces>Delete the face 4. Hotpoints>Delete: Select the two remaining hot-points. 5. With Faces>New using the COONS option: This function creates a new face (and surface) from boundaries that are already defined. Select the 4 Cons of the gap and confirm with middle mouse. 6. Accepting the preview that is given, a new face that fills the gap is created. 2

6

4

5

Mind having the option “Respect user selection” deactivated in the Options List. In other case, if the Cons are not selected sequentially, twisted faces are created.

In the depicted example, the Loop feature selection tool could be used, in order to select all the 4 Cons of the gap with a single click. 47

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors – Gaps (2) 1. Surfs>Info at the depicted face that leaves a gap. The underlying surface is big enough to cover the gap. A way to handle this is to create a new face, that uses the same surface as the existing one. 2. Faces>New, using the EXISITING SURF option. Select the 3 Cons of the gap. Confirm with middle. 3. Select the face, whose surface will be used for the new face. 4. A new face that fills the gap has been created.

1

2

3 C

B A

4 If one cannot remember the sequence of selections (e.g. what to select first – Cons or FACE?) or is not sure if middle click confirmation is needed, it is suggested to look at the Status Bar. Information is given, regarding what function is activated and what entity type has to be selected at the current step of the function.

48

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors – Unconnected faces 1. Isolate the area of the round protrusion. The large face underneath doesn't have a corresponding opening. 2. Cons>Project: Select the red Cons around the protrusion. Enabling the Feature Angle or Loop tool, selection can be done with a single click 3. Confirm end of selection with middle click 4. Select the target face 5. Confirm with middle click 6. Faces>Topo, selecting the involved Cons, in order to connect the protrusion with the underlying face 7. Faces>Delete the interior excess of the large face 8. Faces>Delete the small round face at the top of the protrusion 9. Faces>Orient to achieve the depicted result 1

6 4

8

9

2

Instead of using the function Faces>Delete, one could use the Delete function from the Utilities toolbar. Delete can be used for the deletion of entities of any type.

49

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors – Crack 1. Isolate the area of the depicted crack. 2. Zoom in. The two horizontal lines that correspond to the tolerances are smaller than the gap. This explains why the involved Cons where not automatically pasted. They have to be pasted manually. 3. Cons>Paste: Select the two Cons. The first selected will be moved to the position of the second. 4. Confirm end of selection with middle click. 5. When pasting Cons with distance that exceed the tolerances, a confirmation window opens. Confirm with OK. 6. Cons>Paste the two Cons at the bottom. This will close the crack, but what will happen to the small red Cons in between them? 7. A white dot appears, indicating a collapsed Cons (zero length Cons). This is a topological error. 1

2

3

B

A

Curves matching distance Nodes matching distance

5

7

6

B

A

Cracks are automatically fixed by the Fix function of Tools>Checks>Geometry. 50

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors – Collapsed CONS 1. In order to fix a collapsed Cons manually, apply Hotpoints>Release and select the involved hot points. This operation breaks the connectivity of all the Cons that were connected at the selected hot points 2. All the Cons now appear red. Five hot points are visible. To be able to paste the Cons without creating collapsed ones, the Cons must be properly segmented. Delete the depicted hot point with Hotpoints>Delete 3. Now the Cons can be manually pasted in pairs. Cons>Paste and select the depicted Cons. Confirm with middle. 4. Along the highlighted line, two red Cons exist. They cannot be distinguished because they are superimposed. Without exiting the Cons>Paste function, select the two Cons and confirm with middle. 5. Continue with pasting the two remaining pairs of Cons. 6. The picture shows the result that should be achieved. 2

1

3

B

4

5

A

6 B

A

B A

B

A

Collapsed Cons are automatically fixed by the Fix function of Tools>Checks>Geometry. 51

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors – Unconnected face (2) 1. Deactivate Double Cons visibility. Isolate the area where some problematic red Cons exist. 2. Reactivate Double and zoom in. Some Cons are not connected. There are two ways to handle this case: Either paste the Cons manually, or delete an area of the unconnected face and create a new one with adequate boundaries. For training purposes, the second way will be followed. Hotpoints>Insert and pick a location of the outer Cons as shown. 3. Faces>Cut and pick the two opposite hot points. 4. Curves>Cons2cv, in order to create a curve at the location of the external Cons that will be deleted in the next step. 5. Faces>Delete and select the small face 6. Faces>New>Coons: Select sequentially the 3 Cons and the curve that constitute the boundaries of the face to create. Confirm with middle and accept the previewed surface. 7. The Properties List opens and the user is prompted to select a PID for the new face. Why? Switch to PID color view mode. The neighboring faces have different PIDs, so the PID of the new face cannot be assigned automatically. Select the appropriate PID either from the list or from the screen and confirm with middle click. 1

2

3

4

6

7 D C

A

B 52

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors – Overlap 1. Disable Double, Single and Shadow. Only cyan Cons remain visible. Zoom in the area on the right 2. Enable Double, Single, Shadow and Cross hatches. This is an area of overlapping faces 3. Faces>Info and select an involved face, to see clearly its shape. This makes the existence of the overlap more clear 4. Cons>Project: Select the Cons of one face, confirm with middle. Then select the target face and confirm with middle 5. Faces>Delete the excessive face 6. Hot Points>Delete the unneeded hot points 7. The picture shows the result that should be achieved 1 2 3

4

5

6

7

B A D C Overlaps are automatically fixed by the Fix function of Tools>Checks>Geometry. 53

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Locating and fixing geometry errors – Triple CONS 1. Zoom at the area where cyan Cons are present. Faces>Delete and select a cyan Cons of a face (not a crosshatch). 2. The Faces Delete List preview window opens, indicating that 3 faces are using the Cons, highlighting the first one. Choose to Keep the depicted face. 3. Keep also the second highlighted face. 4. Delete the face, as shown. 5. The problem is resolved. 1

2

4

3

5

54

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Closing small openings: Fill Hole 1. Some holes are considered too small to be included in the mesh. Activate Cons>Fill Hole and select a Cons of an opening 2. The whole chain of Cons that constitute the hole are highlighted 3. To avoid manual selection, type an adequate diameter limit in the Fill Hole Parameters window and press Select 4. All the holes with equivalent diameter less than the specified one are highlighted. Confirm with middle click 5. The holes have been removed 1

3

2

4

5

55

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Fillet sharpening: Dach 1. Zoom in closer to the base of the top round flange. Although not very clear due to coarse resolution, this base is a round fillet. We will sharpen it, in order to avoid generation of very small elements there. 2. To get an idea of the radius and the width of the fillet, make a measurement, selecting just one Cons and choosing sequentially Length and Curvature (min radius) as Result. 3. Activate Faces>Dach>Dach. In the Fillets/Chamfers Parameters window, specify the shown values and press Select. 4. The fillets within the specified radius and width range are identified. Confirm selection with middle click. 5. Choose DELETE FILLET and Join Macros in the Dach's Parameters window, while previewing the new surface. 6. The fillet is sharpened. The orange Cons indicate locations where the adjacent faces will form a single mesh area in the MESH menu. 1

2 3

4

5

6

56

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Fillet sharpening: Dach (2) We will also sharpen the fillet that is adjacent to the large flange of the component. This time, selection will be done manually. 1. Activate Faces>Dach>Dach and select the Cons shown. Ignore the Fillets/Chamfers Parameters window. 2. The whole string of faces gets automatically selected. Confirm with middle click. 3. Make sure that Delete Fillet and Join Macros are enabled in the Dach's Parameters window, while previewing the new surfaces. Press OK. 4. The fillet has been sharpened. 1

4

2

3

When selecting faces manually, the Cons that is picked is of importance. The string of faces that lie opposite to it get automatically selected The Faces>Dach>Dach function is applicable not only on fillets, but also on chamfers. Chamfer selection is done either manually or via the Corner Angle and Width values of the Fillets/Chamfers Parameters window.

57

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Assign PIDs 1. Switch to PID color view mode and zoom in closer to the edge of the sharpened fillet. The DACH function has created a discontinuity, regarding the PIDs of the faces. 2. Switch Shadow to off, to make the view clearer. Activate Faces>Cut and select the two hot points that are shown. 3. Activate Faces>Set Pid and pick the crosshatch of the triangular face that has been created. Confirm with middle click. 4. The properties list appears. Select the PID to assign either from the list or (more easily) by clicking on another face that uses it. 5. Confirm with middle or with double click on the selected entry in the list. 6. The appropriate PID has been assigned. Switch Shadow to on, to make it more clear. Repeat the procedure at the other edge of the sharpened fillet as well. 1

2

4

3

6

58

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Needle faces Faces of very small or zero area constitute a topological problem. Needle faces are identified by Tools>Checks>Geometry and can be fixed automatically. Nevertheless, a manual way to treat them is presented below, for better understanding of the problem. Such faces may derive either from CAD (faces with width smaller than the tolerances) or by error of the user while creating new Cons in ANSA (e.g. by projecting a CONS on a face that uses it). In the later case, many hot points appear close to each other, but they cannot be deleted with Hot Points>Delete. 1. In order to isolate such faces manually, apply from Focus toolbar ---> Not to all the faces that lie next to the dense hot points. 2. The needle faces are revealed. Delete them massively with Faces>Delete and box selection. 3. Make the neighboring faces visible again (e.g. with Focus toolbar ---> Invert). Apply Faces>Topo at the involved area. 4. Hot Points>Delete can now remove the remaining hot points. 5. The result is shown in the picture. 1

2

4

5

3

59

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Unchecked faces Unchecked faces are faces that fail to become shadowed. These faces cannot be meshed, so they have to be eliminated when cleaning up the geometry. Unchecked faces are identified by Tools>Checks>Geometry. The number of Unchecked faces, if any, appears on the GUI index, as displayed in the following picture. Notice that, after the fixing procedure, no Unchecked index appears on the GUI. They can be: 1. Faces with many hot points very close to each other: Apply Hotpoints>Delete to remove the excessive hot points 1

2. Needle faces: Locate the needle faces and delete them (e.g. automatically with Tools>Checks>Geometry and Fix). 3. Face with perimeters that intersect themselves: Increase the resolution or add hot points at the intersecting Cons. 3

4. Faces with bad surface description: Delete the face and create it again in ANSA. 5. Faces with Cons that have very big variation in resolution: Apply a uniform resolution. 60

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Undelete entities What if a face is deleted by mistake? Deleted entities like faces, curves and points are kept in the database. The function Faces>Undelete gives a preview of the deleted faces. The user can select any of them and bring them back to the model. Alternatively, deleted faces can be retrieved by the Undo function of Utilities toolbar

Deleted entities can be discarded from the database, using the function Utilities>Compress (the respective button is by default available at the Utilities toolbar, as featured in the picture). The Compress window that opens, provides info for unused entities of any type. Faces are listed under the "Geometry" branch. Press Details... to see the number of the deleted faces that exist in "undelete status". Press OK to discard the deleted faces, thus reducing the size of the database. Once entities are removed using compress, they cannot be retrieved by any Undelete function Alternatively, deleted faces can be retrieved by the Undo function of Utilities toolbar

61

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Transform>Move: Move or Copy entities – file: /TOPO/symmetry_link.ansa 1. Some faces are wrongly positioned. Apply Utilities>Transform>Move (or from the corresponding button in the Utilities toolbar). Select the mispositioned faces. The PID region feature selection tool can be used, to select all the needed faces with a single click. Confirm with middle click. 2. In the Move Entities window, switch to the Translate tab. Pick two points from the screen, to specify the translation vector and distance. The respecive fields of the Move Entities window are updated automatically. Confirm with middle mouse button 3. The mispositioned faces have been moved, but need to be rotated as well. Without exiting the function, swith to the Rotate tab. Pick two points from screen, to specify the rotation origin and axis. Specify also a rotation angle (e.g. 5 degrees). Perform sequential rotations with the + and – buttons. 4. Press Finish, when reaching the displayed result. Apply Faces>Topo at the red Cons to connect the faces 1

2

3

4

4 62

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Detect similarity and linked faces 1. The two sides of the model are in a big extend symmetric. 2. Faces>Rm.Dbl>Geometry. Choose the Symmetry Plane option 3. The detected similar faces are highlighted in blue and green. As Action, choose to Delete the Green and Replace selected faces with Symmetry Links. 4. Enable Cross hatches. The crosshatches of the former green faces appear orange, indicating that they are linked with a parent face. Apply Faces>Info and select a linked face. An exclamation mark appears and the parent face is highlighted. Note that the linked faces are disconnected from the neighboring non-linked faces, as indicated by the red Cons. 5. Any action that is performed on a face, e.g. cut, mesh (as shown in the picture) etc, is performed automatically to its links as well. 1

2

4

5

!

3

- The symmetry plane is defined from Windows>Settings>Settings>Symmetry plane. By default, it is the global XY plane. - Linked faces can also be created manually, by copying existing faces with the function Transform>Link, from the Utilities toolbar. - The link between faces can be broken with Faces>Convert, selecting child faces (i.e. faces with orange crosshatch).

63

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Middle surface extraction

www.beta-cae.com www.beta-cae.com

Middle surface of sheet steel components: Skin - file: /TOPO/SKIN.igs For simple components without ribs or any kind of T-junctions (i.e components whose shell description in ANSA would not have any triple Cons), the Faces>Mid.Surface>Skin function should be used 1. The geometry has to be clean and must constitute a single, connected volume(it must contain only yellow Cons). Apply Tools>Checks>Geometry (or via Tools toolbar), having all the options enabled (except Unmeshed Macros) 2. Provided that the component passes the geometry check, apply Faces>Mid.Surface>Skin. Choose Offset Type : Link and Offset by : Thickness Factor. Select the faces to skin. Having Auto Selection enabled, all the involved faces can be selected with a single click. Confirm with middle 3. The Cons that correspond to the free edges of the shell description are highlighted. At this step the user can select or deselect Cons, in case the automatic detection was not precise (rarely needed). Confirm with middle 4. Select one of the two sides (red/green), that will be used as reference 5. The thickness is auto-calculated. Thickness factor of 0.5 corresponds to offset distance of half-thickness. Press OFFSET 1

4

2

3

5

65

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Faces offset from their surface Apply Surfaces>Info on a face of the previous example. The face doesn't lie on the surface any more. It is offset in a distance parametrically defined (half of the thickness). This way, if the thickness of the component changes, the face will be automatically moved at the new middle position * Apply Faces>Info on a face in order to see its offset. The offset is displayed in the ANSA Info window

3. The offset distance of any face can be changed by applying Faces>Offset>Link. Select one or more faces and confirm with middle. In the INPUT window, the user can specify either an absolute distance with the tilde as prefix (e.g. ~0.75) or a factor to be multiplied with the thickness of the face's property. Press the Enter key to apply the new offset

 The function Faces>Convert “breaks” the link of offset faces, by creating a new surface on the position of the face  A zero value brings the face exactly on the surface  * If the thickness changes equally from both sides, the face has to remain at the same position and only alter the thickness value. To do so, first use Faces>Convert and then modify the thickness value 66

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Middle surface of complex parts - file: /TOPO/02_MIDDLE_MULTI.ansa

67

For components with T-junctions, use function Faces>Mid.Surface>Casting. Function creates mesh (not faces) at the middle position How it works: Select all the faces and confirm with middle. In the window that opens, the most important parameters are: ‒ Minimum thickness: Specify the minimum thickness value that appears on the model. A value close to the minimum thickness of ribs is a value that will usually lead to good result. In this model, you may try a value of 2 ‒ Target element length: The element length of the mesh that will be generated. If it is left blank, it is considered equal to the Minimum thickness. ! Small values for minimum thickness and target element length increase the execution time of the function. T-junction treatment: “Real middle” : the nodes of the T-junctons will lie above the main shell. “Exact middle” option, the T-junctions will lie at the main shell surface. In order to display the elements according to their thickness, disable the Geometry. visibility flag in the Visibility toolbar Real middle and switch from ENT color view mode to EL.THICK. All visible elements are colored according to their thickness value specified at their nodes ! Generally speaking, “Exact middle” option gives good result and is recommended for ribs that are connected to the main body with sharp edges. In case the root of the ribs consists of big fillets, the result of "Real middle" is better and can be manually corrected with small effort. Introduction to pre processing with ANSA v17.1.2

Exact middle

www.beta-cae.com

Model browser

www.beta-cae.com www.beta-cae.com

Model browser - /PARTS_MANAGER/taurus_reduced.ansa Invoke the Model browser from Lists>Parts or from the respective Lists toolbar button or with CTRL+R. Almost all entities in ANSA belong to a part. The management of Groups and Parts in the Model browser is similar to a file management system that treats the Groups as folders and the Parts as files. Parts and Groups may reside in other Groups to form an assembly tree structure similar to a file tree structure In particular, using the model browser the user –among others- is able to:  Handle and visualize the model tree structure. This structure may derive from CAD or from a PDM system, but it can also be created from within ANSA, in order to compose handy working areas.  Change position of Groups/Parts  Characterize Parts for the definition and realization of connections  Save, delete and replace parts of an assembly to and from other ANSA databases. ! Each Part/Group has a unique name and a unique Module ID. Information for the selected entities is displayed in the info tabs Editing of a part's attributes can be done directly from the lower section of the Model browser window Group Model browser symbols:

Part Empty part

69

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Model browser: Display modes, filtering, view manipulation Display modes: Tree view

List view

Icon view

Easy filtering: Activate the filter button that is available in tree and list view mode. Type the filter under the respecive colomn header

View manipulation: From the context menu:

Clicking on the bulb:

Single click on the bulb: Show/Hide Double click on the bulb: Show only

Bulb symbols: All the contents of the part/group are currently visible Some contents of the part/group are currently visible All the contents of the part/group are currently non visible The part/group is empty 70

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Model browser: Parts identification and visibility control How to identify the part that an entity belongs to: 1. Press Identify at the menu bar of the Model browser. 2. Select a face from the screen. 3. The part that contains the face gets selected. All the entities of the part are highlighted on the screen. 1

2

3

Lock a part: Convenient when working on a single part of a database that contains a bigger assembly. 1. Right-click on the selected part and choose Mark As>Locked. The part is highlighted in yellow in the Model browser 2. Press All (from the Focus toolbar). Only the locked part remains visible. 3. Isolate a few entities of the locked part. 4. Press Invert: The previously non visible entities of the locked part only remain visible. The locked parts can be unlocked by choosing the Not Locked option of the right click menu.

2

3

4

71

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Model browser: Handle the contents of a part – Draw mode per part 1. Enable visibility of the Color column in the Parts tab of the Model browser. Column handling is done by pressing the arrow button. Every part/group possesses a color. 2. Switch to PART view mode (from the Drawing Styles toolbar). The faces are colored according to the part that they belong. Some faces seem to be assigned to the wrong part. We will assign them to the correct part. 3. Press Set Part in the menu bar of the Parts manager. 4. Select the faces. Confirm with middle. 5. Select the target part by picking it from the screen (as shown in the picture) or from the list. 6. Confirm with middle click on the graphics area or by double clicking on the entry of the selected part in the Part Manager. 7. The faces have been assigned to the correct part.

2

1

4

5

3

6

7

2x

72

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Model browser: Move parts between groups – Linked parts We will create a new group that will host some parts of interest, in order to facilitate their manipulation. 1. From the menu bar of the part manager, apply New>Group. 2. Assign a name to the empty group that is created. 3. Select some parts from the list. Drag and drop them to the group that was created before. Two options are available: -Move will remove the parts from the previous group and will add them to the new one. -Link will not harm the initial hierarchy. The parts will be placed as links under the new group. Choose the Link option. Note that instead of drag and drop, the options Cut/Paste from the right click menu can be used. 4. The linked parts are denoted with L. The links regard only the hierarchy of the assembly. No new faces are created. Linked parts can be removed by applying Edit Tree>Unlink from the right click menu. 1

2

3

4

A new group can be created directly by drag and drop of the selected parts to the New Group box that appears.

73

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Model browser: Assign new entities to parts - Current part When a new entity is created, ANSA automatically assigns it to a part, provided that it is clear to which part it should belong. E.g a new face that is created by selecting Cons of a specific part, will belong to the same part as well.

When it is not obvious to which part the new entity must be assigned, the user is prompted to select a part from the Model browser. E.g. Apply Curves>New and pick two hotpoints of different parts. In the Model browser, select the part where the curve will be assigned, by double clicking on it. Alternatively, press the Esc key. The curve is then assigned to the “Current part”.

2x

Every ANSA database has a Current Part. In order to identify it, apply Utilities>Identify Current.The current part gets selected. The settings that regard automatic part assignment, together with other options of the Model browser, are also availabe from Windows>Settings>Settings>Model browser or directly from the Model browser, applying Utilities>Options. Enable the Get the current part option in Settings>Model browser General tab Utilities>Current Part>Put to Current, so that new entities, that are not connected to a single part, will be automatically assigned to the Current Part. In order to specify the current part, select the part and apply Current>On from the right click menu. 74

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Transformation matrix Open file /PARTS_MANAGER/bolt_for_autoposition.ansa Enable WRK.PLN from the Auxiliaries toolbar, in order to visualize the 3 default Working Planes that exist in every ANSA database In the Model browser, notice the Position values of the part. This corresponds to the transformation matrix of the part. In this file, it is designed at the origin of the global coordinate system. Open file /PARTS_MANAGER/assembly_for_autoposition.ansa. It contains an empty part with the same name (bolt), but with a different transformation matrix.

File>Merge file bolt_for_autoposition.ansa. Mind having enabled: -the Merge Parts option, so that the entities of the incoming part with the name "bolt" are assigned to the existing part with the same name (...remember that part names are unique). -the Autoposition Part option, so that the merged entities are positioned based on the trasformation matrix of the part in the current database. 75

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Multi instantiated parts A multi instantiated part is a component that has been designed in the CAD software once, but has been placed inside the assembly several times in different positions. Multi instances and their transformation matrices are read when translating CAD files that contain hierarchy information. Multi instances can be created from within ANSA as well: 1. Apply Transformations>Copy from the right click menu of the bolt part. 2. Switch to the Rotate tab and specify the rotation origin and axis as shown. Select to create 7 copies, at every 45 degrees. 3. In the Transformation Options window, choose to create the new parts as New Instance. 4. The multi instances have been created. They are denoted with the M letter in the Model browser. 5. Suppose one bolt is meshed. Identify its part and apply (from the right-click menu) ANSA DM>Synch. Representation. 6. All the other instances aqcuire the same mesh. 1

2

3

4

5

6

76

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Surface mesh

www.beta-cae.com www.beta-cae.com

Main terms of MESH module Macro Areas (Macros) are the mesh areas of the model. They initially correspond to the geometry faces. Perimeter Segments (Perimeters) are the boundaries of Macros. They initially corespond to the Cons of the TOPO menu. Perimeters appear green, no matter if the corresponding CONS is single, double or triple. Hotpoints are drawn white in the mesh menu. They are fixed mesh nodes at the ends of the perimeters. Their visibility is controlled from Faces Draw toolbar Hot Points Perimeter nodes: They are mesh nodes that are drawn as magenta crosses. The initial distribution of perimeter nodes depends on the Resolution values. Their visibility is controlled from Faces Draw toolbar Perimeter Grids Weld Spots: Fixed mesh node locations inside a macro. Their visibility is controlled from Faces Draw toolbar Spots FE-model elements: Elements of a mesh that is not associated with geometry. This is the mesh that is imported when reading files in neutral solver format (applying File>Input). Its visibility is controlled from Visibility toolbar ---> FE Mod. Connecting Spots: Locations where geometry is connected with FE mesh. Their visibility is controlled from Faces Draw toolbar Spots Faces Draw toolbar

78

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Options window – Controlling element type and order 1

1. When applying any function from MESH menu, all the parameters that influence the function execution are displayed and can be edited from the Options List window. It is suggested to have the Options window constantly open. For example, dock it under the Module Buttons. The Options window can be opened from Windows>Options List. 2. When applying functions that create mesh, the element type (mixed/quad/tria) and element order (1st/2nd) are controlled from the Options window. Alternatively, they can be controlled from the Shell Mesh tab of the Mesh Parameters window, that is invoked from Utilities>Mesh Parameters or from the respective toolbar button, as featured below. The Mesh Parameters and the Options window communicate, i.e. changes that are done in one window will update the current values of the other window as well. The most important Element types are: Mixed: Both quadrilateral and triangular shells will be generated. Use this element type for crash applications. Quad: Generates quadrilateral elements. Triangles appear only at locations where pure quad generation is not possible. The number of triangles is smaller than in the Mixed type, but, at Macros with irregular shape, the quality of the quads and the orientation of the mesh may be poorer. Quad mesh type is adequate for durability applications. Tria: Generates only triangular elements.

2

79

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Mesh generation algorithms The algorithms that generate mesh are available in the Mesh Generation group of functions of the MESH menu: 1. Free: Generates as few elements as possible, trying to maintain the best possible quality. 2. Spot-Mesh: Gives better results to macros that have weld or connecting spots on them. Nevertheless, it is an algorithm of general use, even for macros without spots. Usually produces more elements than FREE. 3. Gradual: Gives better results in macros with uneven nodal distribution. 4. Map: Generates structured mesh on close to quadrilateral shaped macro areas. 5. Adv.Front: Generates mesh, starting from the perimeters of the macros. 6. CFD: Algorithm for variable size mesh, depending on the local curvature. 7. STL: For applications where the elements quality is not important, but the exact shape of the geometry representation is. 1

2

3

5

6

7

4

The nodes of the mesh that is created from these algorithms lie always on the surface of the macros. The mesh uses the perimeter nodes and hotpoints of the perimeter segments, without altering their location. There are only rare cases where the user needs to select the mesh algorithm to use. Usually it is enough to create a draft mesh arbitrarily and then apply functions for mesh improvement. 80

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

The Map algorithm 1. The MAP algorithm, applied with Mixed or Quad element type ensures pure quad generation, provided that the opposite perimeters of the macro have equal number of nodes:

1

2. When Map is applied with Tria element type, structured tria mesh is generated, as if the quads where split at one diagonal to produce two trias. The orentation of the diagonals can be controled by the user. In the Options window, choose the required Split trias for option.

3. When the oriented trias option is used, uniform orientation of the diagonals is achieved. 4. In order to change the orientation, apply Mesh Generation.>Map>Reverse, select the macro and confirm with middle. The Reverse option is available only in combination with oriented trias.

FREE

MAP

2

3

4

81

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Generating mesh - file: /MESH/mesh_file.ansa Lock the part and isolate it on the screen. Every mesh algorithm function has available the options Select, Re-Generate and Visible. 1. Apply Mesh.Generation>Free>Select and pick one or more macro areas. In the Options List window, mind having mixed as element type. Confirm with middle. The mesh is generated. 2. Mesh.Generation>Free>Visible affects all the visible macro areas. No selection is needed. 1

2

3. When using the Select and Visible options, the mesh on already meshed macros is not affected. In order to alter the mesh of a macro (e.g. mesh it with a different algorithm or settings, use the Re-Generate option. E.g apply Mesh Generation>Adv.Front>Re-Generate, select the shown macro and confirm with middle. 3

82

For unmeshed macros, Re-Generate works in the same way as if the Select option was applied. Mesh.Generation >Erase>Select/Visible deletes the mesh of the selected/visible macros. Mesh.Generation >Remesh>Select/Visible meshes an unmeshed macro with the algorithm and settings that were used the last time it was meshed. If the macro had never been meshed, the Free algorithm is used. Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Controlling perimeter nodal number The initial distribution of perimeter nodes depends on the Cons resolution. Cons resolution length influences all perimeters. This is the target distance between consecutive perimeter nodes. Cons resolution distortion influences only curved perimeters, leading to denser perimeter nodes. Distortion distance

Distortion angle

Distortion distance 20%

Distortion distance 1%

The element length of selected perimeters can be changed with the function Perimeters>Length The nodal number of selected perimeters can be changed with Perimeters>Number. The user can either type the node/edges (option in the Options List window) number, or pick a different perimeter to use its nodal number. The nodes are arranged equally spaced along the perimeter. The perimeter is colored red, indicating that its nodal number is not specified via its element length.

Clicking with the right mouse button on another perimeter, repeats the last action to the other perimeter, i.e the same nodal number will be assigned to it. In order to quickly increase/decrease the nodal number of a perimeter, use the function Perimeters>Num +/-. Clicking on a perimeter with the left mouse button adds one perimeter node, while the right mouse button subtracts one The nodal distribution of a perimeter, based on its element length, can be re-assigned applying Perimeters>Init. 83

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Quality criteria - F11 Quality criteria are specified from the Quality Criteria – Presentation Parameters window, that is invoked either from Utilities>Quality Criteria or from the respective toolbar button or by just pressing F11. This window will be also referred as "F11 window". The window contains separate tabs for criteria of shells and solid elements. Enable the checkbox of the required criteria and specify the threshold value in the "Failed" column. Choose also the calculation method for each criterion that can be calculated based on more than one definitions. -> Saves quality criteria settings in text files, with the extension .ansa_qual. -> Loads quality criteria from .ansa_qual files. The current quality criteria are contained in the ANSA.defaults file, by saving it from Windows>Settings. In order to display only selected criteria in the F11 window, apply Edit Criteria Visibility and choose the criteria.

Place the cursor over a criterion in the F11 window, to see a tooltip that explains the criterion definition. All the quality criteria are related only with geometric characteristics of the elements, except from the crash time step, that depends also from the material characteristics and the solution controls (mass scaling, scale factors). When having crash time step enabled, mind having activated the required solver deck and specified the appropriate material characteristics.

84

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Quality check: Hidden view mode 1. Activate Hidden from the Drawing Styles toolbar, in order to view elements according to the criterion they violate.

1 3

A color legend with the visible criteria is displayed. The number of violating elements is shown in the elements index (OFF). 1. A criterion can be activated/deactivated by clicking on its name in the color legend. Right-clicking on the color legend, a context menu appears. From this menu, the threshold value of a criterion can be changed and macros with elements that violate a specific criterion can be isolated (Show/Hide/Show Only). Also, the element of worst quality can be isolated via Show Only Worst. Choose the option Hide Inactive Criteria, to make the color legend shorter. 2. The legend and the elements index can be moved in a different location of the screen, by dragging and dropping them with the middle mouse button. 3. Apply right-mouse button and Show Only, to leave visible only the macros that contain off elements. To locate more easily the element of worst quality, use Show Only Worst from the same context menu. 85

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Quality check: QGRAPH - Info A fringe plot of the elements, according to the value of a criterion is displayed by switching the color view mode Fringe to QGPARH from the Drawing Styles toolbar. The criterion to display is specified in the Graph Parameters tab of the F11 window.

Apply Elements>Info>Info and select an element while in Hidden view mode. Information about the criteria that the element violates is given on the screen. The values of all the active criteria are displayed in the ANSA Info window.

86

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Modifying mesh areas: Join Apply Perimeters>Length [10], on all the perimeters of the part and Mesh Generation>Free. 1. The resulting mesh is of bad quality, because the shape of the macros doesn't enable good mesh generation. Many perimeters lie to close to each other. Make some measurements to see which ones lie much closer than the specified minimum length. Moreover, the angle between some macros is relatively small. The perimeters that connect them can be removed, in order not to impose a restriction for the mesh. The component needs defeaturing. 2. Apply Macros>Join on the perimeters that are highlighted in the picture. 3. The involved macros are connected and they loose their mesh. 4. Hotpoints>Delete the remaining hotpoints. Mesh Generation>Remesh>Visible, to recreate the mesh. 1

2

3

4

When Macros>Join is applied having feature selection tools enabled (e.g. Feature line), confirmation with middle click is needed. In other case, picking a perimeter removes it without confirmation.

87

Any action that modifies a macro area (e.g. joining, deletion-insertion of hotpoints, changing the nodal distribution) leads to loosing the mesh of the macro. In order to avoid applying Remesh or Recons many times, you have the options to enable Erase, Smooth, Reconstruct, Remesh Macros, Keep in the options window. A Preview of the reuslt is also available. In order to join macros or delete hotpoints without losing the initial mesh, enable the option Keep mesh. To avoid deleting hotpoints manually after every Join operation, enable the option Delete hot points. Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Modifying mesh areas: Release, Cut If a perimeter has been removed by mistake, it can be brought back with Macros>Release. The joined perimeters appear orange. Disabling Shadow and Wire from the Drawing Styles toolbar makes selection of perimeters easier. Display the joined perimeters by activating the Double>Joined Perims from Faces Draw visibility toolbar 1. At the depicted area, apply Macros>Cut, picking the two nodes that are shown. 2. Macros>Join the initial perimeters. 3. The resulting macros will not lead to thin elements. The feature line of the component is not altered significantly. This action needs to be repeated at several locations of the component. 1

2

3

! Avoid cutting macros at locations where joined perimeters exist. Needle and unchecked faces can be created, leading to macros that cannot be meshed. In such cases Join the cut faces and Release the joined perimeter. How to see where joined perimeters exist while applying Cut? Enable Draw joined perims in the Options List. Macros>Cut picking perimeters with the right mouse button, works like Macros>Join.

88

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Eliminating other narrow areas – Orient holes 1. The depicted locations would lead to very thin and skewed elements. 2. Hotpoints>Insert: Add two hotpoints as shown. 3. Macros>Cut: Perform two cuts, from the new hotpoints to the opposite perimeter nodes. 1

2

3

4. Macros>Join to remove the initial perimeters. 5. Treat the opposite area in a similar way. 6. The edges of the hole are not at all parallel to the opposite perimeters. Apply Perimeters>Slide and pick a hotpoint of the hole. Move the cursor to achieve a better orientation 7. Enable Wire and Shadow: The macro areas have better shape, but the mesh still needs to be improved. 4

5

6

7

89

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Mesh improvement: Assign adequate nodal number 1. Apply Perimeters>Num +/-, to add one node to the shown perimeter. The nodal number of opposite perimeters becomes equal, allowing better mesh generation. 2. Assignment of adequate nodal distribution is facilitated by creating perpendicular cuts at some locations. Apply Macros>Proj.Cut at the shown area: Pick a hotpoint and then pick sequentially the shown perimeters. The function projects a hotpoint to the each selected perimeter and cuts the macro between the initial and the projected point. 3. Apply Num +/- and Proj.Cut at several locations, to achieve a result like the one that is shown in the picture.

1

3 3

2

90

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Mesh improvement: Split/Join elements – Move nodes 1. The depicted area contains some trias that can be eliminated. 2. Elements>Split>Shells and select the shown edge. The result of element splitting is previewed. Confirm with middle. 3. Elements>Join, to create a quad from two trias. Pick the edge between the two trias to join them. 4. A manual way to improve the element quality and flow is to move nodes manually. Apply Grids>Move. In the MOVE GRIDS window, enable the Surface option in the Guided tab. Pick a node and move the cursor to place it at an adequate position. The Surface option ensures that the node will still lie exactly on the underlying surface. 1

2

3

4

91

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Hints for the Elements>Split/Join functions - Grids>Paste The user can specify the path to split by selecting edges and/or nodes. The respective check boxes must be active. To avoid enabling-disabling the checkboxes with the mouse, the 1 and 2 keys can be used for Edges and Nodes respecively. Selection of many edges that lie opposite to another can be facilitated by activating the Opposite Path selection method. Confirm with middle click.

1 2

Removal of triangles by coarsening the mesh can be done with the Grids>Paste>Manual function. A C B

D

Elements>Split X splits a quad in four trias. Followed by Elements>Join, it can reduce the number of trias at some areas.

Working with the Split, Split X or Paste function, selecting an edge with the right mouse button works as Join. If mesh type is tria, Split and Split X right click works as Swap 92

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Hints for the Grids>Move function - Grids>Origin Switching to the Free tab of the MOVE GRIDS window, free movement of nodes is performed on the screen plane. By disabling axes (X, Y, Z), the movement can be constrained on specific axes of the global coordinate system. It is also possible to work with a local coordinate system, as shown in the picture. Right click on an edge or an element to pick its local system. Then select the nodes to move.

B A

From the Guided tab: 1. Perims Slide: Adequate to slide a hole and/or a washer. 2. Perims Offset: Adequate to resize a hole and/or a washer. 3. Shells Normal: Moves selected grids normal to the element. Useful to correct manually warping violations. 2

1

3

In the Options window, the user can choose if a single node or multiple nodes will be selected. When single is active, no confirmation with middle click is neeeded after selection. By default, the smart option is active.Then, if selection starts with a single mouse click, it works like single. If selection starts with box/polygon or if a feature selection tool is active (e.g. feature line), then it works like multiple, requiring confirmation with middle mouse. 93

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Mesh improvement: Fix Quality 1. The red colored elements violate the minimum length criterion. The problem can be fixed with manual nodal movement, but it is more convenient to use a function that automatically moves nodes as much as needed to fix violations 2. Apply Shell Mesh>Fix Quality>Select and select the area where nodal movements will be performed. Selecting more zones of elements around the violated ones, gives more freedom to the algorithm to fix the violations. Confirm with middle 3. The area that will be affected is previewed: The involved perimeters are highlighted in green. The nodes at the boundary of the selected area are highlighted in yellow, indicating that they will not be affected by the function. At this step, the user can optionally select some edges/nodes to freeze or select more shells to participate in the function, by switching to the respective radio button of the Selection Window. Confirm with middle 4. The result is previewed. The user can press the Invert button in the Preview window to inspect the movements that will be performed. If the violations are not fixed, press Run Again. Accept the result with OK or confirming with middle 5. Violations are fixed. One node has been moved slightly away from the geometry 1

2

4

3

5

94

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Fix Quality: How it works 1. The function Fix Quality considers the quality criteria that are specified in the F11 window. Specifically, it can fix simultaneously the following criteria: length, angle, skew, warp, taper, crash time step, min height, jacobian, mid point devialtion/alignment. It cannot fix aspect and squeeze quality violations 2. After applying Fix Quality, the nodes may not lie exactly on the perimeters and on the underlying surface any more. The allowed distances are specified from the Fix Quality tab of the Mesh Parameters window, together with more options that affect the function. These distances can be defined as absolute values or as a percentage of the target/minimum length. 3. From the Basic tab of the Mesh Parameters window, the user can select to protect some areas from being affected by Fix Quality. E.g choosing to freeze single bounds, no node of the model's free edges will be affected. 1

3

F11

or

2

Enabling the option Split remaining violating quads, warped quads that cannot be fixed with node movements are split into two trias.

95

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Mesh improvement: Smooth 1. Apply Elements>Split>Shells and Join to remove some triangles at the shown area. 2. The flow of the mesh must be improved. Moreover, many off elements exist nearby. Moving nodes manually would be time taking. Applying Fix Quality would fix violations, but the flow of the mesh would not be considered. The Shell Mesh>Smooth function improves the flow of the mesh, incorporating all the capabilities of Fix Quality as well. The same parameters of the F11 and Mesh Parameters windows affect it. 3. Apply Shell Mesh>Smooth>Select and select the area to improve. Confirm with middle. 4. The perimeters and the frozen edges/nodes of the area are previewed. More features to freeze can be selected, in the same way as with the Fix Quality function. 5. The result is previewed, to inspect the automatic node movements. 6. The flow of the mesh is improved and the quality violations have been removed. 1

5

2

6

3

4

After applying Elements>Split/Join or Grids>Paste, usually a mesh smoothing is required as well. In the Options window, mesh improvement with smooth can be set to run automatically after these functions

96

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Protect processed areas: Freeze The processed macros need to be protected from unintentional changes. Apply Macros>Freeze/Un and select the macros. The wire is colored blue. No operation that would alter the macros or their mesh is allowed. If needed to unfreeze a macro, apply the same function, but select the area with the right mouse button.

+

= Freeze

+

= Unfreeze

The function is available also in the TOPO menu as Faces>Freeze/Un Proceed with the rest of the part: Eliminate narrow areas with Macros>Join/Cut as explained before.

97

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Mesh improvement: Reconstruct 1. The shape of the macro areas and perimeters is ok, but the mesh is still not. In order to avoid performing a lot of manual nodal assignment, element splitting and nodal movement, we will perform automatic mesh reconstruction. Apply Shell Mesh>Reconstruct>Select and select all the needed macro areas. Confirm with middle. 2. The perimeters and frozen edges/nodes are previewed similarly as with Fix Quality/Smooth functions. 3. The result is previewed. Note that the Reselect button leads back to step 2. 4. The reconstruct function has created new elements at the area, reducing triangles and improving the mesh flow and orientation. The nodal distribution of the perimeters has been locally altered. The Reconstruct function incorporates all the capabilities of Smooth and Fix Quality, but it is not restricted to move only the initial nodes. It creates a new mesh as well. Any area that still doesn't have a good mesh result will be processed locally afterwards. 1

2

3

4

The perimeters/edges etc preview (step 2) can be skipped by disabling the option Allow feature lines handling from the Perimeters tab of the Mesh Parameters window.

98

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Final inspection of mesh Apply some more manual operations on the mesh of this part to achieve a result like the depicted one. If needed, unfreeze some macros to make more extended changes (e.g. create 3 rows of elements at the lower flange). The number of any Unmeshed macros that skipped the user's attention may appear on the GUI index, just like Unchecked faces. Finally inspect the mesh, by disabling visibility of perimeters (Perims button, from the Faces Draw toolbar).

A more clear view of the mesh is given. This is a way to reveal areas of bad flow and orientation, even if no quality violations exist.

Inspect grids moved from geometry, by disabling additionally the Wire flag button from Drawing Styles toolbar. In order to bring them back to the geometry, use Grids>Origin. Fix possible violating elements using the functions described previously

99

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reconstruct: How it works - General Reconstruct considers the quality criteria of the F11 window in the same way as Fix Quality. Other parameters that influence Reconstruct are set in the Mesh Parameters window. In the Shell Mesh tab, the most important setting is the Target length. It can be specified as: • An absolute value. • Equal to the CONS resolution length. • Equal to the average or to the local length. • Free, that imposes no guideline. The option is adequate for the creation of uniformly flowing quads, regardless of their aspect, as shown in the picture. • By defining an expression (e.g. 0.5*average). Moreover, options to Freeze specific features or to remove triangles from the area of specific features are available.

The settings of the Fix Quality tab affect Reconstruct in the same way as Fix Quality. Additionally, special treatment for Flanges, Fillets, Holes and Tubes can be specified for the Reconstruct function. The settings of the Mesh Parameters window can be saved and loaded from text files with the extension .ansa_mpar. The settings are also contained in the ANSA.defaults file that can be saved from Windows>Settings. 100

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reconstruct: How it works - Holes/Tubes 1

2

Reconstruct can create zones of quad elements around holes, for simulation of washers (pic.1) The settings are specified in the D Features tab of the Mesh Parameters window (pic. 2), by activating the Holes feature. Different treatment can be specified for Bolt holes and General holes. 4 General Holes: Any opening without d D sharp angles. Bolt holes: Openings that can be detected by any of the following three methods: Proximity of holes: Pairs of holes, whose distance and angle are smaller than the specified values (picture 3). Bolt connections: Holes that lie within the search distance of ANSA connections of type Bolt. Shape of holes: Any circular or oval shaped hole with a ratio of length/width smaller than 2 (picture 4). ! A similar treatment can be specified for the shell mesh around holes of components with solid description. The settings are specified in the Features tab of the Mesh Parameters, by activating the Tubes feature. 3

101

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reconstruct: How it works – Holes treatment settings 1. Holes are treated according to the Diameter Ranges that are specified in the respecive column. Press the +/- buttons to add/remove a range. Press the buttons to add/remove a zone. In the Default row, the treatment of holes that do not lie within any of the above ranges can be specified. 2. Target Diameter: Optional field to resize holes. 3. Node Number: Can be specified either as: -an absolute value. -an Expression (e.g. L0=Lmin*1.2 means that the resulting element length at the hole will be 1.2 times the minimum length that is defined in the F11 window). -auto: automatically assigns the minimum number of nodes, that leads to an element length close to the target length, considering also the specified distortion, which is also the maximum number of nodes, so as not to have minimum length violation. 4. Zone N: The width or the diameter of the Nth zone is specified either with an absolute value or using an expression. 5. Typing of expressions can be aided by the expression editor that opens by choosing the respective option from the field's pull down menu. 2

3

4

1

5

102

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reconstruct: How it works - Flanges/Fillets Reconstruct can treat the flanges of the model by creating rows of quad elements according to the settings of the Features tab of the Mesh Parameters window (Flanges feature activated). Identification of flanges is done according to one or more of the following methods: Proximity of faces: Pairs of faces, whose distance and angle is smaller that the specified values. The distance can be specified either as an absolute value or as a factor of the faces average thickness Connections: Faces that lie within the specified distance from a connection entity Shape of faces: Faces with close to quadrilateral shape, bounded with red Cons at the three sides Flanges are treated according to the ranges of widths that the user specifies. ! The specified number of rows should not lead to big violations of the minimum length criterion. If violations at flanges are acceptable, disable the option Grow violating flanges in the Fix Quality tab. In a similar way, rows of quads can be created at the fillets of the model. The treatment is controlled from the Features tab, by activating the Fillets feature. Type the number of rows under the Treatment column for each range of radii and widths.

103

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Automatic defeaturing: Reshape - file: /MESH/mesh_file.ansa Another approach in meshing could be to treat the macro areas automatically. 1. Apply Perimeters>Length to assign a length of 10 on all the visible perimeters. Create a draft mesh (e.g applying Mesh Generation>Free>Visible). As expected, the mesh is of bad quality. 2. Apply Shell Mesh>Reshape>Visible. The perimeter and frozen edges/nodes are previewed (as in the Reconstruct function). Confirm with middle. 3. The mesh has been improved by automatically joining perimeters, adding/removing hotpoints and creating new elements. Reshape incorporates all the functionality of Reconstruct (holes, fillets etc treatment and quality fixing), but, additionally, it performs automatic defeaturing, creating macro areas of more convenient shape. ! No preview of the mesh result is given when applying Reshape. 4. Press Macros>Release just to inspect which perimeters have been joined. 1

2

3

4

104

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reshape: How it works The parameters for defeaturing are specified in the Perimeters tab of the Mesh Parameters window (pic 1). The most important parameter is the Join Perimeters with distance Cut is not a solution because it leads to erasing the mesh. The adequate function is Macros>Edge2Perimeter 1. Suppose that it is decided to close the hole that leads to minimum length violations. Apply Macros>Edge2Perimeter and select the highlighted element edges (the Feature Line selection tool can help) 2. The macro has been cut, without destroying the mesh 3. Switch to Topo menu, apply Cons>Fill Hole and switch back to mesh. Only the small macro area lost the mesh. 4. Mesh it again (e.g. With Mesh Generation>Remesh) 5. Apply Shell Mesh>Reconstruct>Select, selecting the macro 6. The mesh is improved 7. Continue with making manual mesh corrections and isolating areas with Edge2Perimeter. When achieving the required mesh result in an area Freeze it to proceed with the next areas 2 3 1

4

5

6

7

106

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Easy parameters set up – Mesh Parameters Generator Setting up the Mesh Parameters and the Quality Criteria is significant for the mesh result. For easy set up of Mesh Parameters and in order to achieve a fast and good quality mesh result from functions like Reconstruct, Reshape (and Batch Mesh as well, which will be presented later), a wizard is available. 1. It can be accessed through the Mesh Parameters window. Pressing the Create new Mesh Parameters button, the Mesh Parameter Generator 1 window appears. 2. The Mesh Parameters and the Quality Criteria can be defined through this window. These settings will overwrite the settings in the actual Mesh Parameters and Quality Criteria window. These settings can then be saved through the Save option, in order to be available for future use. Through this wizard window, it can be selected whether the Mesh Parameters or/and the Quality Criteria will be defined. A Name for the Mesh Parameters and the Quality Criteria can be set if necessary. The Mesh type can be selected. Available options are: Crash, Durability, NVH, CFD and Structural Tria.

2

107

According to the Mesh Type that is selected, the Mesh Parameters and the Quality Criteria will be set, in order to give a very good "First Mesh Result" for the type of the selected analysis. Available settings that can be defined are: - The Target (element) length - The Minimum length - The Distortion distance Pressing the OK button these settings will overwrite the Mesh Parameters in the Mesh Parameter window. The rest of the Parameters (like fillets/holes/tubes treatment etc.) will get a default value, according to the selected type of Analysis. The Mesh Parameter window will remain open, so that any modification can be applied, if necessary.

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Geometry vs FE mesh / Grids>Origin Nodes that have been moved from their initial position (either with Grids>Move or Fix Quality) can be brought back to their initial position on the macro area, exactly on the underlying surface, using the function Grids>Origin (pic 1). Select the nodes. No confirmation is needed The distance of grids from the underlying surface can be inspected with the aid of the quality criterion Distance from geometry (pic 2). The QGRAPH color view mode is a convenient way to visualize the deviation from geometry. The distance of grids from their initial position on the macro area can be inspected with the criterion Distance from origin (pic 3). The mesh stops being associated with the macro area by applying Elements>Release(pic 4). Select some macro areas and confirm with middle. The macro becomes unmeshed and Origin doesn't work on the elements any more. The released mesh (FE mesh) is connected with the adjacent geometry mesh with yellow spots. More about FE mesh will be shown in the session “Handling non geometry mesh”. 1 2

3

4

108

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Batch mesh

www.beta-cae.com www.beta-cae.com

Batch mesh Batch mesh performs automatic mesh generation and defeaturing, based on predefined mesh parameters and quality criteria. It can be used to mesh many parts of an assembly, using different mesh parameters for different areas of the assembly. E.g. For a frontal crash analyses, the front parts would be meshed with finer mesh, while the rear parts with coarser mesh. Nevertheless, batch mesh can be deployed to easily mesh even one or a few parts with the same mesh requirements, like in the following example: File: /MESH/FR_RT_assembly_clean.ansa We will mesh the part of the assembly with a target length of 10mm. 1. Invoke the Batch Mesh Manager from Tools>Batch Mesh or from the respective toolbar button. Apply New>Meshing Scenario. 2. A Batch Meshing Scenario, togeter with a Default Batch Mesh Session is created. More Sessions can be added under a Scenario, in case there are parts that need to be processed according to different requirements. In this example, one session (the Default Session) is enough. 1

2

110

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Batch mesh: Select entities to mesh 1.The Meshing Scenario doesn't include any entities yet (indicated as "Empty" under the Status column). Double click at the Contents column of the Meshing Scenario. 2. In the window that opens, select all the parts at the left pane. Press the button with the right arrow. 3, The selected parts have been assigned to the scenario. Confirm with the OK button, to exit the window. 4. The Meshing Scenario now contains 10 parts, that have also been automatically assigned to the Default Session. The Status has turned to “! Completed ”, because the contained entities are unmeshed. 1

3

2x

2

4

Selection of entities for batch mesh can be based on ANSA Parts/Groups or on Properties (PIDs). 111

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Batch mesh: Input Quality Criteria 1.Double click at the Quality Criteria column of the Session. 2. A window to specify the quality criteria of the session opens. Specify the criteria as shown in the picture. The window is very similar to the F11 window. Nevertheless, the two windows can contain different quality criteria settings. (Note that a Batch Mesh Scenario can contain many sessions, each one with different quality criteria). Transfers the quality criteria of the session to the F11 window.

3. Exiting the Quality Criteria window with OK, the respective column of the session is updated according to the name of the quality criteria set. 1

2

2x

3

112

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Batch mesh: Input Mesh Parameters 1.Double click at the Mesh Parameters column of the Session. 2. A window to specify the mesh parameters of the session opens. Transfers the mesh parameters of the session to the global Mesh Parameters window. Input the shown settings in the Basic and Perimeters tabs. 1

2

2x

Note that the target length can be specified only as an absolute value, because Batch Mesh, in contrast with Reconstruct/Reshape, doesn't require an existing mesh to work. In case a mesh already exists, the user can choose to erase it, work on it or leave it intact. 113

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Batch mesh: Fillets treatment The easist way to specify fillets treatment is the Deafult>auto. This way, fillets are identified automatically by ANSA and the number of rows is automatically calculated based on the specified target length, distortion and quality critera. Additionally, for fillets of very small radius and width, we can enable the Split treatment (see note below), in order to avoid creation of very small elements.

Except from creating quad rows, the user can choose to Sharpen fillets (in the same way that the function Topo>Faces>Dach>Dach works) or Split fillets (like Topo>Faces>Dach>Divide face). Sharpen

Split

Element rows

Similar treatment can be specified for the chamfers of the model, choosing to Enable chamfer treatment.

114

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Batch mesh: Flanges treatment 1. In the Flanges tab, specify the Flanges treatment as shown. Taking into account that the minumum length is 5mm, this treatment ensures the creation of more than 2 rows of elements at all the flanges where this will not lead to minimum length violations. A result is shown in picture 2. 3. Mesh result if no flanges treatment were specified. The flange is meshed according to the target length (10mm), leading to only one row of elements. 4. Mesh result in case of wrong flanges treatment specification (big number of rows leads to minimum length violations). 1

2

3

4

No flanges treatment 115

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Batch mesh: Holes treatment 1

116

1. Specify also the Holes treatment. Setting the Target Diameter for holes with diameter till 7 as Fill, will lead to removing the small holes, that would result in minimum length violations, even if they were modeled with 4 nodes at their perimeter. The Fill option works in a similar way as the function Topo>Cons>Fill Hole. The node numbers and widths are specified in such a way, that the elements of the created zones will have a good aspect ratio, without violating the minimum length criterion. 2. A result of the above treatment is shown in the picture. 3. An example of inconsistent holes treatment specifications is depicted. Big node number leads to min. length violations. 2 3

A good practice before batch mesh is to create a draft mesh at some macros around some holes and tune the values for the holes treatment using the Reconstruct function. The diameters of all holes are automatically measured when triggering the Contents list button from the Mesh Parameters window. Note that if you try the Measure tool, by switching selection to Cons/Curves, enabling the Loop feature selection tool and choosing Equivalent Circle as result, in oval holes, the Equivalent Circle measurement will result in the diameter of the incscribed -in the hole- circle.

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Batch mesh: Fix Quality settings - Run Scenario - Statistics 1. In the Fix Quality tab, input the shown settings. 2. Exit the Mesh Parameters window of the session with OK. In the Batch Mesh Manager, press Run, to execute all the scenaria and sessions that are checked in the window. 3. After batch mesh execution, the Status of the scenario is !Completed. Double click at the Status column of the scenario. A Report is given for each processed part. The reason for the Error status is that some off elements have remained. Errors that occur during batch mesh (like leaving some off elements or some unmeshed macros) do not stop the whole procedure. They just leave some areas that the user will need to process after batch mesh. Press Select All and then Statistics. 5. Detailed info regarding the achieved element lengths and the remaining quality violations per part is provided. 1

2 3 2x

5

4

117

A quick mesh generation using the batch mesh algorithm can also be done based on the global mesh parameters and quality criteria (without the use of batch mesh scenaria) with Mesh> Mesh Generation>Batch. Additionally Batch function is a good and fast way to optimize the parameters and quality criteria on a specific area instead of the whole part

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Suggested way of working for shell mesh / batch mesh - Before meshing many components with batch mesh, first tune the parameters of the batch mesh session (e.g. trying different defeaturing level and distance), by batch meshing just a few characteristic parts. Do not expect an error free result, but a result that can be easily corrected after batch mesh. - Right click on the batch mesh session and, from the context menu that opens, apply Copy to Global Settings>Meshing Parameters and Quality Criteria. This will transfer the mesh specifications of the session to the F11 and Mesh Parameters windows, that affect the functions for local mesh improvement and the Hidden view mode.

118

Then work on each part to make local mesh improvements: -Press Macros>Release or switch to Topo menu, in order to dispay orange Cons/Perimeters and inspect the defeaturing that has been performed. -Isolate the areas with good mesh result using Edge2Perimeter and Freeze them. -Wherever needed, correct the defeaturing that was performed from batch mesh by isolating the area (Edge2Perimeter) and applying Macros>Release/Join/Cut. -Fix any remaining violating elements using Fix Quality and Grids>Move. -Where the mesh result is too bad to be corrected simply by moving nodes, apply local Reconstruct at areas with bad mesh result. Change the reconstruction parameters temporarily if needed. If reconstruction doesn't give the required result, make manual mesh corrections, applying Elements>Split/Join, Grids>Paste/Move, Shell Mesh>Smooth, Macros>Cut/Proj.Cut, Perimeters>Number/Num +-. *Refer also to the document Mesh quality improvement after Batch Meshing. Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Handling non geometry mesh

www.beta-cae.com www.beta-cae.com

Reconstruct FE mesh (1) 1. File>Input>NASTRAN the file /MESH/reconstruction_fem5.nas We will use Reconstruct to coarsen the mesh and to create zones around the holes. Make some measurements on the element edges to find out the element length. It's about 8mm. 2. The FE mesh doesn't have any macro areas and perimeters. Nevertheless, characteristic feature lines and corner nodes of the model must not be altered during mesh reconstruction. All the remaining interior nodes will be created on the surfaces of the elements of the initial mesh (FE surface). The element edges that will be considered as feature lines and the corner nodes, are identified based on the settings of the Perimeters tab of the Mesh Parameters window. Use the default values for the Feature line angle limit (10 deg) and the Feature line corner angle limit (40 deg). To get precise information about the average element 1 length, apply Utilities>Deck Info. In the DECK INFORMATION window, enable the Shells Info checkbox. The avarage length will be displayed among other info in the DECK REPORT that is given.

Feature Line angle

2

Feature Line corner angle

120

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reconstruct FE mesh (2) 1. In the Basic tab, input the target length as 1.5*average. 2. In Features tab, activate Holes and specify to create 8-node zones of 6mm around the holes of the model. (Make first some measurements to get an idea of the holes sizes). 3. In the Fix Quality tab, input the shown values. Note that for FE mesh, the distance from surface is measured from the initial FE surface, while the distance from perimeters is the distance from the edges that are identified as feature lines. In this example, do not specify any fillets or flanges treatment. 4. Input the mesh quality criteria in the F11 window as shown. The min/max length are consistent with the target length, that is estimated to be about 12mm. 1

2

3

4

121

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Reconstruct FE mesh (3) 1. Apply Shell Mesh>Reconstruct>Visible. The identified feature line edges, corner nodes and hole zones are highlighted. 2. Having active the Edges selection mode, select the shown edges to consider them as feature lines, although their angle is smaller than the specified in the Mesh Parameters. 3. The mesh has been coarsened and zones have been created around the holes, except at locations where the holes lie too close to feature lines. Suppose that creation of zones is judged as more important than following the feature lines locally. 4. Correction at the highlighted area will be done with local reconstruction. Set the target length to average, to avoid further coarsening. The target length can be controled either from the Mesh Parameters or from the Options window, while applying Shell Mesh>Reconstruct>Select. 5. Deselect some identified feature lines, to allow enough space for the zone creation. 6. The mesh result is improved. Fix also the remaining problematic areas with manual corrections (Split/Join/Moveetc).

1

2

4

3

5

6

122

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Fill FE holes 1. Suppose it is decided that the holes of the component should be removed. 2. Apply Shell Mesh>Fill>Holes. To select the edges of the holes, switch the Fill mode option to Single bound holes, input a Max diameter limit and press Identify. Holes are selected. Choose the Fill method and press Next. 3. Holes are filled. Enable Create points at hole centers to create 3d points for reference and optionally set the Reshape result plus to 2 in order to improve the mesh. 4. Press Finish. 3d points are created at the centers of the filled holes. ! Note that holes can be selected and de-selected manually as well (pick the Loop option of the feature selection tool to facilitate selections). 1 2

4

3

123

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Open FE holes 1. Suppose that holes need to be re-opened at the initial locations (i.e at the projection of the 3d points to the existing mesh). Apply Shell Mesh>Project>Holes. First, the area where projections will be searched has to be selected. Select the whole component and confirm with middle. 2. In the Project entities window, input the target Diameter (20) and demand one zone of 6mm width around the holes. 3. Select the points to project. Selection can be done easily with a box, by disabling FE-Mode visibility, leaving visible only the 3d points. ! Changing the Project entities options while performing selection doesn't affect the settings of the already selected points. 4. The automatic reconstruction process begins with feature lines handling. ! If feature lines that intersect the holes are left selected, then the created holes will not be circular and no zone will be created. 5. Accepting the reconstruction result, the holes are opened, creating also washer zones around them. 1 2 3

4

5

!! Opening/Filling of holes, as well as other functions for mesh handling, automatically perform mesh reconstruction. Make sure that consistent values are set in the F11 and Mesh Parameters windows, to avoid obtaining bad mesh results. 124

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Connect FE with Geometry mesh (1) File: /MESH/apaste.ansa 1. The model contains some meshed macros and an area of FE mesh. Enabling the Perims visibility button from the Faces Draw toolbar, the red line at the boundaries of geometry and FE mesh indicates that the meshes are not connected. 2. Measure a distance between a node and the opposite edge to get an idea of the size of the gap. It is about 2mm. 3. Apply Grids>Paste>Auto>Visible. Input a search Distance of 2.5 and press OK. 4. Only few nodes that lie within the search distance are identified. 5. Confirming with middle mouse, the nodes are pasted. Yellow spots appear at the lcoations where geometry is connected with FE. 1

4

2

3

5

125

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Connect FE with Geometry mesh (2) 1. The previous operation was adequate for locations where one-to-one node correspondence existed. In order to connect the locations where no corresponding node exists at the geometry side, while working with the function Grids>Paste>Auto, enable the option Project on geometry and press OK. 2. Hotpoints are created at the projections of the FE mesh boundary nodes to the perimeters of the geometry mesh. The mesh is erased at the affected macros. 3. Confirming with middle mouse, geometry and FE are connected. 4. Apply Mesh Generation>Free>Visible, to remesh the macros. The resulting mesh has no gap between geometry and FE. 1 2

3

126

4

If projection is expected to be done at big macros, it is recommended to apply first Macros>Edge2Perimeter, creating smaller macros that will be affecter, losing the mesh. Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Improving the result of middle surface extraction

www.beta-cae.com www.beta-cae.com

Correcting the middle surface: DELETE and SWAP elements File: /MESH/middle_surface_result_to_correct.ansa 1. The middle surface of the depicted part has been extracted using Topo>Faces>Mid.Surface>Casting. The result needs manual correction, in order to achieve a mesh like the one shown in picture 2. 3. Utilities>Delete and delete all the elements at the area of the protrusion where the result is too bad. 4. Elements>Swap at the depicted edge, in order to swap the common edge of the two trias, so that it follows the real feature line of the part.

1

3

2

4

128

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Correcting the middle surface: PASTE-ALIGN grids 1. Grids>Paste>Manual and select pairs of grids, to "clean" the part from very small elements. 2. Grids>Align: Select the highlighted grids and confirm with middle. 3. In the Align window that opens, make sure that Points selection is active. 4. Select the two outer grids, to define a line along on which the previously selected grids will be aligned, and confirm with middle mouse or Next. 5. The alignment result is previewed. Confirm with middle mouse or Finish. ! Note that projection of the grids to the specified line is searched within a distance equal to the Dist value that is set in the Align window (picture 3). If the grids lied further from the line, they would not be affected. 1

2

4

3

5

129

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Correcting the middle surface: ALIGN grids to a plane In order to make the required nodes co-planar: 1. Apply Grids>Align, switch to Entity nodes selection and select the highlighted elements. 2. Confirming with middle mouse, all the nodes of the elements get selected. Confirm with middle again. 3. Pick 3 nodes, to define the plane on which the nodes will be aligned. (If needed, make the MACROs of the initial solid description visible, to inspect which nodes already lie at the mid-plane and are adequate for the plane definition). Confirm with middle mouse. 4. Accepting the result that is previewed, the area is flattened. 1

2

3

4

130

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Correcting the middle surface: CURVEs>MIDDLE / FILL GAP In order to re-create the mesh of the protrusion, that we deleted before, we will first create guiding curves at the correct middle location. 1. Switch to Topo menu. Apply Curves>Middle, select the first highlighted chain of Cons and confirm with middle. Then select the second chain of Cons and confirm with middle again. 2. The middle curves have been created. 3. Repeat the same procedure with Curves>Middle at the other 3 ribs, in order to reach the result of the picture. ! Set those curves to the same part with the shell elements. 4. Switch back to MESH menu and apply Shell Mesh>Fill>Manual. Choose the Perimeters/Curves option and select the highlighted curves. 5. The mesh that fills the gap is previewed, together with the corner points of the Coons FE surface. Choose the Coons Method and press OK button to confirm. Reconstruction of the result is optional and can be activated via the respective flag and repeat the same procedure with the rest of the curves. ! Set those elements to the same part with the rest of the shells 4 3 1 2

C

A B

D 4

5

6 When applying Fill>Gaps with the Coons Method, selecting non-continuous curves/edges, the gaps between them are considered as straight lines for the creation of the Coons FE surface.

131

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Correcting the middle surface: Connect intersecting mesh 1. The created elements groups intersect each other, without being connected. In order to connect them select to apply the Shell Mesh>Intersect>Skin Description. Switch the Work on option to selected and pick all the elements. ! Selection is facilitated using the PID region selection tool. Confirm with Next. 2.The selected elements apear in green. Confirm with Next. ! At the moment, the quality of the created mesh is not of importance. Our goal is to create the correct shape of the part. For this reason, in the Mesh Parameters window, disable any quality fixing, holes treatment etc, so that automatic reconstruction doesn't move nodes away from the feature lines of the part. 1

2

132

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Correcting the middle surface: Connect intersecting mesh 3.The intersected elements have been created. In Intersect Skin Description window enable Improve mesh quality for a mesh of better quality. Confirm with Finish. 3

In order to easily find the needed function buttons and also to avoid switching between TOPO and MESH menus, custom menus can be used. For example, the user can create a menu like the following in order to improve the middle result

133

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Correcting the middle surface: Project Edges to the mesh The next step will be to connect the created shells of the protrusion with the main shell. 1. Shell Mesh>Project>Edges: This function will create corresponding edges at the target elements. Select first the target elements (where projection will be searched). 2. In the Project entities window that opens, enable the Apply fill gap on results, so that the gap between the origin and resulting edges will be automatically filled with shells. 3. Select the origin edges that will be projected to the target mesh. In this example, pick the lower edges of the protrusion. 4. Automatic reconstruction is performed at the target area. Confirm the preview of feature lines and the preview of the result. 5. The parts manager opens, to select the part of the elements that will fill the gap. Select the part of the middle shells. If needed, apply Macros>Orient to assign uniform orientation to the elements of the protrusion, obtaining the result that is shown in the picture. 2 1 3

4

5

134

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Correcting the middle surface: Reconstruct/nodal thick. recalculation 1-2. In order to improve the quality of the mesh, apply Shell Mesh>Reconstruct>Visible. 3.The elements that were created with Fill>Manual do not have nodal thickness assigned. Mesh reconstruction respects the initial nodal thickness. Nevertheless, we will recalculate the nodal thickness of the whole mesh, based on the final location of the nodes, in order to have a more precise result. 4. Apply Topo>Faces>Mid.Surface>Calculate Thickness, by choosing the desired Check Type accordingly. Both Geometry and FE-Model have to be visible. In the Calculate Middle Surface Thickness window insert a Maximum thickness value of 5 and select the Assign to nodal thickness option 5. Pressing OK nodal thickness is automatically recalculated (T1, T2, T3 and T4 fields of the shells are updated accordingly) 1 2 3

4

5

135

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Correcting the middle surface: convert nodal to property thickness 1. If nodes of shell elements have thickness values, there is an option to convert this nodal to property thickness. To do so, apply Topo>Faces>Mid.Surface>Calculate Thickness. In the Calculate Middle Surface Thickness window choose the desired Check Type accordingly, insert a Maximum thickness value and select the Create PIDS with step options. Both check types have to be visible (here geometry and FE-model). 2. Before converting, activate the property list to see the available properties. In the current case, only 2 properties are listed with a default thickness value of 1mm. 3. Pressing OK shells are separated in property groups of the specified thickness range. Enable the property list to see all newly created properties (the selected ones) 1

1

3

2 3

136

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Depenetration

www.beta-cae.com www.beta-cae.com

Identification of penetration cases The function is available under Mesh>Elements>Penetration and Tools>Checks>Penetration.

ANSA distinguishes between the following penetration cases:

Intersections

Flange penetration check using: - property thickness - user thickness - distance range

Interior Intersections: Only when solids involved

Proximities Detect narrow locations on volume parts, before volume meshing

- More targeted identification of penetration cases according to the solver is done by checking the contact definitions through the check function Tools>Checks>Contacts, taking into account all necessary parameters that the solver determines. The choice of using the Checks>Penetration function or the Checks>Contacts option depends on the existence of contact definitions in the FE-model. The Checks>Contacts should be preferred in case contact definitions are available, since ANSA identifies the penetration locations considering contact related keywords of the solver. 138

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Summary of penetrations

139

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Check for penetration due to intersections – file: /MESH/penetration.ansa Tools>Check>Penetration>Intersections: All intersections are listed in the Checks Manager (pic. 1). The context menu (right-click) of the list provides options for visibility handling, access to automatic fix functions and more. As long as the intersections are small (usually deriving from the meshing procedure), they can be fixed with: -Nodal movements, using the automatic fix function Move Away or manual functions (e.g Grids>Move) of the MESH menu (pic. 2). -Local remeshing to create more compatible mesh at the intersected areas (pic 3)

1

2

Big intersections (pic. 4) or extensive intersected areas indicate badly positioned parts or unclean parts. Depending on the case: -Check that the topology is correct and there are no gaps. -Check that faces have been offset to the middle skin in the right direction. -Use the Transform function to relocate a dislocated part to its proper place -Use other CAD functions to locally modify the geometry. -Use the Intersect entitites fix option.

3

4

140

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Check for penetration due to property thickness Tools>Check>Penetration>Property Thickness: Checks all visible shell elements for Thickness Penetration or intersection, taking into account their Property Thickness. The distance used in the check is determined by means of a thickness factor f, to combine the individual thickness of each shell element, as shown in the table below.

Specify the factor value in the Checks Manager window and press Execute:

F11>Presentation Parameters>Draw Shell as Solid draws the shells as solid bricks, helping the inspection of property thickness penetrations.

141

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Check for penetration due to property thickness Fixing property thickness penetrations: 1. Right click on an error in the Checks window and select the Fix option.

2. For LS-DYNA and PAM-CRASH decks only, the Fix method window appears. Select a method and press OK.

3. If the Move nodes option is selected, the message "Please select penetrated PIDs to freeze" appears in the ANSA Info window. The PIDs are highlighted in green. Any PIDs that the user selects change to blue color and will not be moved during depenetration. Pressing middle mouse button, the penetrations are eliminated by automatically moving nodes to a minimum distance. 4. I the Change contact thickness option is selected, a window shows the min/max penetration distances and the user needs to specify a minimum contact thickness value. This value must be lower than the maximum penetration distance. Pressing Enter, ANSA will alter the value of OPTT (LS-DYNA) / TCONT (PAMCRASH). These keywords are defined in the Property card in ANSA. Note: For all other decks, except LS-DYNA and PAMCRASH, the fix command will invoke directly the Move nodes function, so no Fix Method window will appear. ! Note: Property thickness penetration check, takes into account nodal thickness only for the solvers that support it. For solvers where nodal thickness is not valid, it is disregarded and the property thickness is taken into account. 142

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Volume mesh

www.beta-cae.com www.beta-cae.com

Volume Mesh The functions for Volume Mesh generation and handling are available in two locations: 1. From the Volumes group of the MESH module. If the Volumes group of functions is not visible, enable it from the menu that appears by right clicking on the Modules Buttons window header. 2. From the VOLUME MESH module, that provides a lighter menu, dedicated to volume meshing.

1

2

In most cases of structural applications, volume meshing follows a surface mesh generation and improvement. The volume mesh functions will be presented based on their arrangement in the MESH module, in order to avoid switching between MESH and VOLUME MESH modules.

144

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Solid structural shell mesh type In order to obtain a good tetra volume mesh, first a good quality surface mesh with trias must be created. The adequate surface mesh type for components that will later be volume meshed is Solids Structural Mesh. It is suggested to create a surface mesh with stricter quality criteria than the ones that are needed for the volume mesh.

Enabling the tubes treatment, even without prescribing zones, enforces creation of orthogonal tria mesh in the interior of solid holes, thus describing their shape more accurately. Using fillets treatent Default>auto: - The number of rows depends on the specified distortion angle Da and the specified quality criteria and target length. The angle between consecutive edges must be A>180 – Da. - The density of the mesh along the fillets depends on the specified quality criteria and the target length. An example with different aspect ratios is shown in the pictures.

Tubes treatment disabled

Tubes treatment enabled

145

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Volume entity definition There are two modes for the generation of solid elements: - Unstructured mesh that includes automatic tetra, hexa-interior and polyhedral mesh. This mode requires the definition of a closed volume entity in advance, inside which the solid elements will be generated. - Structured semi-automatic hexa and penta mesh. The volume entity doesn't need to be pre-defined. It is automatically created by ANSA simultaneously with the solid elements Creation of Volume entities prior to unstructured mesh generation: Volumes>Define>Auto Detect: ANSA automatically creates volume entities, by finding closed paths among the meshed faces, FE shells and solid facets as shown in the pictures. Finally the VOLUME window opens, listing the detected Volumes.

Additionally, the user can run a diagnostic check prior to definition, in order to detect possible problems related to the volume definition and creation. Those checks are single bounds on mesh, single cons on geometry, degenerated elements, intersections and duplicate elements. ! Function can work either on visible or all the existing meshed entities in the database Volumes>Define>Manual: Function to pick manually the faces (meshed or unmeshed) and/or FE shells and /or solid facets that constitute a volume.

! A boundary of a volume (macro, shell or solid facet) cannot belong to more than 2 volumes 146

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Volume Mesh Algorithms Volumes>Unstructured Mesh>Tetra FEM: tetrahedral mesh mainly for thin to modelately thick Volumes and nearly uniform surface element length, as in most structural applications. Volumes>Unstructured Mesh>Tetra CFD: tetrahedral mesh mainly for large Volumes, with significant variation in length of the surface mesh, as in most CFD applications (pic. 1). Volumes>Unstructured Mesh>Tetra Rapid: tetrahedral mesh adequate for both structural and CFD applications. Tetra FEM/CFD or Tetra Rapid? - Tetra Rapid is about 6 times faster than the Tetra FEM/CFD and creates similar quality. - Tetra FEM though is more robust on Volumes of more complicated shape. The recommendation is to use the Tetra Rapid and if it fails use the Tetra FEM. Volumes>Unstructured Mesh>Hexa Interior: combination of cartesian hexa mesh (aligned to the global or a local coordinate system) inside the main volume and a transition zone to the surface mesh, with a blend of tetra and pyramid elements (pic. 2). Volumes>Unstructured Mesh>Hexa Poly: combination of tetras all around the surface mesh, cartesian hexahedral mesh with variable size inside the main volume and combination of polyhedral and tetra elements in between (pic. 3). 1 2 3

! In case quad elements exist in the surface mesh there is a Create Pyramids option in the options list (and the volumes card) that controls the generation pyramid elements. If the option is disabled, tetra elements with hanging edges are generated instead of pyramids. 147

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Before meshing: Volume mesh parameters The results of the Volumes>Unstructured Mesh> functions can be controlled by the Options List window or the volumes card invoked with double click or right mouse button . For functions Tetra Rapid, Tetra FEM and Tetra CFD parameters are shown in the following pictures:

or 2x

or

Maximum growth rate: Approximate growth factor of solid element size from layer to layer moving towards the interior of the Volume. This value can be set to 1.0 if no element size growth is desired, or up to 3.0 for a rapid size transition. Maximum element length: Limits the growth of tetras towards the interior. By default this value is set to 0, and in this case ANSA will give a warning in the ANSA Info window and use a value of twice the max. shell element. Tetra quality criterion: The quality criterion value will be used as a guide for the algorithm during the quality improvement stage of the volume mesh generation. It is highly recommended to set a value stricter than the acceptable value, in order to obtain the best possible result and avoid the generation of quality violating elements. ! Solid mesh generation requires more time for stricter criterion values. As a general rule, the user can obtain very quickly an initial volume mesh by using the parameters: Max. Growth rate = 1.2 Max. Length = 0 Tetra Quality Criterion: 4. according to Nastran aspect ratio 148

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Recommendations for volume meshing • For the definition of the volume, ensure that there are no: 1. mesh intersections. Use Tools>Checks>Penetration>Intersections. 2. duplicate elements. Use Tools>Checks>Duplicate. 3. Degenerated shell elements. 4. free boundaries. To check manually, deactivate the visibility of perimeter points(via Perim. Points button from Faces Draw toolbar) and activate visibility of perimeters (via Perims Button from same toolbar) in order to see if there are red or cyan bounds that should not exist. Alternatively use Utilities>Isolate>Bounds, or run the diagnostic check from the Volume detect window • To obtain the best volume result, ensure that the surface mesh has no quality violations, according to the specified quality criteria. Fix them prior to voume meshing. • Perform a surface mesh proximity check, using Tools>Checks>Penetration>Proximities. Check whether the identified areas need locall mesh refinement. • In case generation of the volume mesh fails, a respective message is reported in the ANSA info window. Process stops and the checks window becomes visible listing the problem due to which the volume mesh cannot be generated. Fix the problem in order to proceed

149

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Volume mesh quality criteria - F11 Quality criteria are specified from the Quality Criteria – Presentation Parameters window, that is invoked either from Utilities>Quality Criteria or from the respective toolbar button or by just pressing F11. This window will be also referred as "F11 window". The window contains separate tabs for criteria of shells and solid elements. Enable the checkbox of the required criteria and specify the threshold value in the "Failed" column. Choose also the calculation method for each criterion that can be calculated based on more than one definitions. -> Saves quality criteria settings in text files, with the extension .ansa_qual. -> Loads quality criteria from .ansa_qual files. The current quality criteria are contained in Quality criteria of the Volume scenario In order to display only selected criteria in the F11 window, apply Edit Criteria Visibility and choose the criteria. Place the cursor over a criterion in the F11 window, to see a tooltip that explains the criterion definition.

150

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Quality check: Hidden view mode Quality check of solid mesh is done in the same way like the shell mesh. Activate Hidden from the Drawing Styles toolbar, in order to view elements according to the criterion they violate.

1

3

A color legend with the visible criteria is displayed. The number of violating solid elements is shown in the Volume elements index (OFF). 1. A criterion can be activated/deactivated by clicking on its name in the color legend. Right-clicking on the color legend, a context menu appears. From this menu, the threshold value of a criterion can be changed and solid elements that violate a specific criterion can be isolated (Show/Hide/Show Only). Also, the element of worst quality can be isolated via Show Only Worst. Choose the option Hide Inactive Criteria, to make the color legend shorter. 2. The legend and the elements index can be moved in a different location of the screen, by drag and dropping them with the middle mouse button. 3. Apply right-mouse button and Show Only, to leave visible only all violating solid elements. To locate more easily the element of worst quality, use Show Only Worst from the same context menu. 151

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Volume mesh improvement: Fix quality Quality improvement can be done either manually (applying Improve>Move, Paste, Align, Mesh>Elements>Split>Solids) or automatically. The automatic functions for solid mesh improvement have some differences than in shell mesh: Volumes>Improve>Fix Quality: fixes all types of solid elements except polyhedral. It takes into account all active criteria in the Solids tab of the F11 window. Nodes of the external surface are allowed to deviate from the surface, depending on the External and PID bounds movement settings of the Options List or Volume mesh tab of the Mesh parameters window: External bounds movement: the max distance that nodes are allowed to deviate from the external bounds PID bounds movement: the max distance that nodes belonging to different PIDS are allowed to move The options that are available for the above settings are: Constrained: the user allows the movement of the nodes far from the boundary for a limited distance (Maximum distance from external bounds or Maximum distance from PID bound). Distance can be either a constant value or a value relative to the local element length Unconstrained: the nodes on the bounds (external or PID) can be moved without any limitation Freeze: no movement is allowed on the bounds (external or PID)

and

152

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Volume mesh improvement: Reconstruct - Smooth Volumes>Improve>Reconstruct: Works on tetra and pyramid elements only. It remeshes the selected solid elements based on the criterion that is specified in the Options List window. It doesn't take into account the criteria of the F11 window. Nodes at the external surface are never affected. Solid mesh reconstruction can provide a solution by setting a stricter criterion in the Options List window and reconstructing small areas around violating elements. Volumes>Improve>Smooth: Improves the flow of the solid mesh (...and of the overlying surface mesh, if Freeze Volume Skin is disabled). No quality criteria are taken into account. If the quality problems derive from a bad surface mesh, then the shell mesh must be handled. Note that SHELL MESH>RECONS can be applied on shells that lie on top of solids or directly on the solid facets, only if local remesh is chosen for the Attached solids in the Options List Reconstruct solids from mesh menu: When Reconstruct is used from MESH menu and there are solid elements attached to shells, then an option is available to remesh or not the underlying volume mesh. If the Attached solids option is set to local remesh, the solids are remeshed. If it is set to freeze skin, then reconstruct doesn’t affect both shell and solid mesh.

153

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Surface to volume mesh extraction Using the functions under Volume Mesh>Improve, volume meshes with hexahedral and pentahedral elements are created. Volume mesh is extracted from a surface mesh of one or more selected meshed Macro Areas, or FE shells. The extracted tria shell elements form pentas and the quad elements form hexas. For these functions there is no need to predefine a Volume entity. Some examples are shown in the pictures below: Volume Mesh>Structured Mesh>Translate

Translation vector

Volume Mesh>Structured Mesh>Sweep:

154

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

MAP volume mesh (1) – file: /VOLUME/MAP.ansa Structured Mesh>Map creates hexa and penta elements by node interpolation between opposite Macros or FE shell areas, a Master and a Slave set. The Master and Slave sets don’t have to have the same geometrical shape. This kind of solid meshing doesn't require the definition of a Volume entity in advance. The Volume entity is automatically created after generation of the solids.

1 Structured Mesh>Map. Select the Master area and confirm with Next or with the middle mouse button. 2. Select the Slave area. 3. The bounding macros are automatically selected (Round area). Make sure that all the macros of the boundary are selected. If needed, select/deselect macros. 4. Specify the number of solid layers (Steps) that will be created between the master and the slave area. By default, the number of quad rows of the round is 3 used (in this case 16 steps).

2

4

! Once defined a MAP type volume mesh can be easily remeshed, if its is erased due to some reason, using Volumes>Remesh function

155

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

MAP volume mesh (2) 6 5 5. Provided that you have the Preview solids option from the Options List window checked, the solid mesh is previewed. Notice that the mesh of the slave area is altered, in order to become compatible with the master area. Upon confirmation, depending on the Part and Property selected options in the options list window, the Model browser and the property list will open to assign the newly created volume to a part and a property. 6. The solid mesh is created. Penta elements connect the trias of the master and slave areas, while hexas connect the corresponding quads. - The slave area doesn't need to be meshed. The mesh of the master area will be mapped to it. - If the round contains trias or is unmeshed, the Structured Mesh>Map function will try to mesh it automatically with mapped quads. Pure quad mesh at the round is a prerequisite fom mapped volume mesh generation. - Alternatively, the map algorithm can work without any round. In this case, the transition from the master to the slave area is straight, as shown in picture 7. 7

156

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

MAP volume mesh (3) – file: /VOLUME/MAP_multi.ansa When working with parts that have multiple master areas, you can select more than one faces to start mapping. First, select all the areas of the model at the different steps. Then, select all the opposite slave areas that have not to be meshed necessarily. The round area will be selected automatically, or select with box selection all the remaining nonselected faces. If more than one master area is recognized, we should select the face from which mapping will start.

Working with thin Parts: When working with thin Parts that require solid mesh it is recommended that the MAP function is used with method of Thin parts.

157

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Managing Volumes The VOLUME window (accessed form Volumes>List or from the DB Browser) provides a complete overview of the Volumes, access to quality statistics and also meshing and deleting operations. Edit: Access to the Volume card for parameter changes (Name, PID, max length, etc. depending on the Volume type). Set Pid: Modify the Property of selected Volume entities. Info: Extract volume quality statistics (for unstructured Volumes). Remesh: Remesh selected Volumes (if they are in remesh status after a modification in the edit card or because they were erased due to a change on their surface mesh) or mesh from scratch any unmeshed Volumes. ! Remesh uses the parameters from the Volume edit card and NOT from the Options list.

Erase: Erase the solid elements of a Volume but keep the Volume definition in the List Delete: Delete both elements and Volume definition. Redefine: Enables the modification of the definition of the Volume (add or remove surfaces). Freeze/Unfreeze: Freeze or Unfreeze the macros of the selected Volumes. In case the Shell Mesh>Erase function is applied on a bounding Macro Area, the included solid elements, are erased as well, due to the relation of the Volume with its bounding Macro Areas. The function Volumes>Release detaches the solid elements from the Volume entity (which now remains empty) and become FE model solid elements.

158

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Assembly

www.beta-cae.com www.beta-cae.com

Connections - Terms and presentation Connections are ANSA entities, that carry information like connection position, connected components (also referred as connectivity information) etc. Elements and constraints that represent the connection (FE-representations) can be automatically generated by "realizing" the connections from the Connection Manager of ANSA. The FE-representation of a connection can be easily changed, in order to serve different purposes (e.g use different elements for durablitity and crash simulations)

Points: Spot Weld Points appear as circles, symbolizing the number of connected parts with diameterlike lines. Spot weld poitns with 0, 1, 2 and 3 connected parts are shown on the left. Gumdrops appear as two concentric circles, symbolizing the number of connected parts with diameter-like lines. A gumdrop with 2 connected parts is shown on the left. Gumdorps are very much alike with spot weld points, but they can also carry the information of mass to be added at each position. Bolts appear as hegagons.

Lines: Spot Weld Lines, Adhesive Lines, Seam Lines and Hemmings appear as magenta curves.

Faces: Adhesive Faces appear as faces with magenta boundaries. They are treated as Macro Areas, i.e suitable mesh can be generated on them, in order to guide the generation of surface or solid adhesive elements.

Handling of connections is done from the Assembly toolbar, where all relevant functions are grouped together. 160

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

1D Connections – Spot Weld Points Some characteristic FE-representations of Spot Weld Points are shown in the pictures below:

Before realization

Point-to-point

Mesh independent

Spider pattern

161

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

1D Connections – Bolt

162

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Spot Weld Lines Spot Weld Lines generate the same FE representations as Spot Weld Points. The difference between these two connection types is the way that the locations of the welds are specified: The welds are generated along the Spot Weld Line, based on the specified spacing (S) and margin (M):

S can be a positive or negative or negative real number. A positive S value implies that upon realization, priority will be given to the preservation of the margin value (M). Thus the resulting spacing may vary between S and 2S. A negative S value implies that priority will be given to the preservation of the spacing.

163

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Adhesive lines – Seam Lines Adhesive lines: The user has to specify the width (W) and height (H) of the glue line. If no H is specified, it is calculated based on the distance of the connected flanges. An alternative definition of the width can be done by specifying a diameter value (D): If no W is specified then W*H=3.14*D2/4 Some FE representations of adhesive lines are shown below:

Before realization

Hexas with RBE3s

Hexas pasted on the shells

Seam lines: For most FE representations, a seam line searches for feature lines within a search distance. If a feature line is found, then the connection element is generated between the feature line and its projection on the other connected part. Otherwise, the connection element is generated between the projections of the connection line on both parts

Before realization

Rigid elements

Shells with Heat Affected Zones

164

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Hemmings – Adhesive Faces Some characteristic FE representations are shown below: Hemming:

Before realization

Folded shells with hexas and RBEs

Adhesive Face:

Before realization

Hexas with contact

165

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Drawing Styles

From the CNCTN. switch button in the Visibility toolbar, choose how to draw the connections of the model.

166

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Import of connections Usually connections are created by direct import of connection files. ANSA can input some common connection file formats directly, through the File>Read connections function. A brief description of the formats follows in the table below.

Any other connection file format can be imported in ANSA with the aid of scripting.

167

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Convert 3D-Points to connections Activate the Assembly>Convert>3D points Punction and select the 3d points to convert. Confirm with middle mouse and specify the connection type in the Connection Type window. The connections that are created carry as connectivity the module id of the part specified in the options list window. The connectivity will need to be correctly defined by the user, with the aid of the Connection Manager functionality.

In some cases, the location of connections (x, y, z coordinates) may be available in a txt file. 3D points can then be easily created with the function Topo>Points>New>Num. Input>Import CSV.

What if a wrong connection type has been chosen? Apply the function Assembly>Convert >Cnctn to Cnctn (e.g in order to convert Spotweld Points to Gumdrops). 168

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

User defined connections - Auto When no connection information is available, Connection Entities can be created in ANSA: 1. Apply Assembly>Define>Auto, select a chain of faces and press middle mouse button to confirm. 2. The SPOT-POINTS DEFINITION PARAMETERS window opens, where the user can specify the number of Spotweld Points to generate or the distance (spacing) between them. The margins from the start/end of the selected faces middle line are also controled by the respective options. 3. The effect of any change of the parameters can be inspected: The spotwelds are previewed, distributed to all selected Faces, along a path that runs along their middle. Upon confirmation with the OK button, the connection points are created. As connectivity, they carry the property or the module id of the selected faces, i.e they appear as connecting a single component. Therefore, the connectivity information needs to be corrected using the functionality of the Connection Manager. ! This function is applicable to areas with well defined parallelogram shape. 1

2

3

169

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Creating connections manually – Define connectivity Using the Assembly>Define>Manual function, Connection Entities are defined manually by picking positions on Faces or shell elements (in the case of FE-Model mesh). With this function, the user will first specify the connectivity information of the Connection Entities to be generated and then their location and type. For the definition of the connecitivy, consider the following options:

Single part per Pi: This is the most common option to be used. Select the parts/properties that will be connected and confirm with middle mouse button.

Multiple parts per Pi: Applicable in cases when at least one of the connected flanges consists of faces that belong to different parts/properties. E.g suppose that one connection line needs to be created, that will connect the group of 4 properties of the upper component with the lower component. First select the top PIDs and terminate the selection of the first group with middle mouse button. Then select the PIDs of the second group (in this case there is only one PID) and confirm with middle. Press middle again to terminate the selection of goups.

2x 170

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Creating connections manually – Connection points Single welds: • After selecting the components to connect, activate the Single connection point toolbox. • Choose the adequate Connection Type (in this case SpotWeld Point) • Point on face selection mode: Select arbitrary locations on the elements of the involved components. • Point selection mode: Select existing grids or 3d points. The connections are created upon confirmation with middle mouse button.

Multiple welds – flexible weld paths: • Activate the Multiple connection point toolbox. • Being in Point or Point on face selection mode, the weld path is specified as a polyline or curve created by the selected points. Connection points are created based on the specified spacing and margin. As both spacing and margin may not be able to be respected, based on the length of the line, the Keep margin/spacing option is provided.

Form: Curve

Form: Polyline

171

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Creating connections manually: Overlapping edges / Curves Multiple welds – between overlapping edges: • Activate the Multiple connection point toolbox. • Being in Perimeters or Edges selection mode, the Form section provides different options than in point selection. The weld path can be defined either from the curve that is directly specified from the selected perimeters/edges or from their middle curve. • The middle curve option is adequate in cases when two large flanges overlap. • Select the opposite outer perimeters. The middle curve is automatically calculated and connections are distributed according to the specified margin/spacing.

Connection curves: • Activate the Connection curve toolbox. • Connection curves of any type can be created using similar functionality for the curve definition as described above for multiple connection points. ! In case more than one parts where initially selected, use the Center connections option to position them between the 2 selected parts 172

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Check connection definitions Before generating FE representations for connection points, it is advisable to check their definition by applying the function Tools>Checks>Connections.. Some checks are explained below: • Number of parts Auto - Connect 2. Specify the search parameters in the Auto Edit Parameters window. 3. Upon confirmation, the Pi fields are filled accordingly.

1 2

3

179

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Connections elements generation section

180

In the FE Rep settings section the user can set-up the options and parameters that will be taken into account for the generation of connection elements. When the Realize button is pressed in clipboard mode, all visible settings are applied. When the Realize button is pressed in dynamic mode, all assigned settings are applied. If no settings are assigned and Realize button is pressed, no application/realization will take place. The FE-representation settings appear in color groups, according to the FE model characteristics they affect. The library of FE-representations for each connection type is found in the FE Rep Type entry and is accessed through the pop-up menu on the right. The first column, with the blueprint icon, signifies that the settings have been acquired by a connection template. Leaving the cursor on any item,a help balloon pops-up with the description of the setting. ! Attention must be paid in the Search Dist field that appears for all FE Representations. If a connected component lies further from the connection location, realization will fail. If the Seach Dist is left blank, a value of 10 is assumed. Pressing the Realize button, the visible settings will be applied to the selected connections and the FE-connection models will be generated. Erase FE erases the FE-representation of a realized connection. There are two view modes for the FE Rep. Settings: The dynamic and the static mode, or else clipboard. The dynamic mode (default) allows the set-up of the FE-representation, while, at the same time, the window displays the current settings of the selected connection. This means that while the selection of connections changes, the settings displayed in the window are updated, in order to reflect the settings of the connections currently selected. The dynamic view provides a real-time comparison between the settings of the selected connections and displays the non-common values grayed out. The clipboard provides a static card for the set-up of the FE-representation. The user can switch from one mode to the other through the toggle button at the top. ! Connections read from a connection file or connections generated in ANSA do not have any FE-representation settings at first. Thus, the list may appear empty when in dynamic mode. Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Troubleshooting the Connection Manager

181

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Connection Manager – Selection Assistant Activating the Connection Manager from the corresponding button of the Assembly toolbar on top of ANSA main window, the user can select the connection entities to work with. Selections can be made either with mouse, from the drawing area, or using filters, with the aid of the Connection Selection Assistant window automatically invoked by the Connection Manager. It provides a number of filtering options and fields that form logical expressions for the selection and the visibility control of Connections in two available tabs: Quick Filter and Advanced Filter. Some examples are provided below: 1. In Advanced Filter tab, having visible two parts of an assembly, specify Search as Visible Connectivity and Type as Spotweld. Press Select. All the spotwelds of the visible parts (even the ones that connect them with other parts) are displayed. 2. Press Deselect and change the Search to Visible Connectivity Only. Press Select again. Only the spotwelds between the two parts are selected. Upon confirmation with middle mouse button, the Connections Manager will open. 1 3. The same filtering and selection concept applies for the Quick Filter tab, as displayed in the picture below. 3

4 2

4. More filters can be added from the + button. Using the All Fields option, any attribute of the connections can be selected to be used for filtering.

182

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Bolt definition Bolts can be defined either using the functionality of ANSA Connection entities or (more manually) using the BOLT tool. Automatic definition of ANSA Connection entities: Apply Assembly>Define Connection>Holes to automatically create bolt connections at the identified holes/tubes of the model. Then use the Connections Manager to generate the FE-Representation of the bolts

Manual bolts creation with Decks>Auxiliaries>Bolt: Feature lines or Nodes selection options: Manually select the edges or nodes of each bolt hole respectively. ! Confirm with middle mouse button after finishing selection of each bolt hole. Panels option: Select groups of elements. The corresponding bolt holes of the selected areas are automatically identified, based on the specified Tolerance (i.e maximum distance between opposite holes) and Diam (diameter) range. Create entities section: Specify the type of elements that will be generated for the body, head and nut of the bolt. Moreover, specify the edge zones arround the hole (inner, outer or both) that will be connected withy the bolt elements. Using the Connection Defined by option, an ANSA Connection entity can be created as well. Changing the settings of the connection in the Connection Manager, the bolt FE representation can be easily changed.

183

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Connectors Connectors are generic ANSA entities that are used to connect two or more parts or sub-assemblies, modeling the kinematic constraints that exist between them.

Use as connectivity ANSA Parts/Groups, properties, includes, sets Search for geometric features or in spherical/cylin drical /hexahedral domains Attach to structure via rigid/interpolation elements or any custom FE-entity using script

Connectors are managed from the CONNECTOR_ENTITY list that opens from Decks>Auxiliaries>Connector. The edit card of the Connector contains all the necessary information for the connected components and how to connect them: -“Generic” information (what/where to connect) -“Application” information (what elements to generate) Elements are generated by selecting the Connector from the list and pressing Apply.

Use as representation any built-in FE-entity, custom library item or script

184

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Check connectivity – Identify loose parts After creating connection elements between the components of a model, it is suggested to check the model for unconnected parts. Activate Tools>Checks>Connectivity and select the option Detect unconnected assemblies in the Check Connectivity mode window. As long as unconnected areas exist in the model, they are listed in the Check manager window:

Alternatively, in the Check Connectivity mode window use the option Interactively inspect assembly’s connectivity. First pick an element, from which the search of connecting paths wil start and enable Check for unconnected assemblies. If Check visible only is inactive, check is performed on all database entities. Pressing OK, only the unconnected parts remain visible

185

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Keeping the assembly up-to-date - Replace part When an updated file for a part or sub-assembly (group) is available, it can be incorporated in the ANSA database using the functions Replace or Compare that are accessed from the Model browser. Using Replace, ANSA investigates any entity of the outgoing part that can be maintained and reapplied after the replacement. For this ANSA will ask the user to decide whether to keep entities like Connections and Connectors. Furthermore, ANSA will ask whether to try to paste nodes connecting the outgoing part with the rest of the assembly, according to names or based on proximity. The respecive options are specified in the Replace Part options #1 and #2 windows.

The results of the performed actions, are summarized in the Replace Part Report – Reapply options window that opens. At this point the user can navigate among the provided information, using optionally the filtering capabilities, and accept to proceed (pressing OK) or go back to change some of the previous selections (pressing Reapply). Upon acceptance, the Final Replace Part Report window opens.

186

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Keeping the assembly up-to-date – Compare The Compare functionality allows the full comparison of two parts or whole assemblies, for the identification of differences in geometry, attributes, solver-specific definitions, as well as Connections and Connectors. It is activated from Tools > Compare or from the corresponding icon on the Tools toolbar.The model currently in use can be replaced or can be partially updated according to user directions. Activate Compare>With Current. The incoming model may derive either from an ANSA file or a solver input file or a default-format connections file.Press Next and in the scenario tab select the comparison scenario. Press Finish and the Compare report window appears

Handling, visibility, comparison options

List of differences

187

In the upper side of the window the user has various options regarding the manipulation of the comparison list and the visibility of the two models. In the left and right section of the window, all the results of the compared entities are listed. The two lists are synchronized, so when items of any of the two lists are selected or expanded, their matches of the other side will be selected or expanded too. By default, the results are presented in flat view. In the main area of the window, all the compared entities are listed. Two view modes of the list are available: Tree list (for comparison according to the part/group hierarchy) and "flat" list (entities organized by type)

Upon confirmation with the OK button, replacement takes place. The affected Connections and Connectors are automatically re-applied. Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Model management – Introduction to pre processing decks

www.beta-cae.com www.beta-cae.com

DB Browser The Database Browser provides overview of all entities that exist in the model. Invoked from Containers>Database or from the respective toolbar button Visibility control of individual entity types from the Visible column. Double-click on an entity group to open the corresponding List. Context menu with options for visibility handling (Show/Hide/Show only), opening of lists and creation of new entities.

Includes, Filters and Sets can be activated from the corresponding buttons of the same toolbar and docked accordingly, as displayed in the picture.

189

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

List Handling 1. Context menu with options for handling of the selected entities, e.g: -Visibility control -Massively Modify attributes -Reference: open a list with the entities that use the seleced ones -Save List in a text file -Output only selected entities of the list 2. The options of the context menu appear also as buttons at the bottom of the list, by pressing the lower left arrow button. 3. Every field of the edit card of an entity can be dispayed as a column of the list. Select the columns to display, by pressing the top right arrow button: Either type the name of the field or press List fields to select among all the available fields. 4. The edit card of an entity opens with the Edit option or with double-click on an entry of the list.

3 1

2

190

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

List Handling – Entity Card The entity card corresponds to the solver card. The displayed fields depend on the current solver deck. F1

?

F7 F1

F2

F2

F1: Pick from screen F2: Directly open the edit card of a referenced entity ?: Open HELP list to select entity F7: Zoom in the referenced entity Leave the cursor on a field to get a tooltip regarding its meaning according to the solver

191

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

List Handling - Filtering 1. Simple filtering: Type the filtering expression directly in the filter widget. Expressions are written in the form: :. A compo box with filtering suggestions appears while the user types. E.g when typing numbers (without typing the field label), suggestions for filtering of ids are given. 2. Advanced filtering: Predefined filters are available (selected/visible/current/unused). Option to create user defined filters (New/Edit) 3. Pressing New/Edit the Advanced Filter window opens, providing an interface to: Create new filters (from the context menu of the Filter Name section) or edit existing ones. Specify the Filter Rules. Activate the selected filter by pressing Apply.

1

2

3

192

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

List Handling - Modify Massive modification of fields of all selected entities is done in two ways: Quick modify: Right-click on the label of a column and type the new value. This way the user is able to modify the contents of a single column only Modify option of the entities context menu. Using this option the modification rule can be saved in the ANSA.xml file and used again and additionally modification can take place to more that one columns simultaneously. To perform such a modification, press right mouse button in the open space of the lists window or select from the list the entities to be modified, press right mouse button and select Modify. An interface for the definition of modification rules opens. Type the modification rules manually in the Modify Rules section (tab completion is supported). Once finished, press OK to

apply the modification ! Note that in order to get the value from a field, you have to type it exactly as it appears in the entity’s card. Here for example, the OPTT value will be the result of subtraction of 0.3mm from the real thickness value which in the property card pf LS-DYNA, appears as T1

193

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

List Handling - Modify A warning window appears in case there are entities that failed the modification. Pressing OK, the Property>Failed Modification window appears, listing all the failed entities

The property list is updated with the new values in the columns

194

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Useful expressions for Modify Modifications can be done either by specifying a new value for all selected entities or by using expressions. Some characteristic examples of the expressions syntax in ANSA are shown below.

Renumber all selected entities so as to start from 10

COUNTER+10

Add at the end of property names “T=”

$.” T=“.T

Substitute with“_” in names

tr($, “ “, “_”)

Substitute the keyword “RAIL” by “BEAM” in names

subifm ($, “RAIL”, “BEAM”)

“$” stands for the “current” value. Type a field name directly to reference it as a variable in an expression.

195

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

ANSA Sets Access the Sets list from: - Containers>Sets or from the respective toolbar button Decks>Auxiliaries>SET A set can be created by: - Choosing the New option in the SET list or - Drag & Drop entities in the New Set box that appears in the SET list (picture 1)

Modify the contents of a set e.g by: - Drag & Drop entities to the entry of the Set in the SET list or - Selecting the set and choosing the Modify Contents option of the SET list (picture 2).

1

2

196

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

ANSA Sets – Modify Contents When a set is created with the New option or when the Modify Contents option is applied, the Modifying SET window opens in order to select/deselect entities. The window resembles the Database Browser. Click on the type of the entities to be added or removed. The list of the entities opens. Select entities either from the list or from the screen and press OK. ! Note that if entities of the same type have to be added in the set, user has to select them with CTRL button pressed.

2x

197

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Creating line elements All types of line elements or constraints that use 2 nodes are created with a similar interface. For example, apply NASTRAN>Element>CBAR

Pick mode: Nodes. Select the required nodes, either in pairs or sequentially.

B D A

C

F E

Pick mode: Node sets. Select two groups of nodes. Line elements are created based on the Node set connection parameters.

The type of existing line elements can be changed (e.g convert CBARs to CBEAMs) from DECK>Elements>UTIL>Change Type>1-D Entities 198

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Creating rigid elements with many nodes Handling of rigid elements with many nodes is similar for all solver decks and rigid element types. For example, apply NASTRAN>Elements>RBE2>Many Nodes. 1. The wizard opens and prompts you to select the slave nodes of the rigid elements from the screen and confirm with middle mouse button, or press the Next button. 2. Next step is to specify the master node. Either select an existing node or do not select any node. Just press the middle mouse button (or Next button), as shown in the picture. The master node is then automatically created at the geometrical center of the previously selected nodes. 3. As a last step, define the degrees of freedom in the CM field and press Finish. 1

2

3

Alternatively, definition of the RBE2 can be done with the aid of ANSA Sets. Apply NASTRAN>Elements>RBE2>Set. From the SETS HELP list that opens, select an existing set or press New to create a new set without exiting the function. Continue with selection of the master node as described before. The selected set doesn't need to contain directly grids. E.g if a set with properties is selected, then all the grids of the elements of the properties will be connected to the RBE. Creation of elements on Set is available in ANSA, even for solvers that do not support this kind of definition. In such cases, by File>Output, the elements will be written as required by the solver. ! In order to change the nodes that are connected to the rigid element, apply NASTRAN>Elements>RBE2>Branch. 199

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Includes (1) Include files are handled from Containers>Includes or from the respective Containers toolbar button. Includes are created: 1. By File>Input, when INCLUDE statements exist in the input file ! Includes named Auxiliary_ are created automatically by ANSA during input and contain the keywords found inbetween INCLUDE statements. The Auxiliary includes ensure that when the file is exported again (File>Output) it will maintain its original structure. 2. By File>Input with the Input in new Include option, when importing any input file. 3. Manually in ANSA, with Drag & Drop of entities in the Includes tab of the DB browser. 4. Directly from ANSA parts/groups, using the Utilities>Parts To Include option of the Model browser. 1

2

3

4

200

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Includes (2) OUT OF INCLUDES: All entities that do not belong to any include. New entities are automatically assigned to the OUT OF INCLUDES. Set an include as Current (option available in the context menu), in order that new entities be assigned to it.

Exporting a file with Includes (File>Output): Normal mode (when inline and read-only are deactivated): An INCLUDE statement is written in the main file and a separate file is generated for the include. Inline: The contents of the include are written directly in the main file. No separate file is generated. Read-only: An INCLUDE statement is written in the main file, but no separate file is generated.

The Auxiliary includes that are automaticaly created by ANSA are always marked as inline. 201

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Renumber entities Functions for quick renumbering of nodes or elements: - Utilities>Renumber or - from the corresponding Utilities toolbar button Elements>UTIL>Renumber. Renumbering of entities of any type, according to user specified rules: Invoke the Renumber Tool from Utilities>Renumber>Edit. Model Entity Groups section: Select the entity type for which a numbering rule needs to be created. Numbering Rules section: Specify the settings of each rule. E.g ranges (From/To), entities to renumber (Select), Force renumbering in case of already occupied ids etc. Special Rules section: Definition of special rules for elements and nodes of specific Properties, Parts/Groups, Includes etc. Renumbering is applied by pressing the Renumber button.

202

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

File output Apply File>Output. The Output Parameters window opens. • General tab: Output All/Visible/Model. Using the Model option, any unused entities will be excluded from the output file. The ANSA Comments contain information that can be used from ANSA when inputting the file again (File>Input), e.g parts/groups hierarchy, entity card comments, colors etc. • Filter tab: Advanced options to write or not some entities.

• Miscellaneous tab: Options that depend on the solver deck. The option Output element's thickness controls how to output elements that have nodal thickness defined in the element card.

203

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

EPILYSIS: set up and run a model for static analysis in ANSA

www.beta-cae.com www.beta-cae.com

Introduction to Epilysis Epilysis is an implicit Finite Element Method solver, available within the ANSA/EPILYSIS/META suite, covering numerous solution types. It may be used by an engineer involved in CAE and is available since version 16.0.0. It operates either as standalone software or through ANSA interface. Epilysis, uses the same entities and solution types as NASTRAN. The supported solution types in brief are:

• SOL 101: Linear Static Analysis • SOL 103: Real Symmetric Eigenvalue Analysis • SOL 108: Direct Frequency Response • SOL 111: Modal Frequency Response • SOL 109: Direct Transient Response • SOL 112: Modal Transient Response • SOL 400 (Linear Contacts): Quasi-Static analysis with linear elements and nonlinear contacts

205

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Statement of the problem– file: EPILYSIS/epilysis_model.ansa 1. Consider the model shown in picture. A force of 1000 (N) is applied along the Z axis. The displacements, as well as stresses and strains need to be computed. Model is constrained with single point constraints (SPC1).

2. Consider the same model of the above picture. A moment of 1000 (N mm) is applied around the X axis. The displacements, as well as stresses and strains need to be computed. Model is constrained with single point constraints (SPC1) at the same locations

206

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Boundary conditions definition In order to define boundary conditions on the model, single point constraints need to be created: 1.Select DECK:NASTRAN>Bcs > SPC > SPC1 > Set 2.In the window that will open pick the predefined Set 3.In the C field of the SPC1 card type 123456 in order to constrain all degrees of freedom 1

2

! Note that each time a boundary constraint is defined from the BCs group of functions, a corresponding B.C. Set is created automatically. Boundary conditions that affect the same subcase, should have the same SID in the boundary condition card ! In order to make visible the SPC1, activate the corresponding flag buttons in the database browser

207

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Loads definition 2 kinds of loads are going to be applied for the analysis. A force along the Z global axis and a moment around x global axis. To define the force select 1. BCs > FORCES > Node 2. Pick the Master node of the RBE2 3. In the FORCE card that will open type 1000 in the F field in order to specify the magnitude of the force and 1 in the N3 field in order to give the orientation vector of the force along the global Z axis. 2

3

Master node of the RBE2 To define the moment select 1. BCs > FORCES > Node 2. Pick the Master node of the RBE2 3. In the FORCE card that will open switch to MOMENT the TYPE field and type 1000 in the F field in order to specify the magnitude of the moment, 1 in the N1 field in order to give the orientation vector of the moment around the global X axis and 2 in the SID field. 3

208

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Set up the Header The modelling phase is completed. The header of this model will be set up with the required load cases regarding linear static solution (SOL 101) 1. Activate the B.C. SETs>HEADER>New 2. From the Executive Control section , double click to SOL and in the respective window that pops up, select 101 SESTATIC: Statics. Press OK. The respective solution is inserted in the Text edit section of the header window. Optionally insert a title and a subtitle to describe the analysis in a better way.

1

2

2x

209

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Set up the Header: select loads and constraints In the Case Control section we are going to select the loads and constraints of the model and define the subcase structure for the analysis 1. Navigate through the Case Control available options and double click to DISPLACEMENTS and select to output results for ALL model. 2. Repeat step 1 and select STRESS and STRAIN to be computed for ALL model as well and SPC=1 as well ! DISPLACEMENT, STRESS, STRAIN and SPC apply to both subcases. For this reason they have to be placed above the subcase level.

1

2

210

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Set up the Header: subcases The Case Control section includes 2 subcases. Subcase 1 corresponds to the first loading condition (Force along Z axis) while the second subcase defines the second loading condition (Moment around X axis). 1. To define them, switch to the Subcase List tab. 2. Press right mouse button and select New 3. A new subcase is created. On the subcase, press right mouse button again and select Edit 4. Type the necessary loads and constraints and press OK

1 2 3 4

211

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Set up the Header: subcases 1. Switch to the Text Edit tab. The new subcase is added. 2. In order to add a second, copy-paste the text and 3. Make the appropriate changes in the corresponding lines(TITLE, SUBTITLE and LOAD) 1 2 3

! Activate the subcase so that it will participate in the current header definition ! In a similar fashion, we can define the second subcase 212

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Set up the Header: parameters In the Parameters specify PARAM POST = -1 (in order to output the .op2 file that will be read by META post processor) and press ok. File is ready to run.

213

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com

Run the model in ANSA ! Prerequisite : Before running the model, check the whole model through the Check Manager. Apply Tools > Check Manager > NASTRAN Checks > To Checks > Execute In order to solve through ANSA interface, select the NASTRAN deck. Apply EPILYSIS>SOLVE>IN ANSA. In the Analysis tab window define the entities that will be considered (All), and the name of the job

In the Options tab, define among others: the scratch directory where the scratch files will be output and the maximum amount of memory of the analysis. Optionally, activate to start automatically META when solving is finished

Go back the Analysis tab and click Start. The status of the solution and the possible errors will appear in the Epilysis window Start META to post process the results

214

Introduction to pre processing with ANSA v17.1.2

www.beta-cae.com