HyperMesh 2019 Core Tutorials [PDF]

Zitiervorschau

Altair HyperMesh 2019

Core Tutorials

altairhyperworks.com

Intellectual Property Rights Notice Copyrights, Trademarks, Trade Secrets, Patents & Third Party Software Licenses Altair HyperMesh 2019 Copyright 1990-2019 The Platform for Innovation™ Altair Engineering Inc. Copyright © 1986-2019. All Rights Reserved. Note: Pre-release versions of Altair software are provided ‘as is’, without warranty of any kind. Usage of pre-release versions is strictly limited to non-production purposes.

Altair HyperWorks™ - The Platform for Innovation™ Altair AcuConsole™ ©2006-2019 Altair AcuSolve™ ©1997-2019 Altair ElectroFlo™ ©1992-2019 Altair ESAComp™ ©1992-2019 Altair Feko™ ©1999-2014 Altair Development S.A. (Pty) Ltd.; ©2014-2019 Altair Engineering Inc. Altair Flux™ ©1983-2019 Altair FluxMotor™ ©2017-2019 Altair HyperCrash™ ©2001-2019 Altair HyperGraph™ ©1995-2019 Altair HyperLife™ ©1990-2019 Altair HyperMesh™ ©1990-2019 Altair HyperStudy™ ©1999-2019 Altair HyperView™ ©1999-2019 Altair Virtual Wind Tunnel™ ©2012-2019 Altair HyperXtrude™ ©1999-2019 Altair MotionSolve™ ©2002-2019 Altair MotionView™ ©1993-2019 Altair Multiscale Designer™ ©2011-2019 Altair OptiStruct™ ©1996-2019 Altair Radioss™ ©1986-2019 Altair SimLab™ ©2004-2019 Altair SimSolid™ ©2015-2019 Altair nanoFluidX™ ©2013-2018 Fluidyna GmbH, © 2018-2019 Altair Engineering Inc. Altair ultraFluidX™ ©2010-2018 Fluidyna GmbH, © 2018-2019 Altair Engineering Inc.

Altair WinProp™ ©2000-2019; Altair ConnectMe™ ©2014-2019; Plus other products from the Altair solidThinking Platform.

Altair Packaged Solution Offerings (PSOs) Altair Automated Reporting Director™ ©2008-2019 Altair GeoMechanics Director™ ©2011-2019 Altair Impact Simulation Director™ ©2010-2019 Altair Model Mesher Director™ ©2010-2019 Altair NVH Director™ ©2010-2019 Altair Squeak and Rattle Director™ ©2012-2019 Altair Virtual Gauge Director™ ©2012-2019 Altair Weight Analytics™ ©2013-2019 Altair Weld Certification Director™ ©2014-2019 Altair Multi-Disciplinary Optimization Director™ ©2012-2019

Altair solidThinking - Where Innovation Begins™ Altair Inspire™ ©2009-2019 including Altair Inspire Motion and Altair Inspire Structures Altair Inspire™ Extrude-Metal ©1996-2019 (formerly Click2Extrude®-Metal) Altair Inspire™ Extrude-Polymer ©1996-2019 (formerly Click2Extrude®-Polymer) Altair Inspire™ Cast ©2011-2019 (formerly Click2Cast®) Altair Inspire™ Form ©1998-2019 (formerly Click2Form®) Altair Inspire™ Mold ©2009-2019 (initial release-Q2 2019) Altair Inspire™ Studio ©1993-2019 (formerly ‘Evolve’) Altair Compose™ ©2007-2019 (formerly solidThinking Compose®) Altair Activate™ ©1989-2019 (formerly solidThinking Activate®) Altair Embed™ ©1989-2019 (formerly solidThinking Embed®) • Altair Embed SE™ ©1989-2019 (formerly solidThinking Embed® SE) • Altair Embed/Digital Power Designer ©2012-2019 Altair SimLab™ ©2004-2019 Altair 365™ ©1994-2019

Altair PBSWorks™ - Accelerating Innovation in the Cloud™ Altair PBS Professional™ ©1994-2019 Altair Control™ ©2008-2019; (formerly PBS Control) Altair Access™ ©2008-2019; (formerly PBS Access)

Proprietary Information of Altair Engineering

Altair Accelerator™ ©1995-2019; (formerly NetworkComputer) Altair Accelerator Plus™©1995-2019; (formerly WorkloadXelerator) Altair FlowTracer™ ©1995-2019; (formerly FlowTracer) Altair Allocator™ ©1995-2019; (formerly LicenseAllocator) Altair Monitor™ ©1995-2019; (formerly LicenseMonitor) Altair Hero™ ©1995-2019; (formerly HERO) Altair Software Asset Optimization™ (SAO) ©2007-2019 Note: Compute Manager™ ©2012-2017 is now part of Altair Access Display Manager™ ©2013-2017 is now part of Altair Access PBS Application Services™ ©2008-2017 is now part of Altair Access PBS Analytics™ ©2008-2017 is now part of Altair Control PBS Desktop™ ©2008-2012 is now part of Altair Access, specifically Altair Access desktop, which also has Altair Access web and Altair Access mobile e-Compute™ ©2000-2010 was replaced by “Compute Manager” which is now Altair Access

Altair SmartWorks™ - Innovation Intelligence® Altair SmartCore™ ©2011-2019 Altair SmartEdge™ ©2010-2019 Altair SmartSight™ ©2014-2019 Altair intellectual property rights are protected under U.S. and international laws and treaties. Additionally, Altair software is protected under patent #6,859,792 and other patents pending. All other marks are the property of their respective owners. ALTAIR ENGINEERING INC. Proprietary and Confidential. Contains Trade Secret Information. Not for use or disclosure outside of Altair and its licensed clients. Information contained in Altair software shall not be decompiled, disassembled, “unlocked”, reverse translated, reverse engineered, or publicly displayed or publicly performed in any manner. Usage of the software is only as explicitly permitted in the end user software license agreement. Copyright notice does not imply publication.

Third party software licenses AcuConsole contains material licensed from Intelligent Light (www.ilight.com) and used by permission. Software Security Measures: Altair Engineering Inc. and its subsidiaries and affiliates reserve the right to embed software security mechanisms in the Software for the purpose of detecting the installation and/or use of illegal copies of the Software. The Software may collect and transmit non-proprietary data about those illegal copies. Data collected will not include any customer data created by or used in connection with the Software

Proprietary Information of Altair Engineering

and will not be provided to any third party, except as may be required by law or legal process or to enforce our rights with respect to the use of any illegal copies of the Software. By using the Software, each user consents to such detection and collection of data, as well as its transmission and use if an illegal copy of the Software is detected. No steps may be taken to avoid or detect the purpose of any such security mechanisms.

Proprietary Information of Altair Engineering

Technical Support Altair provides comprehensive software support via web FAQs, tutorials, training classes, telephone and e-mail.

Altair Support on the World Wide Web The Altair web site is a valuable online companion to Altair software. Visit www.altairhyperworks.com for tips and tricks, training course schedules, training/tutorial videos, and other useful information.

Altair Training Classes Altair training courses provide a hands-on introduction to our products, focusing on overall functionality. Courses are conducted at our main and regional offices or at your facility. If you are interested in training at your facility, please contact your account manager for more details. If you do not know who your account manager is, please send an e-mail to [email protected] and your account manager will contact you.

Telephone and E-mail When contacting Altair support, please specify the product and version number you are using along with a detailed description of the problem. Many times, it is very beneficial for the support engineer to know what type of workstation, operating system, RAM, and graphics board you have, so please have that information ready. If you send an e-mail, please specify the workstation type, operating system, RAM, and graphics board information in the e-mail. To contact an Altair support representative, reference the following table or the information available on the HyperWorks website: www.altairhyperworks.com/ClientCenterHWSupportProduct.aspx. Location

Telephone

E-mail

Australia

64.9.413.7981

[email protected]

Brazil

55.11.3884.0414

[email protected]

Canada

416.447.6463

[email protected]

China

86.400.619.6186

[email protected]

France

33.1.4133.0992

[email protected]

Germany

49.7031.6208.22

[email protected]

India

91.80.6629.4500

[email protected]

1.800.425.0234 (toll free) Israel Italy

[email protected] 39.800.905.595

[email protected]

Location

Telephone

E-mail

Japan

81.3.6225.5830

[email protected]

Malaysia

[email protected]

Mexico

55.56.58.68.08

[email protected]

South Africa

27 21 8311500

[email protected]

South Korea

82.70.4050.9200

[email protected]

Spain

34 910 810 080

[email protected]

Sweden

46.46.460.2828

[email protected]

United Kingdom

01926.468.600

[email protected]

United States

248.614.2425

[email protected]

For questions or comments about this help system, send an email to [email protected]. In addition, the following countries have resellers for Altair Engineering: Colombia, Czech Republic, Ecuador, Israel, Russia, Netherlands, Turkey, Poland, Singapore, Vietnam, Indonesia Official offices with resellers: Canada, China, France, Germany, India, Malaysia, Italy, Japan, Korea, Spain, Taiwan, United Kingdom, USA See www.altair.com for complete contact information.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.1

Contents Basics............................................................................................................................ 3 HM-1000: Getting Started with HyperMesh ...................................................................... 4 HM-1010: Opening and Saving Files ............................................................................... 8 HM-1020: Working with Panels .................................................................................... 12 HM-1030: Organizing a Model ..................................................................................... 21 HM-1040: Controlling the Display ................................................................................. 33 Geometry .................................................................................................................... 47 HM-2000: Importing and Repairing CAD ....................................................................... 48 HM-2010: Generating a Midsurface .............................................................................. 55 HM-2015: Auto-Midsurfacing with Advanced Extraction Options........................................ 58 HM-2020: Simplifying Geometry .................................................................................. 66 HM-2030: Refining Topology to Achieve a Quality Mesh ................................................... 71 HM-2040: Creating and Editing Line Data ...................................................................... 80 HM-2050: Creating Surfaces from Elements .................................................................. 98 HM-2060: Creating and Editing Solid Geometry............................................................ 107 HM-2070: Geometry and Mesh Editing Using the Quick Edit Panel................................... 121 HM-2080: Modifying Models using solidThinking Inspire ................................................ 130 HM-2090: Dimensioning ........................................................................................... 133 Meshing .................................................................................................................... 143 HM-3000: Creating 1-D Elements............................................................................... 144 HM-3100: AutoMeshing ............................................................................................ 148 HM-3110: Meshing without Surfaces .......................................................................... 161 HM-3120: 2-D Mesh in Curved Surfaces ...................................................................... 170 HM-3130: QI Mesh Creation ...................................................................................... 174 HM-3140: Batch Meshing .......................................................................................... 184 HM-3150: Meshing a Model Using Shrink Wrap ............................................................ 190 HM-3200: Tetrameshing ........................................................................................... 197 HM-3210: Creating a Hex-Penta Mesh using Surfaces ................................................... 205 HM-3220: Creating a Hexahedral Mesh using the Solid Map Function .............................. 220 HM-3270: Using the TetraMesh Process Manager ......................................................... 228 Quality ...................................................................................................................... 237 HM-3300: Checking and Editing Mesh ......................................................................... 238 HM-3320: Penetration .............................................................................................. 265 Assembly .................................................................................................................. 278 HM-3400: Creating Connectors .................................................................................. 279 HM-3410: Creating Area Connectors........................................................................... 297 HM-3420: Creating Bolt Connectors ........................................................................... 303 HM-3430: Part Replacement Through Connectors ......................................................... 308 HM-3440: Model Build and Assembly .......................................................................... 313 HM-3450: Multi-Component Replacement ................................................................... 325 Morph ....................................................................................................................... 330 HM-3510: Freehand Morphing ................................................................................... 331 HM-3520: Sculpting ................................................................................................. 337 HM-3530: Changing a Curvature Using Map to Geometry .............................................. 339 HM-3540: Changing a Profile Using Map to Sections ..................................................... 341

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.2

HM-3550: Morph Volume .......................................................................................... 343 HM-3560: Basics of Domains and Handles ................................................................... 350 HM-3570: Altering Cross-Sections Using Domains ........................................................ 356 HM-3580: Morphing About an Axis Using Domains ........................................................ 358 HM-3590: Morph Adhesive Layers .............................................................................. 360 HM-3600: Morph Tube to Different Configurations ........................................................ 364 HM-3610: Shaping a Dome Using Cyclic Symmetry ...................................................... 369 HM-3620: Shaping a Bead Using Cyclic Symmetry........................................................ 375 HM-3625: Morph a Symmetric Part onto a New Geometry ............................................. 381 HM-3630: Morphing with Shapes ............................................................................... 385 HM-3640: Interpolating Loads Using Shapes................................................................ 390 HM-3650: Creating Shapes Using Record .................................................................... 395 HM-3660: Maintaining Area Using Constraints.............................................................. 400 HM-3670: Positioning a Dummy Using Limiting Constraints............................................ 404 HM-3680: Preserving a Shape Using Cluster Constraints ............................................... 407 HM-3690: Remeshing Domains After Morphing ............................................................ 413 Analysis Setup .......................................................................................................... 417 HM-4000: Setting up Loading Conditions..................................................................... 418 HM-4010: Formatting Model for Analysis ..................................................................... 426 HM-4020: Obtaining and Assigning Beam Cross-Section Properties using HyperBeam ........ 438 HM-4030: Defining Composites .................................................................................. 448 HM-4040: Working with Loads on Geometry ................................................................ 455 HM-4060: Working with Include Files.......................................................................... 467 HM-4070: OptiView .................................................................................................. 476 Customization ........................................................................................................... 479 HM-8010: Add a Button to the User Page on the Utility Menu ......................................... 480 HM-8020: Create a Utility Menu Macro From a Command File ........................................ 483 HM-8030: Create a Utility Menu Macro to Create Constraints on a Plane .......................... 487 HM-8040: Create a Utility Menu Macro from a Tcl Script ................................................ 492 HM-8050: Create Forces on Nodes and Add a Button on the User Page ............................ 496 HM-8060: Calculate the Resultant Sum of Forces ......................................................... 501 HM-8070: Create Spline Surfaces on Tria Elements ...................................................... 506 HM-8080: Calculate the Radius of an Arc .................................................................... 512 HM-8090: Create an OptiStruct PSHELL property ......................................................... 518 Post-Processing ........................................................................................................ 522 HM-9000: Exporting Data for Fatigue Analysis ............................................................. 523 HM-9010: Free Body Diagram ................................................................................... 526

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.3

Basics

1

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

HM-1000: Getting Started with HyperMesh In this tutorial, you will explore the basic concepts of HyperMesh's user interface. It is highly recommended that you review this tutorial as it provides a general overview of HyperMesh.

Tools The HyperMesh interface contains several areas. Each is described below.

Feature

Description

Title bar

The bar across the top of the interface is the title bar. It contains the version of HyperMesh that you are running and the name of the file you are working on.

Menu bar

Located just under the title bar. Like the pull-down menus in many graphical user interface applications, these menus "drop down" a list of options when clicked. Use these options to access different areas of HyperMesh functionality.

Toolbars

Located around the graphics area, these buttons provide quick access to commonly-used functions, such as changing display options. They can be dragged and placed at the top or side of the graphics area.

Proprietary Information of Altair Engineering

p.4

Altair HyperMesh 2019 Tutorials

Tab area

p.5

The tab area is so named because various specialized tools display on tabs in this area of the interface. Two such examples are the Model Browser and the Utility Menu. •

The Model tab contains the Model Browser. This tool displays the contents of a model in a hierarchical tree format. It can be used to create and edit many types of entities, and also to organize them and control their display status.

•

The Utility Menu contains four pages of tools that perform various functions, accessed via buttons at the bottom of the menu. The Disp page tools control how a model is displayed in the graphics area. The other pages available are QA/Model (element checking tools), Geom/Mesh (tools for working with a model’s geometry as well as for creating and editing meshes), and User (custom tools you create). The content of the Utility tab changes based upon the selected user profile.

Graphics area

The graphics area is the display area for your model. You can interact with the model in three-dimensional space in real time. In addition to viewing the model, entities can be selected interactively from the graphics area.

Main menu

The main menu displays the functions available on each page. You access those functions by clicking on the button corresponding to the function you wish to use.

Main menu pages

The main menu pages menu divides the main menu into groups of related functions. Only one page of the main menu is displayed at a time. The Geom page contains functions for creating and editing geometry. The 1D, 2D, and 3D pages contain element creation and editing tools grouped according to element type. The Analysis page contains functions to set up analysis problems and define boundary conditions. The Tool page contains miscellaneous tools and model checking functions. The Post page contains post-processing functions.

Command window

You can type HyperMesh commands directly into this text box and execute them instead of using the HyperMesh graphical user interface. This window is not displayed by default, but can be opened via the View menu.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Status bar

The status bar is located at the bottom of the screen. The left end of the status bar displays your current location in the main menu. By default, Geometry is displayed. The four fields on the right side of the status bar display the current Include file, current component collector, current part, and current load collector. As you work in HyperMesh, any warning or error messages also display in the status bar. Warning messages appear in green and error messages appear in red. Hint: You can hold the left mouse button down on top of a panel to see a description for it in the status bar.

Starting HyperMesh To start HyperMesh in Windows 7, go to Start > All Programs > Altair HyperWorks > HyperMesh Desktop or HyperMesh. To start HyperMesh on UNIX, perform the following steps: 1.

Go to your operating system prompt.

2.

Enter the full path of the HyperMesh script (e.g., \altair\scripts\hm) and press ENTER. Or

3.

Type in a pre-defined alias that you or a systems administrator has created in the user .alias or .cshrc file in the user home directory.

Start Directory By default, HyperMesh uses a "start directory" for files. HyperMesh reads and writes a number of files from the start directory: •

At start up, HyperMesh reads configuration files (hm.mac, hmmenu.set, etc.).

•

Upon closing, HyperMesh writes out a command history file (command.cmf) and a menu settings file (hmmenu.set).

•

By default, HyperMesh will read from/write to this directory for any open, save, save as, import, or export functionality.

•

Image files (.jpg) created using the F6 key are saved to the start directory.

To determine the start directory on Windows, perform the following steps: 1.

Right-click the HyperMesh icon.

Proprietary Information of Altair Engineering

p.6

Altair HyperMesh 2019 Tutorials

2.

Go to Properties.

3.

On the Shortcut tab, view the path in the Start In field.

On UNIX, the start directory is determined by the following: •

Location in which you typed the command to run HyperMesh

•

Your "home" directory if configuration files are not found in the start directory

HyperMesh Help To obtain help for a particular feature, go to the Help menu and select HyperWorks Desktop or HyperWorks Help Home. The help is organized by product and contains the following types of information: •

How to use individual functions

•

Notes on interfacing HyperMesh with external data types

•

Tutorials

•

Reference guides

Model Files All files referenced in the HyperMesh tutorials are located in the hm.zip file unless otherwise note

Proprietary Information of Altair Engineering

p.7

Altair HyperMesh 2019 Tutorials

HM-1010: Opening and Saving Files In this tutorial, you will learn how to: •

Open a HyperMesh file

•

Import a file into a current HyperMesh session

•

Save the HyperMesh session as a HyperMesh model file

•

Export all of the geometry to an IGES file

•

Export all of the mesh data to an OptiStruct input file

•

Delete all of the data from the current HyperMesh session

•

Import an IGES file

•

Import an OptiStruct file to the current HyperMesh session

Model Files This exercise uses the following model files: bumper_cen_mid1.hm, bumper_mid.hm, bumper_end.igs, and bumper_end_rgd.fem. Each model file contains different sections of the bumper, that when combined make up the whole bumper model. Copy the model file(s) from the hm.zip file to your working directory.

Exercise

Step 1: Open the HyperMesh model file, bumper_cen_mid1.hm. 1.

Start HyperMesh Desktop.

2.

To open a HyperMesh model file, click File > Open > Model from the menu bar, or click

2.

on the Standard toolbar.

In the Open File dialog, open the bumper_cen_mid1.hm model file. HyperMesh loads a model containing mesh and geometry data.

Proprietary Information of Altair Engineering

p.8

Altair HyperMesh 2019 Tutorials

p.9

Step 2: Import the HyperMesh model file, bumper_mid.hm, into the current HyperMesh session. 1.

To open the Import tab, click File > Import > Model from the menu bar, or click on the Standard toolbar.

2.

In the Import tab, click

3.

In the Open dialog, open the bumper_mid.hm model file.

4.

Click Import. HyperMesh imports the bumper_mid.hm model file on top of the existing data.

.

Step 3: Import the IGES geometry file, bumper_end.iges, into the current HyperMesh session. 1.

In the Import tab, click

2.

From the File type list, select IGES.

3.

Click

4.

In the Select IGES file dialog, open the bumper_end.iges geometry file.

5.

Click Import. HyperMesh imports the IGES geometry file's data.

.

.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.10

Step 4: Import the OptiStruct input file, bumper_end_rgd.fem, into the current HyperMesh session. 1.

In the Import tab, click

2.

From the File type list, select OptiStruct.

3.

In the File field, open the bumper_end_rgd.fem input file.

4.

Click Import. HyperMesh imports a mesh for the bumper's end portion to the geometry representing the bumper’s end.

.

Step 5: Save the HyperMesh session as a HyperMesh model file called practice.hm. 1.

From the menu bar, click File > Save As > Model.

2.

In the Save Model As dialog, navigate to your working directory and save the data in your current session as a binary data file labeled practice.hm.

Step 6: Export the model’s geometry data to an IGES file called practice.iges. 1.

To access the Export tab, click File > Export > Geometry from the menu bar, or click on the Standard toolbar.

2.

From the File type list, select IGES.

3.

In the File field, navigate to your working directory and save the file as practice.igs.

4.

Click Export. HyperMesh exports all of the geometry data (points, lines, surfaces) loaded in your current session as a .iges file.

Step 7: Export the model’s mesh data to an OptiStruct input file called practice.fem. 1.

In the Export tab, click

2.

From the File type list, select OptiStruct.

.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

In the File field, navigate to your working directory and save the file as practice.fem.

4.

Click Export. HyperMesh exports all of the finite element data (nodes, elements, loads) loaded in your current session as a .fem file.

Step 8 (Optional): Delete all data from the current HyperMesh session by starting a new session. 1.

To open a new HyperMesh model, click File > New > Model from the menu bar, or click

2.

on the Standard toolbar.

In the HyperMesh dialog, click Yes if you would like to discard all current model data.

Step 9 (Optional): Import the IGES geometry file you created, practice.igs. 1.

To import the practice.igs file into your current session repeat step 3. HyperMesh imports the geometry data in the file to the existing data.

Step 10 (Optional): Import the Optistruct input file you created, practice.fem, into the current HyperMesh session. 1.

To import the practice.fem file into the current session, repeat step 4. HyperMesh imports the data in the file to the existing data.

With the completion of Steps 8, 9, and 10, your current HyperMesh session should contain all of the geometry and mesh data that existed in the HyperMesh session that you saved to a HyperMesh file in Step 5.

Step 11 (Optional): Save your work. 1.

From the menu bar, click File > Save > Model.

Proprietary Information of Altair Engineering

p.11

Altair HyperMesh 2019 Tutorials

HM-1020: Working with Panels A large portion of HyperMesh functionality is organized into panels. Many panels have common attributes and controls, so once you become familiar with the features of one panel, it is much easier to understand other panels. In this tutorial, you will learn how to: •

Use the entity selector and the extended entity selection menu to select and unselect nodes and elements from the graphics area.

•

Use the orientation selector to define vectors along which to translate nodes and elements.

•

Switch between different entities to select and methods to define vectors.

•

Toggle between two options.

•

Enter, copy and paste, and calculate numbers.

•

Use the rapid menu functionality to execute commands with the mouse buttons rather than clicking buttons.

•

Interrupt, but not exit, a panel to go to another panel using the keyboard function keys.

Model Files This exercise uses the bumper.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Open and view the model file, bumper.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, navigate to your working directory and open the bumper.hm model file. A model appears in the graphics area.

Step 2: In the Translate panel, select nodes from the graphics area. 1.

To open the Translate panel, click Mesh > Translate > Nodes from the menu bar.

2.

Click the entity selector to active it. Note:

The cyan border around the entity selector indicates that it is active.

Proprietary Information of Altair Engineering

p.12

Altair HyperMesh 2019 Tutorials

p.13

on the Visualization toolbar to change the element

3.

Optional: If necessary, click view style to wireframe.

4.

In the graphics area, left-click on the corners of the elements to select a few nodes. HyperMesh positions a small, white node at each element corner you select.

5.

To reset the selection of nodes, click

on the entity selector.

Step 3: Select and unselect elements from the graphics area. 1.

Click on the entity selector, and select elems from the list of entities that can be translated. The entity selector is now set to elems.

2.

In the graphics area, left-click on the element handles (the dot at the element's center) to select several elements. HyperMesh highlights the elements you select in white.

3.

To unselect an element, right-click on the element handle in the graphics area.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.14

Step 4: Select and unselect elements using the quick window selection method. 1.

Verify that the entity selector is active and set to elems.

2.

In the graphics area, press SHIFT, left-click, and draw a rectangular window around a few elements. HyperMesh selects all of the element handles inside of the rectangular window you drew.

3.

To unselect the elements, press SHIFT, right-click, and draw a rectangular window around the selected elements.

4.

In the graphics area, press SHIFT and left-click. The Quick window pop-up menu appears, containing eight icons.

5.

Still pressing SHIFT, click elements.

, and draw a polygon window around a few unselected

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

p.15

Release the SHIFT key and mouse button. HyperMesh selects all of the element handles inside of the polygon window.

Step 5: Select and unselect elements by using the extended entity selection menu. 1.

Click elems >> reverse. HyperMesh unselects the elements that you selected, and selects the elements that were not selected.

2.

Click elems >> by adjacent. HyperMesh selects the elements that are adjacent to the selected elements.

Step 6: Shade the elements, reset the selection, and select a few adjacent elements. 1.

On the Visualization toolbar, click mode, rather than wireframe mode.

2.

To clear the selection of elems, click

Proprietary Information of Altair Engineering

. HyperMesh displays the elements in shaded

on the entity selector.

Altair HyperMesh 2019 Tutorials

3.

p.16

Using the entity selector, select a few elements that are adjacent to each other in the graphics area.

Step 7: Specify a direction vector (N1 and N2 only) along which to translate the selected elements. 1.

On the orientation selector, click and select N1, N2, N3 from the list of vector and plane options, which define the direction in which to translate the selected elements.

2.

To activate the N1 selector, click Note:

3.

.

The cyan border around the N1 selector indicates that it is active. Since the entity selector is no longer active, HyperMesh changes the color of the selected elements in the graphics area to gray.

In the graphics area, select any node for N1. HyperMesh highlights the selected node in green, and the active selector advances to N2 in the Translate panel.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

In the graphics area, select a node near N1 for N2. HyperMesh highlights the selected node in blue, and the active selector advances to N3 in the Translate panel. Note:

For this tutorial, you do not need to select a node for N3. Selecting N1 and N2 defines a vector for the direction of translation. This vector goes from N1 towards N2. Selecting N3 defines a plane. The direction of translation is the positive direction of the vector normal to the plane. The positive direction is determined by the right-hand rule.

Step 8: Specify a distance to translate the selected elements and then translate them. 1.

Click the second toggle and select magnitude = N2-N1.

2.

Click translate+. HyperMesh translates the selected elements in the N1 to N2 direction by N2-N1 units in the graphics area. Note:

HyperMesh places a thick black border around translate+, which indicates that it is a rapid menu button.

Proprietary Information of Altair Engineering

p.17

Altair HyperMesh 2019 Tutorials

3.

Instead of clicking translate+, middle-mouse click. HyperMesh translates the selected elements again by N2-N1 units.

4.

Click translate- twice. HyperMesh translates the selected elements in the negative N1N2 vector direction, and restores them to their initial position.

Step 9: Measure the distance between two nodes. 1.

To interrupt, but not exit the Translate panel and go to the Distance panel on the Geom page, press F4. Note:

The graphics area is currently not displaying the elements and nodes that you selected in the Translate panel, however, they are still selected. When you return to the Translate panel, they will reappear.

2.

In the Distance panel, click two nodes. The N1 selector is active.

3.

In the graphics area, select any node for N1. HyperMesh highlights the selected node in green, and the active selector advances to N2.

4.

In the graphics area, select a node near N1 for N2. The distance between N1 and N2 appears in the distance = field.

Proprietary Information of Altair Engineering

p.18

Altair HyperMesh 2019 Tutorials

5.

In the distance = field, highlight the value.

6.

To copy the value, press CTRL + C.

7.

To return to the Translate panel, click return. The graphics area displays the elements and nodes you selected earlier in the Translate panel.

Step 10: Specify a distance to translate the selected elements and then translate them. 1.

Click the second toggle and select magnitude =.

2.

In the magnitude = field, highlight the value.

3.

To paste the distance= value that you copied from the Distance panel, press CTRL + V.

4.

Click translate+. HyperMesh translates the selected elements in the direction from N1 to N2 by the number of units specified in the magnitude = field.

5.

Click translate- once. HyperMesh translates the selected elements in the negative N1N2 vector direction, and restores them to their initial position.

Step 11: Calculate 5.5 * 10.5 and specify the resulting value for magnitude =. 1.

In the magnitude= field, right-click. The HyperMesh calculator appears.

Proprietary Information of Altair Engineering

p.19

Altair HyperMesh 2019 Tutorials

p.20

2.

Click 5 . 5 (in that order).

3.

Click enter.

4.

Click 10 . 5 (in that order).

5.

Click X. The calculator displays a calculated value of 57.75.

6.

Click exit. The calculator closes and 57.75 appears in the magnitude = field.

7.

Optional: To enter a value in the magnitude = field, left-click in the field to highlight the current value, then enter a new value.

Step 12: Specify a new vector and translate the elements again. 1.

To reset the direction of the translated elements, click N1 becomes the active selector.

on the direction selector.

2.

In the graphics area, select three nodes for N1, N2, N3 to define a plane.

3.

Click translate+ or middle-mouse click. HyperMesh translates the elements 57.75 units in the positive direction normal to the defined plane.

4.

To exit the panel, click return.

Step 13 (Optional): Save your work. 1.

When you have completed all of the exercises in this tutorial, click File > Save > Model from the menu bar.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

HM-1030: Organizing a Model A large portion of HyperMesh functionality is organized into panels. Many panels have common attributes and controls, so once you become familiar with the features of one panel, it is much easier to understand other panels. In this tutorial, you will learn how to: •

Create geometry and organize it into components

•

Organize elements into the components

•

Rename components

•

Identify and delete empty components

•

Delete all of the geometry lines

•

Reorder the components in a specific order

•

Renumber all of the components, starting with ID 1 and incrementing by 1

•

Create an assembly

•

Organize the constraint

Model Files This exercise uses the bumper.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise It is recommend that you review the general overview before completing this tutorial.

Step 1: Retrieve the model file, bumper.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, navigate to your working directory and open the bumper.hm model file. A model appears in the graphics area.

Proprietary Information of Altair Engineering

p.21

Altair HyperMesh 2019 Tutorials

Step 2: Create a component named geometry to hold the model’s geometry. 1.

To create a new component, click Collectors > Create > Components from the menu bar, or right-click in the Model browser and select Create > Components from the context menu.

2.

In the Create component dialog, enter geometry in the Name field.

3.

Click the Color icon, and select yellow.

4.

Click Create. The Model browser displays the current component collector geometry in bold.

Step 3: Create two geometry lines and organize them into different components. 1.

To open the Lines panel, click Geometry > Create > Lines > Standard Nodes from the menu bar.

2.

Activate the node list selector.

3.

In the graphics area, select two opposite and diagonal nodes of the same element as illustrated in the image below:

Proprietary Information of Altair Engineering

p.22

Altair HyperMesh 2019 Tutorials

4.

Click create. HyperMesh creates a yellow line. Note:

This line is the same color as the geometry component, because it is organized into the current component, geometry.

5.

In the Model browser, Component folder, right-click on rigid and select Make Current from the context menu. HyperMesh makes the rigid component the active component.

6.

In the graphics area, select two opposite and diagonal nodes of the same element, but different than the element selected above.

Proprietary Information of Altair Engineering

p.23

Altair HyperMesh 2019 Tutorials

7.

Click create. HyperMesh creates a red line. Note:

8.

This line is the same color the rigid component, because it is organized into the current component, rigid.

To exit the panel, click return.

Step 4: Move all of the model’s geometry surfaces into the component, geometry. 1.

To open the Organize panel, click Geometry > Organize > Surfaces from the menu bar.

2.

To go to the Collectors subpanel, click collectors.

3.

Click on the entity selector, and select surfs from the list of entities that can be collected. The entity selector is now set to surfs.

4.

Click surfs >> all. HyperMesh highlights all of the displayed surfaces in white, which indicates they are selected. Note:

If there are surfaces that are not displayed, HyperMesh still selects them because you selected surfs >> all.

Proprietary Information of Altair Engineering

p.24

Altair HyperMesh 2019 Tutorials

5.

Click dest component=.

6.

From the list of components, select geometry.

7.

Click move. Hypermesh moves the selected surfaces into the geometry component, and colors the geometric entities yellow to match the component color.

Step 5: Move all the model’s shell elements (quads and trias) into the component, center. In this step, you should still be in the Organize panel, collectors subpanel. 1.

Click on the entity selector, and select elems from the list of entities that can be collected. The entity selector is now set to elems.

2.

Click elems >> by collector.

3.

Select the components: mid1, mid2, and end.

4.

Optional: To select a component in the graphics area, left-click on it. A check mark appears in the check box of the component you selected in the panel area.

5.

Optional: To unselect a component, right-click its check box in the panel area, or rightclick on it in the graphics area.

Proprietary Information of Altair Engineering

p.25

Altair HyperMesh 2019 Tutorials

6.

To complete your component selection, click select.

7.

Click dest component =.

8.

Select the component center.

9.

Click move. HyperMesh moves the elements in the selected components into the center component, and colors all of the shell elements cyan blue to match the component color.

10. To exit the panel, click return.

Step 6: Rename the component center to shells. 1.

In the Model browser, Component folder, right-click on center and select Rename from the context menu.

2.

In the editable field, rename the component shells and then press ENTER.

Proprietary Information of Altair Engineering

p.26

Altair HyperMesh 2019 Tutorials

Step 7: Identify and delete all of the empty components. 1.

To open the Delete panel, press F2.

2.

Set the entity selector to comps.

3.

Click preview empty. The Status bar displays a message that says, "3 entities are empty." Note:

4.

The empty entities are the mid1, mid2, and end components that no longer have elements in them.

Click comps. HyperMesh displays a complete list of the model’s components. Note:

The empty components are indicated with a selected check box.

5.

To return to the Delete panel, click return.

6.

Click delete entity. The Status bar displays a message that says, "Deleted 3 comps 336 elems 28 surfs"

Step 8: Delete all the geometry lines in the model. In this step, you should still be in the Delete panel. 1.

Set the entity selector to lines.

2.

Click lines >> all.

3.

Click delete entity. HyperMesh deletes the two lines you created earlier.

4.

To exit the Delete panel, click return.

Step 9: Move the component, geometry, to the front in the components list. 1.

To open the Reorder panel, click Collectors > Reorder > Components from the menu bar.

2.

Click comps. HyperMesh displays a complete list of the model’s components.

3.

On the right side of the panel, click the bottom switch and select name(id). HyperMesh displays the IDs for each component next to its name. The ID for shells is 1, the ID for rigid is 5, and the ID for geometry is 6.

Proprietary Information of Altair Engineering

p.27

Altair HyperMesh 2019 Tutorials

4.

Select the component, geometry.

5.

To complete your selection, click select.

6.

Under move to, select front.

7.

Click reorder. HyperMesh applies the reorder function to the component, geometry.

8.

To review the reordered list of components, click comps. Note:

9.

The component, geometry, is at the top of the list. However, it still has the same ID, (6).

To exit the panel, click return.

Step 10: Renumber the components to be the same as their position in the list. 1.

To open the Renumber panel, click Collectors > Renumber > Components from the menu bar.

2.

Go to the single subpanel.

3.

Set the entity selector to comps.

4.

Click comps. HyperMesh displays a complete list of the model’s components.

5.

On the right side of the panel, click comps >> all.

6.

To complete your selection, click select.

7.

In the start with = field, enter 1.

8.

In the increment by = field, enter 1.

9.

In the offset = field, enter 0.

10. Click renumber. HyperMesh renumbers the components. 11. To review the renumbered list of components, click comps. Note:

The components are numbered according to their position in the list. Set the view to name(id) to see the numbers.

Proprietary Information of Altair Engineering

p.28

Altair HyperMesh 2019 Tutorials

12. To exit the panel, click return. Note:

Having components with IDs that do not reflect their position in the model’s list of components will not result in errors. However, having components with IDs that do reflect their position in the model’s list of components can be helpful for organizational purposes.

Step 11: Create an assembly containing the components, shells and rigid. 1.

In the Model browser, right-click and select Create > Assembly from the context menu.

2.

In the Create Assembly dialog, enter elements in the Name field.

3.

Select a Color for the assembly.

4.

Click Create. HyperMesh creates the assembly.

5.

In the Model browser, Component folder, select rigid and shells. Tip:

6.

To select multiple components, press Ctrl + left-click.

To add the selected components to the elements assembly, drag the components, using the left mouse button, over the elements assembly until it highlights.

Proprietary Information of Altair Engineering

p.29

Altair HyperMesh 2019 Tutorials

Step 12: Create a load collector named constraints. 1.

To create a load collector, click Collectors > Create > Load Collectors from the menu bar, or right-click in the Model browser and select Create > Load Collector from the context menu.

2.

In the Create Load Collector dialog, enter constraints in the Name field.

3.

Click the Color icon, and select red.

4.

Click Create. HyperMesh creates the load collector, and the Status bar displays a message that says, "Load collector created". Note:

The constraints load collector is displayed in bold in the Model browser, which indicates that it is the active load collector. Any loads that are created will be organized into this load collector.

Step 13: Move the model’s one constraint into the load collector, constraints. The existing load collector, loads, contains several forces and one constraint. In this step, you will use the Organize panel is to move the one constraint in the load collector, constraints. 1.

To open the Organize panel, click Collectors > Organize > Load Collectors from the menu bar.

2.

Go to the collectors subpanel.

3.

Set the entity selector to loads.

4.

Select loads >> by config.

5.

Click config =, and select const.

6.

In the center of the panel, toggle from displayed to all.

7.

Click select entities.

Proprietary Information of Altair Engineering

p.30

Altair HyperMesh 2019 Tutorials

8.

Verify that dest component= is set to the load collector, constraints.

9.

Click move. HyperMesh moves the selected constraints into the load collector, constraints.

Step 14: Create a component from the Model Browser. 1.

In the Model browser, right-click and select Create > Component from the context menu.

2.

In the Create Component dialog, enter component1 in the Name field.

3.

Click the Color icon, and select pink.

4.

Click Create. HyperMesh creates the component, and appends it to the list.

5.

In the Model browser, expand the Components folder to see that component1 is boldfaced in the list, which indicates that it is the current component.

Step 15: Review the existing assembly elements from the Model Browser. 1.

In the Model browser, expand the Assembly Hierarchy folder and then expand the elements assembly folder. It contains two components, rigid and shells. Note:

Use can use the Assemblies panel to add components from one assembly to another assembly. The Model browser does not allow you to do this, but you can create assemblies from it.

Proprietary Information of Altair Engineering

p.31

Altair HyperMesh 2019 Tutorials

Step 16: Add the components, geometry and component1, to the assembly, assem_mid, using the Model browser. 1.

In the Model browser, select the geometry and component1 components. Tip:

2.

To select multiple items in the Model browser one at a time, press and hold Ctrl and then left-click the items. If you wish to select multiple items in the Model browser at once, left-click the first item, press and hold SHIFT, and then left-click the last item in the list.

To add the selected components to the assem_mid assembly, drag the components, using the left mouse button, over the assem_mid assembly until it highlights.

Step 17: Rename assem_mid to assem_geom in the Model browser. 1.

In the Model browser, Assembly folder, right-click on assem_mid and select Rename from the context menu.

2.

In the editable field, rename the assembly assem_geom and then press Enter.

Step 18: Delete component1 from the Model Browser. 1.

In the Model browser, right-click on component1 and select Delete from the context menu.

2.

In the HyperMesh dialog, click Yes to confirm that you wish to delete the component. HyperMesh deletes component1. Note: In the Model browser, there is no longer a boldfaced component name. This indicates that there is no current component specified.

Step 19: Set the current component from the Model Browser. 1.

In the Model browser, Component folder, right-click on shells and select Make Current from the context menu. Note:

The shells component name is boldfaced.

Proprietary Information of Altair Engineering

p.32

Altair HyperMesh 2019 Tutorials

HM-1040: Controlling the Display When performing finite element modeling and analysis setup, it is important to be able to view the model from different vantage points and control the visibility of entities. You may need to rotate the model to understand the shape, zoom in to view details more closely, or hide specific parts of the model so other parts can be seen. Sometimes a shaded view is best, while other times, a wireframe view allows you work on details inside the model. HyperMesh has many functions to help you control the view, visibility, and display of entities. In this tutorial, you will learn how to: •

Control the points of view using the mouse and toolbar.

•

Control the visibility of entities using the Display panel, Mask panel, and tools on the Utility menu.

•

Control how entities look by using the toolbar and the Model browser.

•

Rename components.

•

Identify and delete empty components.

•

Delete all of the geometry lines.

Model Files This exercise uses the bumper.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Retrieve the HyperMesh model file, bumper.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, navigate to your working directory and open the bumper.hm model file. A model appears in the graphics area.

Step 2: Manipulate the model view using the mouse controls. In this step, you will learn how to use CTRL + mouse keys to rotate the model, change the center of rotation, zoom, fit, and pan. 1.

Move your mouse pointer into the graphics area.

2.

Press CTRL + Left Mouse Button (LMB) and move the mouse around. The model rotates with the movement of the mouse, and a small white square appears in the middle of the graphics area, indicating the center of the rotation.

Proprietary Information of Altair Engineering

p.33

Altair HyperMesh 2019 Tutorials

p.34

3.

Release the LMB and press it again to rotate the model in a different direction.

4.

Press CTRL and quick-click the LMB anywhere on the model. The center of rotation square appears near where you clicked, and HyperMesh searches for one of the conditions listed below, in the listed order, and relocates the center of rotation at or near the first condition identified. •

A nearby node or surface vertex

•

A nearby surface edge to project onto

•

A nearby geometry surface or shaded element

Note:

If none of the conditions are met, the center of rotation is relocated to the center of the screen.

5.

To rotate the model and view the change in rotation behavior, press CTRL + LMB.

6.

Press CTRL and quick-click the LMB anywhere in the graphics area, except for on the model. HyperMesh relocates the center of rotation square to the center of the screen.

7.

To rotate the model and observe the change in rotation behavior, press CTRL + LMB.

8.

Press CTRL + Middle Mouse Button (MMB) and move the mouse around. HyperMesh draws a white line along the path of the mouse movement.

9.

Release the mouse button. HyperMesh zooms in on the portion of the model where the line was drawn. Note:

You can also simply draw a line to zoom in on a portion of the model.

10. Press CTRL + quick-click the MMB. Hypermesh fits the model to the graphics area. 11. Press CTRL and spin the Mouse Wheel. Hypermesh zooms in or out on the model, depending on which direction you spin the mouse wheel. 12. Move the mouse pointer to a different location in the graphics area and repeat step 2.11. HyperMesh zooms zooms in or out on the model from where the mouse handle is located. 13. To fit the model to the graphics area, press CTRL + quick-click the MMB. 14. Press CTRL + Right Mouse Button (RMB) and move the mouse around. Hypermesh pans (translates) the model according to the mouse movement.

Step 3: Manipulate the view of the model using the rotate functions on the toolbar. 1.

On the View Controls toolbar, left-click

2.

Move the mouse pointer into the graphics area. The center of rotation square appears.

3.

Press and hold the LMB, and then move the mouse around. The model rotates with the movement of the mouse, similar to the way the model rotates when you press CTRL + LMB and move the mouse.

4.

Click the MMB on the model. The center of rotation square appears near where you clicked.

5.

To exit the rotation mode, move the mouse pointer out of the graphics area or rightclick.

Proprietary Information of Altair Engineering

(Dynamic Rotate).

Altair HyperMesh 2019 Tutorials

p.35

6.

On the View Controls toolbar, right-click (Dynamic Rotate) and move the mouse pointer into the graphics area. The center of rotation square appears.

7.

To change the center of rotation, click the MMB on the model.

8.

Click the LMB near the center of rotation square. The model rotates continuously in the direction of your mouse pointer, relative to the center of rotation.

9.

With the LMB still pressed, move the mouse around slowly. The direction and speed of the rotating model changes. Note:

The farther the mouse pointer is from the center of rotation, the quicker the model rotates.

10. To rotate the model in a different direction, release the LMB, and then click it again. 11. Click the MMB anywhere in the graphics area, except on the model. The center of rotation square is relocates to the screen’s center. 12. To exit the rotation mode, move the mouse pointer out of the graphics area or leftclick.

Step 4: Manipulate the view of the model by using the zoom in and out functions on the toolbar. 1.

On the View Controls toolbar, left-click (Circle / Dynamic Zoom). The Status bar displays the message, "Circle the data to be zoomed in on."

2.

Move the mouse pointer into the graphics area.

3.

Press the LMB and move the mouse around in the graphics area. HyperMesh draws a white line along the path of the mouse movement.

4.

Release the LMB. HyperMesh zooms in on the portion of the model where the line was drawn. Note:

You can also simply draw a linear line to zoom in on a portion of the model. This function is similar to pressing CTRL + MMB to zoom into a portion of the model.

5.

On the Standard Views toolbar, click graphics area.

6.

On the View Controls toolbar, left-click (Zoom In / Out). HyperMesh zooms in on the model by the factor specified in the Options panel.

7.

On the View Controls toolbar, right-click on the model by the same factor.

8.

To open the Options panel, click Preferences > Meshing Options or Geometry Options from the menu bar.

9.

Go to the geometry or mesh subpanel.

10. In the zoom factor = field, enter 4. 11. To exit the panel, click return.

Proprietary Information of Altair Engineering

(Fit). HyperMesh fits the model to the

(Zoom In / Out). HyperMesh zooms out

Altair HyperMesh 2019 Tutorials

p.36

12. On the View Controls toolbar, left-click the model by the larger, specified factor.

(Zoom In / Out). HyperMesh zooms in on

13. On the View Controls toolbar, right-click (Zoom In / Out). The Status bar displays the message "Drag up/down to zoom in/out." 14. Move the mouse pointer into the graphics area, press the LMB, and then move the mouse pointer up and down. HyperMesh zooms in and out on the model according to how far you move the mouse up or down. 15. To exit the dynamic zoom mode, move the mouse pointer out of the graphics area or left-click.

Step 5: Manipulate the model view using the arrows and view panel on the toolbar. 1.

On the View Controls toolbar, right-click or left-click any of the Rotate icons (

,

, ). The model rotates in the direction of the arrow by the rotation angle specified in the Options panel. 2.

On the Standard Views toolbar, click

3.

To open the Options panel, click Preferences > Meshing Options or Geometry Options from the menu bar.

4.

In the rotate angle = field, enter 90.

5.

To return to the main menu, click return.

6.

On the View Controls toolbar, click any of the Rotate icons ( rotates by the new specified rotation angle, 90.

7.

Change the view of the model to any view.

8.

To rotate the model, press CTRL + LMB, or click any of the Rotate icons on the View Controls toolbar.

9.

To zoom in or out on the model, press CTRL + MMB, or click any of the Zoom icons on the View Controls toolbar.

(XY Top Plane View).

,

,

). The model

10. From the Model browser, right-click anywhere and select Create > View from the context menu. 11. To see the new view name, expand the View folder. 12. Right-click on the view and select Rename from the context menu. 13. In the editable field, enter my_view for the new name. 14. To display a different view of the model, click

(XY Plane Top View).

15. To display the view, click my_view in the Model browser.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 6: Control the display of components using the toolbar. 1.

On the Visualization toolbar, click (Shaded Elements and Mesh Lines). HyperMesh shades the model's shell elements.

2.

Left-click next to (Shaded Elements and Mesh Lines), and select (Shaded Elements and Feature Lines). HyperMesh shades the model's elements and displays the features lines, mesh lines are no longer displayed.

3.

Left-click next to (Shaded Elements and Feature Lines), and select (Shaded Elements). HyperMesh hides the model's feature lines.

Proprietary Information of Altair Engineering

p.37

Altair HyperMesh 2019 Tutorials

4.

p.38

To return to the wireframe shading mode, click on the Visualization toolbar.

(Wireframe Elements Skin Only)

Step 7: Control the display of components using the Model browser. 1.

On the Visualization toolbar, click with no mesh lines.

2.

In the Model browser, right-click and select Columns > Show FE Style from the context menu. A new column appears in the Model browser.

Proprietary Information of Altair Engineering

. HyperMesh shades all of the model's elements,

Altair HyperMesh 2019 Tutorials

p.39

3.

For the mid1 component, left-click

4.

From the pop-up menu of displays modes, select (Wireframe Elements Skin Only). HyperMesh changes only the mid1 components display mode to wireframe.

5.

Experiment with the other display modes. Ico n

in the FE Style column.

Display Mode

Wireframe Elements – Element edges are displayed with lines. Wireframe Elements Skin Only – Element edges are displayed with lines for shell elements only. Shaded Elements – The element is displayed as a filled polygon. Shaded Elements with Mesh Lines – The element is displayed as a filled polygon with the feature edges drawn in mesh line color. Hidden Line with Feature Lines – The element is displayed as a filled polygon with the feature edges in mesh line color.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.40

Transparent – The element is displayed as a filled transparent polygon.

Step 8: Control the visibility of various entity categories using the Model browser. 1.

In the Model browser, right-click and select Expand All from the context menu. All of the folders in the browser expand.

2.

At the top of the browser, click all the entities in the model.

3.

Click

(Display none). HyperMesh turns off the display of

(Display all). HyperMesh displays all of the entities in the model.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.41

4.

Left-click Component (5) to select all of the components in the model.

5.

Click (Display none). HyperMesh turns off the display of all the component collectors. Note:

Display all, Display none, and Display reverse act globally (on all entities) if you have not selected any of the entities in the Model browser. If a folder is selected (highlighted), HyperMesh will perform the action only on the entities within that folder. If an individual entity is selected, HyperMesh will perform the action only on that entity.

6.

Left-click in the white space of the browser. HyperMesh deselects all of the entities in the browser.

7.

Click (Display reverse). HyperMesh reverses the display and only shows the components, instead of everything but the components.

8.

Click (Component View). HyperMesh displays only the component collectors in the browser.

9.

At the top of the browser, click select Note:

10. Click

next to

(Elements). Display all, Display none, and Display reverse will no longer affect the display of the geometry in the components. (Display none). HyperMesh only displays the components geometry.

11. Set the elements and geometry filter to 12. Click

(Elements and Geometry Filter), and

(Elements and Geometry).

(Display reverse). HyperMesh only displays the component's elements.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.42

Step 9: Control the visibility of individual components using the Model browser. A component collector has two ‘compartments’: one for elements and the other for geometry. From the Model browser, you can control the element and geometry display of individual components using these compartments. 1.

Next to the mid2, end, and rigid components, click (elements). HyperMesh displays the elements in the center and mid1 components.

2.

On your keyboard, press F. HyperMesh fits the displayed components to the graphics area.

3.

Next to the components mid2 and end, click geometry in the mid2 and end components.

4.

Press F. HyperMesh fits the displayed components to the graphics area.

(geometry). HyperMesh displays the

Step 10: Control the display of entities using the Mask panel. 1.

To open the Mask panel, click

2.

Go to the mask subpanel.

3.

Set the entity selector to elems.

4.

Click elems >> by collector.

5.

Select the component, mid1.

6.

To complete your selection of components, click select.

Proprietary Information of Altair Engineering

(Mask) on the Display toolbar.

Altair HyperMesh 2019 Tutorials

p.43

7.

From the graphics area, manually select a few elements in the center (blue) component.

8.

To mask the elements, click mask. The elements in the mid1 component and the elements you selected from the graphics area are no longer displayed. Note:

9.

In the Model browser, notice that the elements ( ) for the components center and mid1 are still displayed. Their display icons indicate that they are activated even though some or all of the elements in these components are masked (hidden).

In the Mask panel, click unmask all, or on the Display toolbar click (unmask all). HyperMesh displays all of the elements in the components, center and mid1, again. Note:

The elements in the other components are not displayed. This is because these components are not active in the Display panel.

10. To return to the main menu, click return.

Step 11: Control the display of entities using the Find panel. 1.

To open the Find panel, click

(Find) on the Display toolbar.

2.

Go to the find entities subpanel.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

Click elems >> by collector.

4.

Select the component, end.

5.

Click select.

6.

To find the elements, click find. HyperMesh displays the elements in the component, end.

In the Model browser, notice that the elements for the component, end, are now shown as active ( ). This is because the collector containing the entities that are to be displayed (found) must be active.

7.

Go to the find attached subpanel.

8.

Click attached to: elems >> displayed.

9.

To find the elements, click find. HyperMesh displays some of the elements in the components, mid2 and rigid. These elements are immediately adjacent and connected to the selected elements. Note:

The elements for these components are now shown as active ( ). The components were made active so that the elements could be displayed.

Proprietary Information of Altair Engineering

p.44

Altair HyperMesh 2019 Tutorials

p.45

10. To return to the main menu, click return. 11. On the Display toolbar, click elements. Note:

(Unmask All). HyperMesh displays all of the model's

This is because the Find panel finds the entities it is supposed to find, activates (displays) the corresponding collectors, and then masks the other entities in the collectors it activated. In this case, the last find command displayed on the components, mid2 and rigid, in the Model browser.

Step 12: Change the display of entities using the Mask tab. 1.

In the Model browser, click on any of the white space to make sure nothing is selected.

2.

Click

(Display none).

3.

Click

(Display all).

Note:

Performing these two steps makes sure that everything is displayed in the model.

4.

Click the Mask tab.

5.

In the Isolate column of Components, click . HyperMesh displays only the components in the model (elements, geometry, and connectors), and masks everything else.

6.

Expand the Components branch to expose the connectors, elements, and geometry.

7.

In the Hide column of Elements, click model, and only displays the surfaces.

8.

Expand the LoadCollectors branch to expose loads and equations.

9.

Expand the Loads branch to expose constraints, forces, moments, and so on.

. HyperMesh masks the elements in the

10. In the Show column of Constraints, click display of the surfaces.

. HyperMesh adds constraints to the

11. Expand the Elements branch to expose 0D/rigids, springs/gaps, 1D, 2D, and 3D. 12. In the Isolate column of 0D/Rigids, click . HyperMesh adds rigid elements to the display, and masks the surfaces. The constraints remain displayed. Note:

When you use Isolate below the top level of the list, HyperMesh will not mask anything outside of the top level that the entity being isolated belongs to. Rigids belong to components at the top level, therefore Hypermesh will not mask any entities in the other top levels.

13. In the Isolate column of Components, click . HyperMesh displays all of the entities in the components, and masks the constraints. Note:

When you use Isolate at the top level of the list (components, groups, loadcollectors, morphing, multibodies, and systemcollectors), HyperMesh will mask everything outside of the entity type being isolated.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 13: Change the color of components using the Model browser. 1.

In the Model browser, Component folder, click the Color icon next to mid1.

2.

From the color pop-up, select a different color.

3.

Observe the change in color of the elements in mid1.

Proprietary Information of Altair Engineering

p.46

Altair HyperMesh 2019 Tutorials

Geometry

Proprietary Information of Altair Engineering

p.47

2

Altair HyperMesh 2019 Tutorials

HM-2000: Importing and Repairing CAD In this tutorial, you will: •

Delete untrimmed surfaces

•

Close missing surfaces

•

Set the cleanup tolerance

•

Equivalence free edges

•

Delete duplicate surfaces

The benefits of importing and repairing CAD are: •

Correcting any errors in the geometry from import

•

Creating the simplified part needed for the analysis

•

Meshing a part all at once

•

Ensuring proper connectivity of mesh

•

Obtaining a desirable mesh pattern and quality

Model Files This exercise uses the clip_repair.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Importing and Repairing CAD Geometry Data

Proprietary Information of Altair Engineering

p.48

Altair HyperMesh 2019 Tutorials

p.49

Step 1: Open and view the model file, clip_repair.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the clip_repair.hm model file.

Step 2: View the model in topology display toolbar and shaded mode to evaluate its integrity. 1.

Observe where the model has incorrect connectivity and missing or duplicate surfaces.

2.

To open the Auto Geometry Cleanup panel, click Geometry > Autocleanup from the menu bar. The surface edges are now colored according to their topology status. Note:

3.

To display the model's geometry in wire frame mode, click toolbar. Note:

4.

This occurs because Geometry Color is set to

. on the Visualization

The Visualization toolbar contains icons that control the display of the surfaces and surface edges. Surfaces can be shaded with or without edges or wireframe. Right-click the icons to access the drop-down menu for additional options. Place your mouse over the cursor to view a description of the button’s functionality.

To open the Visualization browser and access the Topology options, click Note:

.

The Topology options control the display of the surfaces and surface edges. Surfaces can be shaded or wireframe. The check boxes within the Visualization browser turn the display of the different edge types and fixed points (surface vertices) on or off.

5.

Select only the Free check box. The graphics area displays only the free edges.

6.

Observe the free (red) edges and make note of where they are. Free edges show where there is incorrect connectivity or gaps.

7.

Observe the locations where there are closed loops of free edges. These are locations that probably have missing surfaces.

Free edges indicating surface discontinuities of the clip geometry

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.50

8.

Select only the Non-manifold check box.

9.

Observe the non-manifold edges and make note of where they are. Non-manifold edges show where there are more than two surfaces sharing an edge, which might indicate incorrect connectivity. For this part, there are yellow edges completely surrounding two areas. This indicates that there are probably duplicate surfaces in these locations.

10. Select all of the check boxes. 11. Close the Visualization browser. 12. To exit the panel, click return. 13. To shade the model's geometry and surface edges, click toolbar.

on the Visualization

14. To locate any errors in the geometry, rotate, zoom, and pan. 15. Note the areas to be worked on: •

A surface that overhangs a round corner

•

A missing surface

Surface overhanging an edge and a missing surface

Step 3: Delete the surface that overhangs the round corner. 1.

To open the Delete panel, click Geometry > Delete > Surfaces from the menu bar, or press F2.

2.

Optional: If you opened the Delete panel by pressing F2, set the entity selector to surfs.

3.

Select the overhanging surface shown in the previous image.

4.

Click delete entity. HyperMesh deletes the selected entities.

5.

To exit the panel, click return.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 4: Create surfaces to fill large gaps in the model. 1.

To open the panel from which you can create a surface, click Geometry > Create > Surfaces > Spline/Filler from the menu bar.

2.

Clear the Keep tangency check box.

3.

Set the entity selector to lines.

4.

Verify the Auto create (free edges only) check box is selected. The Auto create option simplifies the selection of the lines bounding the missing surface. Once a line is selected, HyperMesh selects the remaining free edges that form a closed loop, and then creates the filler surface.

5.

Zoom into the area indicated in the following image.

Area of missing surfaces

6.

Select one of the red lines bounding one of the gaps (missing surfaces) shown in the previous image. HyperMesh creates a filler surface to close the hole.

7.

Repeat step 4.6 to create a filler surface in the other gap.

8.

To exit the panel, click return.

Step 5: Set the global geometry cleanup tolerance to .01. 1.

Press O. The Options panel opens.

2.

Go to the geometry subpanel.

3.

In the cleanup tol = field, type 0.01 to stitch the surfaces with a gap less than 0.01

4.

To exit the panel, click return.

Proprietary Information of Altair Engineering

p.51

Altair HyperMesh 2019 Tutorials

Step 6: Combine multiple free edge pairs at one time with the equivalence tool. 1.

From the menu bar, click Geometry > Edit > Surface Edges > Equivalence.

2.

Select the equiv free edges only check box.

3.

Select surfs >> all.

4.

Verify that the cleanup tol= is set to 0.01. This is the global cleanup tolerance that you specified in the Options panel.

5.

Click equivalence. HyperMesh combines any free edge pairs within the specified cleanup tolerance. Most of the red free edges are combined into green shared edges. The few remaining are caused by gaps larger than the cleanup tolerance.

Step 7: Combine free edge pairs, one pair at a time, using the toggle. 1.

Go to the toggle subpanel.

2.

In the cleanup tol = field, type 0.1.

3.

Click one of the free edges shown in the following image. When you select the edge, it will change from red to green, indicating that the free edge pair has been equivalenced.

Area where free edges need to be toggled

4.

Use toggle to equivalence the other edges shown in the previous image.

Step 8: Combine the remaining free edge pair using replace. 1.

Go to the replace subpanel.

2.

In the Model browser, View folder, right-click on View2 and select Show from the context menu. The graphics area displays two edges to retain and remove for replacement.

Proprietary Information of Altair Engineering

p.52

Altair HyperMesh 2019 Tutorials

3.

With the moved edge line selector active, click the leftmost free edge.

4.

With the retained edge line selector now active, select the rightmost red edge.

5.

In the cleanup tol = field, enter 0.1.

6.

Click replace. HyperMesh posts a message similar to, "Gap = (.200018). Do you still wish to replace?".

7.

To close the gap, click Yes.

8.

To exit the replace subpanel, click return.

Proprietary Information of Altair Engineering

p.53

Altair HyperMesh 2019 Tutorials

p.54

Step 9: Find and delete all duplicate surfaces. 1.

From the menu bar, click Geometry > Defeature > Duplicates.

2.

Click surfs >> displayed.

3.

In the cleanup tol = field, type 0.01.

4.

Click find. The status bar displays the following message, "2 duplicated surfaces were found."

5.

To remove duplicate surfaces, click delete.

Step 10: Observe the model again to identify any remaining free edges, or missing or duplicate surfaces. 1.

On the Visualization toolbar, change the geometry color mode to click to shade the model's geometry and surface edges.

2.

Observe the model again to identify the remaining free edges and missing or duplicate surfaces. Note:

3.

All of the edges in the model should be displayed as green shared edges, indicating that you have a completely enclosed thin solid part.

To exit the return panel, click return.

Step 11 (Optional): Save your work. With the cleanup operations completed, now is a good time to save your work. 1.

From the menu bar, click File > Save > Model.

Proprietary Information of Altair Engineering

and

Altair HyperMesh 2019 Tutorials

p.55

HM-2010: Generating a Midsurface In this tutorial, you will learn how to: •

Create a midsurface

•

Visualize the midsurface by using shading options and transparency

This exercise uses CAD geometry data for a thin solid clip. Because of the small thickness of the part, it is assumed that it will be modeled for FEA as shell elements. The elements will be created on the mid-plane of the part.

Model Files This exercise uses the clip_midsurface.hm model file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Generating a Midsurface The surfaces in this model have no connectivity errors. This could be because the file was imported without errors or because the errors were corrected using HyperMesh. In this case, errors in the topology were repaired in the previous exercise (missing surfaces are recreated, duplicate surfaces are deleted, gaps are closed, and so on). For this tutorial, you can continue using the model you created in tutorial HM-2000, or you can open the new, clip_midsurface.hm, file. Either way, the geometry is at the point where you can use the Midsurface panel to generate a midsurface.

Step 1: Retrieve and view the model file. 1.

Open the clip_midsurface.hm model file.

2.

On the Visualization toolbar, click

to shade the model's geometry and surface

edges, and click to change the geometry color mode to mixed. The surfaces displayed in the graphics area represent a solid part. Note:

These visualization techniques will be necessary for viewing the newly created midsurface.

Step 2: Generate a midsurface from midsurface panel. 1.

From the menu bar, click Geometry > Create > Midsurfaces > Auto.

2.

Verify that the closed solid option is selected, and the entity selector is active and set to surfs.

3.

Select one surface.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

p.56

To start the midsurface generation, click extract. HyperMesh creates the midsurface, and organizes the surfaces into a new Middle Surface component. When HyperMesh creates the midsurface, transparency is turned on for all of the other components in the model except the new Middle Surface component.

Step 3: Review the part’s midsurface. 1.

In the Model browser, only display the Middle Surface component. The graphics area displays the midsurfaces generated for the solid sections of the model using the automidsurface panel.

Midsurface generated from a volume of surfaces

2.

In the Model browser, turn the geometry for the lvl10 component back on.

3.

To open the Transparency panel, click

4.

With the comps selector active, select a line or surface of the lvl10 component. HyperMesh selects the entire component because the entity selector is set to comps. Tip:

on the Visualization toolbar.

You may need to zoom in on the model to select a valid entity.

5.

Under transparency, click several times. The surfaces in the lvl10 component become more and more transparent.

6.

Optional: Drag the transparency slider back and forth to control the level of transparency.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

7.

To visualize the midsurface, rotate, zoom, and pan.

Close-up of the midsurface with the lvl10 component set to full transparency

Step 4 (Optional): Save your work. Now that the midsurface has been created, it is a good time to save the model. 1.

From the menu bar, click File > Save > Model.

Summary You have now created surfaces on the mid-plane of the part. These surfaces can now be meshed or further modifications can be made to their topology, depending on the requirements of the analysis.

Proprietary Information of Altair Engineering

p.57

Altair HyperMesh 2019 Tutorials

HM-2015: Auto-Midsurfacing with Advanced Extraction Options In this tutorial, you will learn how to: •

Use the offset+planes+sweeps option when midsurfacing.

•

Manually correct gaps in an auto-generated midsurface using the plates edit function.

In this tutorial, you will be using CAD geometry data for a box with thin ribs inside of it. Because the geometry consists of thin planar sections, it is assumed that it will be modeled for FEA as shell elements. The elements will be created on the mid-planes of each section.

Model Files This exercise uses the Insert_planes.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Generating a Midsurface

Step 1: Retrieve and View the Model File 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the Insert_planes.hm model file.

4.

From the menu bar, click Geometry > Create > Midsurfaces > Auto.

5.

In the Auto Midsurface panel, click the toggle and select closed solid.

Proprietary Information of Altair Engineering

p.58

Altair HyperMesh 2019 Tutorials

6.

Select any surface.

7.

Click extraction options.

8.

From the drop-down menu, select offset+planes+sweeps.

9.

Go to the auto extraction subpanel.

p.59

10. Click extract. 11. Shade the model's geometry and surface edges by clicking toolbar.

on the Visualization

12. Review the generated midsurface by hiding the Body.1 component in the Model browser. Some of the plates do not properly cross.

Step 2: Use Plates Edit to Resolve Midsurface Gaps 1.

In Model browser, display the component Body.1.

2.

On the Visualization toolbar, set the geometry display mode to

Proprietary Information of Altair Engineering

.

Altair HyperMesh 2019 Tutorials

3.

From the panel area, select the interim edit tools from the drop-down.

4.

From the edit plates subpanel, click show/edit all. HyperMesh populates the Model browser with plates that were detected by the tool. Note:

If you have not yet extracted the middle surface using either the offset+planes or offset+planes+sweeps options, then the model will not have any plate information yet. Plate components will not be populated in this situation.

5.

In the Model browser, hide the components Body.1 and Middle Surface.

6.

Verify that the full plate surfs selector is active.

7.

Select the green face. HyperMesh selects all of the plates in the ^Planar plate #0 component.

8.

Hide all of the plates in the ^Planar plate #0 component by right-clicking on the green face.

9.

Hide the three remaining exterior sides. HyperMesh hides the components ^Planar plate #2, ^Planar plate #3, and ^Planar plate #4.

Proprietary Information of Altair Engineering

p.60

Altair HyperMesh 2019 Tutorials

10. Select any face from the long interior rib, as shown in the following image. This rib was split into three groups by the algorithm, and needs to be reunited into one component.

11. Select the two remaining plates from the long interior rib.

12. Merge the three plates into a single planar plate by setting the plate type to planar.

13. Click merge plates or middle-click in the graphics area. HyperMesh combines the three plates into a single component and displays them in the same color.

Proprietary Information of Altair Engineering

p.61

Altair HyperMesh 2019 Tutorials

14. Using the full plate selector, select the newly created plate.

15. Click the single surface selector. The selected plate is isolated, and one side is colored blue and the other side is colored green.

16. Review the isolated plate by toggling non-plates off/non-plates on to non-plates off. 17. Notice the long narrow surface that displays with the left-most plate. Select it with the single plate

selector, and set it to plate edge.

18. Click the full plate selector to recover the view you had before isolating and reviewing the plate, and hide the plate sides shown in blue and green. 19. Merge the two remaining internal ribs. 20. Click update. 21. Click return.

Proprietary Information of Altair Engineering

p.62

Altair HyperMesh 2019 Tutorials

22. Review the generated misdurface by hiding the Body.1 component in the Model browser. The plates are closer together, but they are still not the full length of the rib due to the holes that trim the plates.

Step 3: Use Plates Edit a Second Time to Resolve Remaining Gaps In this step, you will need to tell the auto-midsurface algorithm not to trim the plates where the holes are. 1.

In the interim edit tools panel, edit plates subpanel, click show/edit all. HyperMesh populates less plate components in the Model browser because some plates were merged in the previous steps.

2.

Hide all of the components except ^Plate edge.

Proprietary Information of Altair Engineering

p.63

Altair HyperMesh 2019 Tutorials

3.

Using the single surface surfs selector, select all four internal surfaces of the two holes. Note:

Each hole has two internal surfaces.

4.

Click not a trim surface. HyperMesh organizes the selected surfaces into a new component labeled ^Not a trim surface.

5.

Click update.

6.

Click return.

Proprietary Information of Altair Engineering

p.64

Altair HyperMesh 2019 Tutorials

7.

Review the generated misdurface by hiding the Body.1 component in the Model browser. There is now a yellow edge where the plates meet, which indicates that the plates are intersected correctly. It would have been possible to reorganize the plates and create the Not a trim surface component at the same time.

Step 4 (Optional): Save Your Work 1.

From the menu bar, click File > Save > Model.

Summary The model now contains surfaces on the mid-plane of the part. You used insert planes and plates edit to ensure that there were no erroneous gaps in the generated midsurfaces. You can now mesh these surfaces, or further modify their topology, depending on the requirements of the analysis.

Proprietary Information of Altair Engineering

p.65

Altair HyperMesh 2019 Tutorials

HM-2020: Simplifying Geometry In this tutorial, you will learn how to: •

Mesh the clip, review the mesh quality, and determine the features to be simplified

•

Remove surface fillets

•

Remove edge fillets

•

Remove pinholes

This exercise involves changing the shape of a part in order to simplify the geometry. Certain details of the shape, such as small holes or blends, may simply not be necessary for the analysis being performed. When these details are removed, the analysis can run more efficiently. Additionally, mesh quality is often improved as well. Changing the geometry to match the desired shape can also allow a mesh to be created more quickly.

Model Files This exercise uses the clip_defeature.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory. This model file contains geometry that has been midsurfaced. Surfaces have been created on the mid-plane of the part.

Exercise In this exercise, you will mesh the model using an element size of 2.5. You can assume a simple structural analysis will be run on the part, and thus does not require much detail. There are unnecessary features in this model that can also be removed.

Proprietary Information of Altair Engineering

p.66

Altair HyperMesh 2019 Tutorials

p.67

Step 1: Open and view the model file, clip_defeature.hm. 1.

From the menu bar, click File > Open > Model.

2.

In the Open Model dialog, open the clip_defeature.hm model file.

Step 2: To easily work with the midsurface, turn off the display of the lvl10 component. If the lvl10 component is displayed, it needs to be turned off so that you can easily work on the midsurface geometry. 1.

In the Model browser, Component folder, click geometry display.

next to lvl10 to turn off its

Step 3: Mesh the clip to view mesh quality before defeaturing. on the Visualization

1.

To shade the model's geometry and surface edges, click toolbar.

2.

To open the AutoMesh panel, click Mesh > Create > 2D AutoMesh from the menu bar, or press F12.

3.

Set the entity selector to surfs.

4.

In the element size = field, type 2.5.

5.

From the mesh type list, select mixed.

6.

Toggle the meshing mode from interactive to automatic.

7.

Verify that the elems to surf comp toggle is set.

8.

To select all of the displayed surfaces, click surfs >> displayed.

9.

Click mesh. HyperMesh generates the mesh preview.

Initial mesh on the clip model

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

10. To exit the panel, click return.

Step 4 (Optional): Review the quality of the mesh. In this step, you will review the quality of the mesh that was created. Pay attention to the areas that have an irregular, poor quality mesh. An irregular, poor quality mesh generally contains rows and columns of quads that are not neat. You will use the Check Elements panel to evaluate the minimum length check of the elements. 1.

To open the Check Elements panel, click Mesh > Check > Elements > Check Elements from the menu bar, or press F10.

2.

Go to the 2-d subpanel.

3.

In the length < field, enter 1.

4.

To evaluate the minimum length, click length. Many of the elements that failed the length test are located around the fillets of this model. Tip:

For better visualization of element quality, you may need to display the geometry in wire frame mode by clicking on the Visualization toolbar.

Elements failing the length check

5.

To exit the panel, click return.

Step 5: Remove the four small pinholes. Pinholes are closed free edge loops within a surface. Pinholes do not need to be circular. 1.

To open the Defeature panel, click Geometry > Defeature > Pinholes from the menu bar.

2.

In the diameter < field, enter 3.0.

3.

Select surfs >> all.

Proprietary Information of Altair Engineering

p.68

Altair HyperMesh 2019 Tutorials

4.

p.69

Click find. HyperMesh identifies all of the pinholes that have a diameter of 3 or less in the model, and places a white xP symbol in their centers.

Pinholes identified using a 3 mm diameter

5.

Click delete. HyperMesh removes the selected pinholes in the model and replaces them with fixed points located at the center of the original pinholes. The mesh also updates according to the changes in the geometry.

Step 6: Remove all surface fillets in the clip. 1.

Go to the surf fillets subpanel.

2.

If the model's geometry and surface edges are not shaded, click Visualization toolbar.

3.

Under find fillets in selected, click surfs >> displayed.

4.

In the min radius field, type 2.0.

5.

Click find. HyperMesh identifies all of the surface fillets with a radius of 2 or greater in the model.

Surface fillets identified for removal

Proprietary Information of Altair Engineering

on the

Altair HyperMesh 2019 Tutorials

6.

Click remove.

Step 7: Automatically identify and remove rounded corners of surfaces. You should still be in the Defeature panel. 1.

Go to the edge fillets subpanel.

2.

Click surfs >> displayed.

3.

In the min radius field, type 1.0.

4.

To find all of the fillets in the model, set the bottom switch to all.

5.

Click find. HyperMesh identifies all of the edge fillets that meet the filter criteria, and displays a F symbol where they are located in the model along with radial lines.

Edge fillets identified for removal

6.

With the fillets entity selector active, right-click on one of the F fillet markers on the screen to deselect the fillet.

7.

Click remove. HyperMesh deletes all of the selected edge fillets except for the one which was deselected in step 6.

Step 8 (Optional): Save your work. Now that the model has been simplified, it is a good time to save the model. 1.

From the menu bar, click File > Save > Model.

Summary The model is now represented in a much simpler form that suits the analysis that will be performed. Holes, surface fillets, and edge fillets were removed that were considered too small to be captured by the desired element size of 2.5.

Proprietary Information of Altair Engineering

p.70

Altair HyperMesh 2019 Tutorials

HM-2030: Refining Topology to Achieve a Quality Mesh In this tutorial, you will learn how to: •

Mesh the part to determine poor element quality

•

Suppress small edges

•

Split surfaces

•

Remove interior fixed points

•

Replace closely placed fixed points

•

Create final mesh

Topological details of the geometry may affect the quality of the mesh created from the surfaces. Some of these details may not reflect any major feature of the part’s shape, and can be removed without concern. When modifying the topology affects the shape of the surfaces, a compromise must be made between the part shape and the element quality necessary for the analysis. Other times, adding topological features that do not change the shape of the part may actually help create a better quality mesh.

Model Files This exercise uses the clip_refine.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Refining Topology to Achieve a Quality Mesh

Step 1: Open the model file, clip_refine.hm. 1.

From the menu bar, click File > Open > Model.

2.

In the Open Model dialog, open the clip_refine.hm model file.

3.

Take a few moments to observe the model using the different visual options available in HyperMesh (rotation, zooming, etc.).

Step 2: Create a preliminary mesh. 1.

To open the Automesh panel, click Mesh > Create > 2D AutoMesh from the menu bar, or press F12.

2.

Set the entity selector to surfs.

3.

Go to the size and bias subpanel.

4.

In the element size = field, type 2.5.

5.

From the mesh type list, select mixed.

6.

Switch the meshing mode from interactive to automatic.

Proprietary Information of Altair Engineering

p.71

Altair HyperMesh 2019 Tutorials

7.

Click surfs >> displayed.

8.

Click mesh. HyperMesh meshes the surfaces.

p.72

Initial mesh on the defeatured clip model

Step 3: Review the mesh quality. 1.

Take a minute to rotate, zoom, and pan the model to review the mesh that was created. Pay attention to the locations where the mesh was not created in rows and columns of quads.

2.

To open the Check Elements panel, click Mesh > Check > Elements > Check Elements from the menu bar, or press F10.

3.

Go to the 2-d subpanel.

4.

In the length < field, enter 1.

5.

To evaluate the minimum length, click length. HyperMesh highlights the elements that failed the check.

6.

To exit the panel, click return.

7.

In the Model browser, Component folder, click the display of it's elements.

next to Middle Surface to turn off

Step 4: Remove short edges by combining fixed points. 1.

To open the Replace panel, click Geometry > Edit > Fixed Points > Replace from the menu bar.

2.

Verify that the moved points selector is active.

3.

Select the lower fixed point as indicated in the following image. Tip:

If there are no visible fixed points on your model, verify that the Display toolbar.

Proprietary Information of Altair Engineering

is selected on

Altair HyperMesh 2019 Tutorials

4.

Activate the retained point selector.

5.

Select the upper fixed point as indicated in the following image.

6.

Click replace.

Selecting fixed points to be combined

Step 5: Remove the fixed points interior to all surfaces. You should still be in the Points panel. 1.

Go to the suppress subpanel

2.

Under at cursor, verify that the point selector is active.

3.

Select the four fixed points as illustrated in the following image. HyperMesh deletes each fixed point when you select it. These fixed points are left over from a defeaturing operation where small holes (pinholes) were removed. They could remain without greatly sacrificing the element quality, given the element size used for the mesh, but the mesh would be better without them.

Fixed points to be removed

Proprietary Information of Altair Engineering

p.73

Altair HyperMesh 2019 Tutorials

4.

To exit the panel, click return.

Step 6: Add edges to the surfaces to control the mesh pattern. 1.

To open the Trim with Nodes panel, click Geometry > Edit > Surfaces > Trim with Nodes from the menu bar.

2.

Under node normal to edge, click node.

3.

Zoom into the area illustrated in the following image and select the indicated fixed point.

4.

With the lines selector now active, select the line shown in the image below. HyperMesh creates an edge from the location of the fixed point perpendicular to the line.

Select fixed point and line to split the surface.

5.

Repeat steps 6.2 through 6.4 for the point and line illustrated in the following image.

Select fixed point and line to split the surface.

Proprietary Information of Altair Engineering

p.74

Altair HyperMesh 2019 Tutorials

6.

Repeat steps 6.2 through 6.4 for the point and line illustrated in the following image.

Select fixed point and line to split the surface.

7.

Repeat steps 6.2 through 6.4 for the point and line illustrated in the following image.

Select fixed point and line to split the surface

Proprietary Information of Altair Engineering

p.75

Altair HyperMesh 2019 Tutorials

Step 7: Add edges to the surfaces to control the mesh pattern. 1.

Go to the trim with surfs/planes subpanel.

2.

In the with plane column, verify that the surfs selector is active.

3.

Select the five surfaces indicated in the following image.

Surfaces to be selected for splitting

4.

Verify that the direction selector is set to N1, N2, N3.

5.

Click N1 to make the selector active.

6.

Press and hold your left mouse button, move it over the edge as indicated in the following figure, and then release it when the cursor changes to a square with a dot in the center

.

7.

Click two points anywhere along the edge. Do not click a third. Hypermesh places nodes on the line for N1 and N2.

8.

To open the Distance panel, press F4.

9.

Go to the three nodes subpanel.

10. Press and hold your left mouse button, move it over the edge of the hole as indicated in the following image, and then release it when the cursor changes to a square with a dot in the center

.

Select fixed point and line to split the surface

Proprietary Information of Altair Engineering

p.76

Altair HyperMesh 2019 Tutorials

11. Click three points anywhere along the edge. HyperMesh places temporary nodes on the line representing N1, N2, and N3. Note:

The technique you used to create nodes to select where none existed before can be used in any place where nodes need to be selected but do not exist in the model. You can create nodes in this manner on lines, surfaces and elements. For more details, see the HyperMesh online help. Pick the index and type, Picking Nodes on Geometry or Elements.

12. Click circle center. HyperMesh creates a node at the center of the hold. 13. To exit the Surface Edit panel, click return. 14. Activate the B selector. 15. Select the node that was just created at the center of the hole. 16. Click trim. HyperMesh trims the surfaces through the center of the hole. 17. To exit the panel, click return.

Step 8:

Suppress shared edges causing a small edge.

1.

To go to the (Un)suppress panel, click Geometry > Edit > Surface Edges > (Un)Suppress from the menu bar.

2.

Select the five lines illustrated in the following image.

Surface edges to suppress by toggling

3.

Click suppress. HyperMesh suppresses each line, which in indicated by a blue, dashed line.

Step 9: Remesh the part. In this step, you will remesh the surfaces of the part, using the automatic mode, a size of 2.5, and the mixed mesh type.

Proprietary Information of Altair Engineering

p.77

Altair HyperMesh 2019 Tutorials

p.78

1.

In the Model browser, Component folder, click it's elements.

next to Middle Surface to display

2.

To open the Automesh panel, click Mesh > Create > 2D AutoMesh from the menu bar, or press F12.

3.

Verify that elem size = is set to 2.5 and the mesh type is set to mixed.

4.

To select all of the displayed surfaces, click surfs >> displayed.

5.

Click mesh.

Step 10: Review the mesh quality. 1.

Take a minute to rotate, zoom, and pan the model to review the mesh that was created. The mesh consists completely of rows and columns of quads.

2.

To open the Check Elements panel, click Mesh > Check > Elements > Check Elements from the menu bar, or press F10.

3.

Go to the 2-d subpanel.

4.

In the length < field, enter 1.

5.

To evaluate the minimum length, click length. HyperMesh highlights only two elements that failed the check. Both of these elements failed the check because of the shape of the part. These elements are not too small compared to the global element size, therefore you can leave them as is.

6.

To open the Automesh panel, click Mesh > Create > 2D AutoMesh from the menu bar, or press F12.

7.

Go to the QI optimize subpanel.

8.

Verify that elem size = is set to 2.5 and the mesh type is set to mixed.

9.

Click edit criteria.

10. In the Criteria File Editor dialog, enter 2.500 in the Target element size field. 11. Click Apply. 12. Click OK. 13. To select all of the displayed surfaces, select surfs >> displayed. 14. Click mesh. HyperMesh replaces the old mesh with a new mesh. 15. If there is a message saying, "There is a conflict between the user requested element size and quality criteria ideal element size," click the Recompute quality criteria button using a size of 2.5. 16. To access the Quality Index panel, click Mesh > Check > Elements > Quality Index from the menu bar. 17. Go to page 1. 18. Verify that the comp. QI is 0.01. This low value indicates that the mesh is good quality. The higher the number, the lower the mesh quality.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 11 (Optional): Save your work. The part is now meshed and ready to be set up for an analysis. Save the model, if desired. 1.

From the menu bar, click File > Save > Model.

Proprietary Information of Altair Engineering

p.79

Altair HyperMesh 2019 Tutorials

p.80

HM-2040: Creating and Editing Line Data In this tutorial, you will learn how to: •

Create circle, arc, line, and tangent lines

•

Duplicate and translate lines

•

Edit lines by splitting and displaying their IDs

•

Delete redundant arcs and lines

•

Duplicate and reflect an arc

•

Create a surface square and two parallel lines on an X-Y plane

•

Create a fillet between two lines

•

Exporting geometry in IGES format

Sometimes CAE users need to create models from sketches where there is no pre-existing geometry. The tools in this tutorial will help you accomplish that task.

Exercise: Creating and Editing Line Data In this exercise, you will learn how to create lines and surfaces.

Step 1: Create a component collector to geometry. 1.

To create a component, right-click in the Model browser and select Create > Component from the context menu, or click Collectors > Create > Components from the menu bar.

2.

In the Create Component dialog, enter geometry in the Name field.

3.

Click the Color swatch and select yellow from the box of colors.

4.

Click Create.

Step 2: Create nodes. 1.

On the standard toolbar, click

.

2.

To open the Create Nodes panel in the XYZ subpanel, click Geometry > Create > Nodes > XYZ from the menu bar.5

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

p.81

Enter the following X, Y, and Z coordinates listed in the table below to create five nodes. Click create for each of the nodes. Node

X

Y

Z

1

0

0

0

2

0

0

25

3

0

0

37

4

0

5

25

5

0

5

-2

4.

Click return.

5.

To fit the size of the model to the graphics area, press f.

Step 3: Display the node IDs. 1.

To open the Numbers panel, click

on the Display toolbar.

2.

Verify that the entity selector is set to nodes.

3.

To select all of the nodes in the model, click nodes >> all.

4.

Select the display check box.

5.

Click on. HyperMesh displays the node IDs.

6.

Click return.

Step 4: Create a circle. 1.

To open the Circle Center and Radius panel, click Geometry > Create > Lines > Circle Center and Radius from the menu bar.

2.

Verify that the node list selector is active.

3.

Select Node 2. This will be the location of the circle’s center.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.82

4.

Set the orientation vector to x-axis.

5.

In the radius field, enter 5.

6.

Click create. HyperMesh creates the circles's center.

Step 5: Create an arc. 1.

To open the Arc Center and Radius subpanel, click

2.

Verify that the node list entity selector is active.

3.

Select node 2. This node will be the center of the arc as well as the base for the axis of rotation.

4.

Verify that the orientation vector is set to x-axis.

5.

In the Radius field, enter 2.5.

6.

In the Offset field, enter 90.

7.

In the Angle field, enter 180.

8.

Click create. HyperMesh creates an arc.

9.

On the Standard toolbar, click

Proprietary Information of Altair Engineering

.

.

Altair HyperMesh 2019 Tutorials

p.83

Step 6: Create a line. 1.

To open the Linear Nodes subpanel, click

2.

Select Node 4 and Node 5.

3.

Click create. HyperMesh creates a line between nodes 4 and 5.

4.

Click return.

.

Step 7: Duplicate and translate lines. 1.

To open the Translate panel, click Geometry > Translate > Lines from the menu bar.

2.

Verify that the entity selector is set to lines.

3.

Select the line that was created between nodes 4 and 5.

4.

Click lines >> duplicate >> current comp. Hypermesh copies the new line into the current component, Geometry.

5.

Set the orientation vector to y-axis.

6.

In the magnitude = field, enter 10.0.

7.

Click translate-.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

8.

Click return.

Step 8: Edit lines by splitting at a line. 1.

To open the Line Edit panel, click Geometry > Edit > Lines > Split at Line from the menu bar.

2.

Verify that the lines selector is active.

3.

Select the top, right curved line of the circle indicated in the following image.

4.

Click cut line.

5.

Select the line between nodes 4 and 5.

6.

Click split. The circle has one quarter of it's radius split off from the rest.

7.

Repeat steps 8.2 through 8.6 to select the top, left curved line of the circle and the other line that was translated in step 7.

8.

Click return.

Step 9: Display the line IDs. 1.

Go to the Numbers panel.

2.

Set the entity selector to lines.

3.

Click lines >> all. HyperMesh selects all of the lines in the model.

4.

Verify that the display check box is selected.

5.

To display all of the line IDs, click on.

6.

Click return.

Proprietary Information of Altair Engineering

p.84

Altair HyperMesh 2019 Tutorials

p.85

Step 10: Delete a redundant arc. 1.

To open the Delete panel, click

on the Collectors toolbar, or press F2.

2.

Set the entity selector to lines.

3.

Select the bottom right curved line of the circle indicated in the following image.

4.

Click delete entity. HyperMesh deletes the redundant arc.

5.

Select the bottom left curve and then click delete entity.

6.

Click return.

Step 11: Duplicate and reflect an arc. 1.

To open the Reflect panel, click Geometry > Reflect > Lines from the menu bar.

2.

Set the entity selector to lines.

3.

Select the arc (line ID 2).

4.

Set the orientation vector to z-axis.

5.

Select Node 2 as the base node.

6.

Click lines >> duplicate >> original comp to copy the new line into the current component, Geometry.

7.

Click reflect. HyperMesh creates the lower arc.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

8.

Click return.

Step 12: Create two tangent lines. 1.

To go to the Tangents panel, click Geometry > Create > Lines > Tangent from the menu bar.

2.

Set the entity selector to node list.

3.

Select Node 3.

4.

Activate the line selector.

5.

Select the semi-circular line (line ID 5). Note:

Your line IDs may be different, depending on whether you needed to perform the split/delete/duplicate tasks more than once.

6.

Click create. HyperMesh creates two tangent lines.

7.

Select one of the tangent lines.

8.

Repeat steps 12.3 through 12.7.

9.

Select the other tangent line.

Proprietary Information of Altair Engineering

p.86

Altair HyperMesh 2019 Tutorials

10. To exit the panel, click return.

Step 13: Redisplay the line IDs. 1.

Go to the Numbers panel.

2.

Set the entity selector to lines.

3.

Click lines >> all.

4.

Verify that the display check box is selected.

5.

Click on. HyperMesh displays all of the line IDs.

6.

To exit the panel, click return.

Step 14: Split curves by tangent line and delete redundant line. 1.

Go to the Split at Line subpanel.

2.

Verify that the lines selector is active.

3.

Select the semi-circular line (ID 5). Note:

The line IDs may be different.

4.

Click cut line.

5.

Select the left tangent line (ID 9).

6.

Click split. HyperMesh splits the semi-circular line (ID 5) with the selected tangent line (ID 9).

7.

Repeat steps 14.2 through 14.6 to cut the semi-circular line (ID 5) with the right tangent line (ID 8).

Proprietary Information of Altair Engineering

p.87

Altair HyperMesh 2019 Tutorials

8.

Go to the Delete panel.

9.

Verify that entity selector is active and set to lines.

10. Select the semi-circular line between the two tangent lines indicated in the following image.

11. Click delete entity. HyperMesh deletes the semi-circular line. 12. To exit the panels, click return twice.

Proprietary Information of Altair Engineering

p.88

Altair HyperMesh 2019 Tutorials

Step 15: Create a component collector for surfaces. 1.

In the Model browser, right-click and select Create > Component from the context menu.

2.

In the Create component dialog, enter surfaces in the Name field.

3.

Click the Color icon, and select purple.

4.

Click Create.

Step 16: Create a surface square on an X-Y plane. 1.

From the main menu, go to the 2D page and select Planes.

2.

Go to the Square subpanel.

3.

Set the orientation vector to z-axis.

4.

Select Node 1 as the base reference node.

5.

Switch mesh, keep surf to surface only.

6.

In the size= field, enter 30.

7.

Click create. HyperMesh creates a square surface.

8.

To exit the panel, click return.

Step 17: Create a line that connects two parallel lines on an X-Y plane. 1.

To open the Intersect panel, click Geometry > Create > Lines > Intersect.

2.

To create a line on the X-Y plane, set the orientation vector to z-axis.

Proprietary Information of Altair Engineering

p.89

Altair HyperMesh 2019 Tutorials

p.90

3.

Select Node 1 as the base node.

4.

Activate the line list selector.

5.

Select the two straight lines that are perpendicular to the X-Y plane indicated in the following image. HyperMesh displays a bold, white line in the graphics area to represent the results.

6.

Click create. HyperMesh creates the line.

7.

To exit the panel, click return.

Step 18: Switch the current working component surfaces to geometry. 1.

In the Model browser, Component folder, right-click on geometry and select Make Current from the context menu. Note:

From this point on, when you create any new elements or geometry, HyperMesh will place them in the geometry component collector.

Step 19: Extend a line to a surface edge. 1.

On the Standard Views toolbar, click

2.

To open the Extend panel, click Geometry > Edit > Lines > Extend from the menu bar.

3.

Toggle from distance = to to:.

4.

Set the entity selector to line.

Proprietary Information of Altair Engineering

.

Altair HyperMesh 2019 Tutorials

5.

Activate the top line selector.

6.

Select the line that you created in step 17 (the line that passes through Node 1) as the line to be extended. HyperMesh places a red V at the beginning of the line to be extended.

7.

Activate the lower line selector.

8.

Select the lower-right edge of the purple plane indicated in the following image.

Proprietary Information of Altair Engineering

p.91

Altair HyperMesh 2019 Tutorials

9.

Click extend-. HyperMesh extends the line to reach one surface edge.

10. To exit the panel, click return. Your model should resemble the following image.

Step 20: Create a fillet between two lines. 1.

To open the Fillet subpanel, click Geometry > Create > Lines > Fillet from the menu bar.

2.

Select the Trim original lines check box.

3.

In the Radius= field, enter 5.

4.

Activate the 1st line selector.

Proprietary Information of Altair Engineering

p.92

Altair HyperMesh 2019 Tutorials

5.

Select the vertical line through which the extended line passes indicated in the following image.

6.

Activate the 2nd line selector.

7.

Select the extended line that you created in step 19. The status bar reads, "Please select fillet quadrant", which indicates that HyperMesh wants you to select a reference location for the fillet.

Proprietary Information of Altair Engineering

p.93

Altair HyperMesh 2019 Tutorials

8.

Select the top, right X for the fillet quadrant indicated in the following image. HyperMesh creates a fillet.

9.

To return to the Lines panel, click return.

Proprietary Information of Altair Engineering

p.94

Altair HyperMesh 2019 Tutorials

Step 21: Trim a line by plane and delete a redundant line segment. 1.

To open the Split at Plane panel, click Geometry > Edit > Lines > Split at Plane from the menu bar.

2.

Verify that the lines selector is active.

3.

Select the vertical line that does not have a fillet indicated in the following image.

4.

Set the orientation vector to z-axis.

5.

Select Node 1 as the base node.

6.

Click split. HyperMesh splits the line by the X-Y plane.

7.

Go to the Delete panel.

8.

Set the entity selector to lines.

Proprietary Information of Altair Engineering

p.95

Altair HyperMesh 2019 Tutorials

9.

Select the small line segment under the X-Y plane.

10. Click delete entity. HyperMesh removes the line segment. 11. To exit the panels, click return twice.

Step 22: Remove all temp nodes. 1.

To go to the Temp Nodes panel, click Mesh > Delete > Nodes from the menu bar, or press Shift + F2.

2.

Click clear all. HyperMesh removes all of the temp nodes.

3.

To exit the panel, click return.

Step 23: Change the rendering mode. 1.

To shade the model's geometry and surface edges, click on the Visualization toolbar. The plane (purple) becomes shaded instead of wire frame.

Proprietary Information of Altair Engineering

p.96

Altair HyperMesh 2019 Tutorials

Step 24: Export all geometry as an IGES file. 1.

To open the Export Geometry tab, click File > Export > Geometry from the menu bar.

2.

From the File type list, select Iges.

3.

From the File field, navigate to the location of your working directory and save the file.

4.

From the Units field, select an export unit system.

5.

Click Export. HyperMesh generates the IGES file. Note:

This file can be shared with other CAD packages such as UG, Catia, and ProE.

Proprietary Information of Altair Engineering

p.97

Altair HyperMesh 2019 Tutorials

HM-2050: Creating Surfaces from Elements In this tutorial, you will learn how to: •

Generate surfaces from existing elements

•

Plot elements

•

Control what surfaces are created

The surfaces created in this process are regular surfaces that can be used for geometry editing (for changes to a design) and meshing, and to export geometry information (in reverse engineering applications, for example). This is particularly useful if you are trying to obtain geometry information (surfaces) from a model containing elements only.

Model Files This exercise uses the fe_to_surf.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory. The model is the tetrahedral mesh of a bracket. It is organized into a single component, and does not contain any entities besides the solid elements.

Exercise

Step 1: Open the model fe_to_surf.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

Proprietary Information of Altair Engineering

p.98

Altair HyperMesh 2019 Tutorials

3.

In the Open Model dialog, open the fe_to_surf.hm model file.

4.

Review the shape of the bracket. Note:

This solid mesh was obtained by running the HyperMesh tetramesher on a tria mesh of the surfaces defining the initial part.

In this tutorial, you will reverse this process by obtaining the shell elements and then the surfaces. You can then, for example, remesh the surfaces with a different element size, or export them as an IGES file.

Step 2: Use the faces panel to generate shell elements on the outside of the solid mesh 1.

To open the Faces panel, select faces from the Tool page.

2.

Verify that the entity selector is set to comps.

3.

Select any element. HyperMesh temporarily highlights the element, which signifies that the component has been selected.

4.

You do not have to change the tolerance field, as it does not influence the creation of face elements.

5.

Click find faces. HyperMesh creates shell elements on the free faces of the solid elements (faces that are not shared with any other element), and places them into the ^faces component collector.

6.

In the Model browser, turn off the element display of the tetras component.

7.

To return to the main menu, click return.

Faces (shell) elements

Proprietary Information of Altair Engineering

p.99

Altair HyperMesh 2019 Tutorials

p.100

Step 3: Obtain surfaces from elements. In this step, you will use the Surfaces panel and the From FE subpanel on the tria (faces) elements to obtain surfaces and understand the behavior of the panel. 1.

To open the From FE subpanel, click Geometry > Create > Surfaces > From FE from the menu bar.

2.

To select all of the displayed elements, click elems >> displayed.

3.

Use the toggles to select Auto Detect Features and Mesh Based Auto Tol. Note:

Auto Detect Features automatically creates 1D plot elements at feature lines. Features are created where the normals of adjacent elements vary more than the feature angle specified in the Options panel. Once the feature lines are created, it also combines open-ended features to form closed loops. These features are used as delineations for the new surfaces being created. Mesh-Based Auto Tol determines the tolerance as a factor of the average element size. The new surfaces created are allowed to deviate from the existing mesh no more than the specified/calculated tolerance value.

4.

Set the Surface Complexity to 5 using the slider bar.

5.

Click create. It may take HyperMesh up to 40 seconds to create surfaces.

6.

In the Model browser, turn off the display of all the elements to review the surfaces that were created.

7.

Click return.

8.

To shade the model's geometry and surface edges, click toolbar.

9.

Review the surface by rotating and zooming in and out of the model. The delineation of the surfaces may or may not correspond to what you may expect or wish to obtain. For example, you may want to have three separate surfaces in some areas of the model and fewer surfaces in other areas.

on the Visualization

10. To go to the Delete panel, press F2. 11. Verify that the entity selector is to set surfs. 12. Click surfs >> all. 13. Click delete entity. 14. In the Model browser, turn on the element display of the ^faces component. 15. Click return. In this step, you have learned how to use the FE surf panel to generate some surfaces that can later be meshed. You have also seen that when the surface generation engine (From FE tool) is asked to create surface delineation automatically, the surfaces obtained may not necessarily have the specific delineation you wish to obtain. In order to obtain specific delineation, plot elements can be used to define the boundaries of the various surfaces, and can be supplied to the engine (From FE tool).

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.101

Step 4: Capture features with plot elements. Delineating the surfaces to be created is an essential step in obtaining the desired surfaces. This level of control is achieved by supplying the surface generator with some plot elements, which will indicate what the boundaries of the various surfaces should be. This function works well only when the selected plot elements form closed loops. The new surfaces should have boundaries that respect the features of the tria mesh. The tria mesh captures, to some extent, the features of the initial geometry. Generate plot elements that correspond to the features of the mesh. You can use the edges, features, and edit element panels to create plot elements. Using the Features panel is one of the most automated ways of generating plot elements, although it does not always create the features as desired. Some manual methods will be used to modify the results of automatic feature creation. In this step, you will use the features panel to automatically generate plot elements capturing the features of the tria mesh (^faces component). Use a break angle of 30 degrees. 1.

To open the Features panel, click features from Tool page.

2.

Set the entity selector to elems.

3.

Click elems >> displayed.

4.

In the feature angle= field, enter 30.

5.

Change the analysis option from simple to advanced. Note:

This option performs further analysis on the features created based on the angle and combines and extends them to create closed loops.

6.

Click features. HyperMesh generates plot elements representing the features of the mesh. These plots elements are automatically created in a component collector named ^feature.

7.

Zoom into the areas indicated in the following image to see how many plot elements were created to define the boundary area. Note:

In the following steps you will remove the unnecessary plot elements.

Plot elements representing features

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

8.

Go to the edit subpanel.

9.

Activate the element features to remove: elem selector.

10. Select one of the plot elements indicated in the following image. HyperMesh selects the entire row of elements to the next intersection as you select the plot elements. 11. Click remove.

Features to be removed

12. Repeat steps 4.10 and 4.11 to remove the remaining plot elements.

Step 5: Add a new delineation feature 1.

Activate the nodes to add features: node list selector.

2.

Click nodelist >> by path.

3.

Select the nodes indicated in following image. HyperMesh selects all of the nodes in the path between these two nodes.

4.

Click add. HyperMesh creates a new feature line.

Nodes to create a new feature

Proprietary Information of Altair Engineering

p.102

Altair HyperMesh 2019 Tutorials

5.

Rotate, zoom, and pan the model to locate the features created with a zigzag pattern, as indicated in the following image. Note:

In the following steps, you will delete these features and create new smooth ones.

6.

Activate the element features to remove: elem selector.

7.

Select one of the plot elements as indicated in the following image. HyperMesh selects the entire row of elements to the next intersection as you select plot elements.

8.

Click remove.

Plot elements to be removed

9.

Repeat steps 5.7 and 5.8 to remove the remaining plot features.

10. Activate the nodes to add features: node path selector. 11. Select the nodes indicated in following image. HyperMesh selects all of the nodes in the path between these two nodes. 12. Click add. HyperMesh creates a new feature line.

Proprietary Information of Altair Engineering

p.103

Altair HyperMesh 2019 Tutorials

New features added

13. Repeat steps 5.11 and 5.12 to select the nodes indicated in the previous image, and create a new feature line. 14. Repeat the previous cleanup operations to create features to your needs. The following image shows an example of the final features. Notice that many of the features in the cylindrical holes have been removed.

Model with corrected features

You created plot elements that will be used in the surfaces panel to indicate the boundaries of the surfaces to generate. These plot elements were generated in an attempt to capture the features of the tria mesh. The number and location of plot elements generated using this approach is directly dependent on the value that is chosen for the feature angle. In most situations, a lower feature angle will generate more plot elements while a higher one will yield fewer plot elements. It is often useful to experiment with different values for the feature angle as one value may bring you much closer to the desired set of plot elements than another, significantly limiting the amount of subsequent editing required.

Proprietary Information of Altair Engineering

p.104

Altair HyperMesh 2019 Tutorials

In this section, you learned how to create and edit plot elements using the features panel. The creation process was straightforward, but required some editing in order to obtain a set of plot elements forming closed loops only. Various tools are available to make the editing process as easy as possible and you used the ones that would allow you to get to your goal the most effectively. Now that both the shell elements and the plot elements delineating the surfaces are available, you will generate surfaces on the entire model.

Step 6: Generate surfaces using the Surfaces panel's from FE subpanel 1.

Open the From FE subpanel.

2.

Click elems >> by collector.

3.

Select the ^faces check box.

4.

Click select.

5.

Use the first toggle to select the feature edges selector.

6.

Click feature edges >> by collector.

7.

Select the ^feature check box.

8.

Click select.

9.

Leave all other options unchanged.

10. Click create. 11. In the Model browser, turn off the display of all the elements to review the surfaces that were generated. 12. Click return.

Surfaces generated

Proprietary Information of Altair Engineering

p.105

Altair HyperMesh 2019 Tutorials

The surfaces generated could now be exported or used for any surface editing or meshing operation. This concludes this tutorial. You may discard this model or save it to your working directory for your own reference. As this tutorial showed, this is a powerful tool in generating surface data where none is available, but needed. It also provides you with a great deal of control over the surfaces that are generated through the use of plot elements. Automated and semi-automated ways let you create and edit plot elements quickly and easily.

Proprietary Information of Altair Engineering

p.106

Altair HyperMesh 2019 Tutorials

HM-2060: Creating and Editing Solid Geometry In this tutorial, you will learn what solid geometry and topology is, and what 3D topology looks like. Solids are geometric entities that define a three-dimensional volume. Geometric entities are defined as follows: •

Point: 0 dimensional; has only x, y, and z coordinates

•

Line: one-dimensional; has length, can be curved through three-dimensional space

•

Surface: two-dimensional; has an area

•

Solid: three-dimensional; has a volume

The use of solid geometry is helpful when dividing a part into multiple volumes, for example, to divide a part into simple, mappable regions for hex meshing.

Model Files This exercise uses the solid_geom.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Proprietary Information of Altair Engineering

p.107

Altair HyperMesh 2019 Tutorials

Exercise: Creating and editing solid geometry

Step 1: Retrieve model file, solid_geom.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the solid_geom.hm model file.

Step 2: Create solid geometry from the bounding surfaces. 1.

To open the Bounding Surfaces, click Geometry > Create > Solids > Bounding Surfaces from the menu bar.

2.

Verify that the Auto select solid surfaces check box is selected.

3.

Select one surface on the part. HyperMesh automatically selects all of the surfaces.

4.

Click create. HyperMesh creates the solid, and the status bar displays message that says one solid has been created. Note:

5.

The solids are identified by thicker lines than surfaces.

To exit the panel, click return.

Step 3: Create a solid geometry cylinder using primitives. 1.

To open the Cylinder Full panel, click Geometry > Create > Solids > Cylinder Full from the menu bar.

2.

Click bottom center and then select one of the temporary nodes as illustrated in the following image. The cursor advances to the normal vector selector.

Proprietary Information of Altair Engineering

p.108

Altair HyperMesh 2019 Tutorials

p.109

3.

Select the remaining temporary node shown in the previous image.

4.

In the Base radius=, enter 1.5.

5.

In the Height= field, enter 25.

6.

Click create. HyperMesh creates solid cylinder in the middle of the first solid that was created.

7.

To exit the panel, click return.

Step 4: Subtract the cylinder’s volume from the rest of the part. 1.

To open the Boolean subpanel, click Geometry > Edit > Solids > Boolean from the menu bar.

2.

Verify that operation type: is set to simple (combine all).

3.

Set operation: to A-B (remove B from A).

4.

Verify that the A: solids selector is active, and then select the original solid.

5.

Activate the B: solids selector, and then select the solid cylinder created in step 3.

6.

Click calculate.

7.

Click return.

8.

To confirm the material has been removed, click rotate the model to inspect the part.

on the Visualization toolbar and

Step 5: Split the solid geometry using bounding lines. 1.

To go to the trim with lines subpanel, click Geometry > Edit > Solids > Trim with Lines subpanel.

2.

Activate the with bounding lines selector and set it to solids.

3.

Click anywhere on the model to select it.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

Under the with bounding lines selector, activate the lines selector.

5.

Select the four lines indicated in the following image.

6.

Click trim. HyperMesh trims a plane. Note:

The two solids now intersect.

Proprietary Information of Altair Engineering

p.110

Altair HyperMesh 2019 Tutorials

p.111

Step 6: Split the solid geometry using a cut line. In this step, you should still be in the Solid Edit panel, trim with lines subpanel. 1.

Activate the with cut lines selector and set it to solids.

2.

Select the small, tetrahedral shaped solid created in step 5.

3.

In the Model browser, View folder, right-click on View1 and select Show from the context menu.

4.

Click drag a cut line.

5.

To define the end points of a line that roughly divides the tetrahedral solid in half, select the two locations indicated in the following image.

6.

To split the solid, middle-mouse click.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

7.

Select the half of the original tetrahedral solid indicated in the following image.

8.

To split the solid indicated in the following image, repeat steps 6.4 through 6.6.

9.

Select the solid indicated in the following image.

Proprietary Information of Altair Engineering

p.112

Altair HyperMesh 2019 Tutorials

10. In the Model browser, View folder, right-click on View2 and select Show from the context menu. 11. To split the solid indicated in the following image, repeat steps 6.4 through 6.6.

Step 7: Merge solids together. In this step, you should still be in the Solid Edit panel. 1.

Go to the merge subpanel.

2.

Activate the to be merged: solids selector.

3.

Select the three solids indicated in the following image.

4.

Click merge. HyperMesh merges the solids. Note:

The resulting solids in the tetrahedral area should resemble the following image. There should be two solid entities, with one of them being hexahedral in shape in the corner.

Proprietary Information of Altair Engineering

p.113

Altair HyperMesh 2019 Tutorials

Step 8: Split the solid geometry with a user-defined plane. In this step, you should still be in the Solid Edit panel. 1.

Go to the trim with plane/surf subpanel.

2.

From the Model browser, View folder, right-click on View3 and select Show from the context menu.

3.

Activate the with plane selector and set to solids.

4.

Select the large solid representing the majority of the part.

5.

Set the orientation vector to N1, N2, N3.

6.

With N1 active, press and hold your left mouse button, and move the mouse cursor over one of the edges indicated in the following image. HyperMesh highlights the edge.

Proprietary Information of Altair Engineering

p.114

Altair HyperMesh 2019 Tutorials

7.

Release the mouse button, and left-click in the middle of the edge. A green temp node appears at the location to indicate the selection for N1. Note:

The plane selector advances to the N2 selection.

8.

In the same manner, highlight the other line shown in the previous image.

9.

Release the mouse button, and select two nodes along its length. Note:

Your selection should look similar to the following image.

Proprietary Information of Altair Engineering

p.115

Altair HyperMesh 2019 Tutorials

10. Click trim. HyperMesh trims the solid.

Step 9: Split the solid geometry with a swept line. In this step, you should still be in the Solid Edit panel. 1.

Go to the trim with lines subpanel.

2.

Activate the with sweep lines selector and set it to solids.

3.

Select the solid with the cylinder removed.

4.

Activate the lines selector.

Proprietary Information of Altair Engineering

p.116

Altair HyperMesh 2019 Tutorials

5.

Select the edges indicated in the following image.

6.

Under sweep to:, set the orientation vector to x-axis.

7.

Under the orientation vector, verify that sweep all is selected.

6.

Click trim. HyperMesh trims the solid.

Step 10: Split the solid geometry with a principal plane. In this step, you should still be in the Solid Edit panel. 1.

Go to the trim with plane/surf subpanel.

2.

Activate the with plane selector and set it to solids.

3.

Select the solid with the cylinder removed.

4.

Set the orientation vector to z-axis.

5.

Press and hold your left mouse button, and move the mouse cursor over the edge indicated in the following image. HyperMesh highlights the edge.

Proprietary Information of Altair Engineering

p.117

Altair HyperMesh 2019 Tutorials

6.

Release the mouse button, and left-click anywhere along the edge. A purple temp node appears at the location to indicate the selection for the base node.

7.

Click trim. HyperMesh trims the solid.

8.

To exit the panel, click return.

Step 11: Split the solid geometry by creating surfaces inside the solids. 1.

To open the Spline/Filler subpanel, click Geometry > Create > Surfaces > Spline/Filler from the menu bar.

2.

Clear the Auto create (free edges only) and keep tangency check boxes.

3.

Select the five lines indicated in the following image.

Proprietary Information of Altair Engineering

p.118

Altair HyperMesh 2019 Tutorials

4.

Click create. HyperMesh creates a surface.

5.

To exit the panel, click return.

6.

To go to the Trim with Plane/Surface subpanel, click Geometry > Edit > Solids > Trim with Plane/Surfaces from the menu bar.

7.

Activate the with surfs selector and set to solids.

8.

Select the solid with the cylinder removed.

9.

Activate the surfs selector.

10. Select the surface that you created in step 11.4. 11. Click trim. 12. To exit the panel, click return. 13. Go to the Spline/Filler subpanel. 14. Set the entity selector to lines. 15. Select the four lines indicated in the following image.

Proprietary Information of Altair Engineering

p.119

Altair HyperMesh 2019 Tutorials

p.120

16. Click create. HyperMesh creates a surface. 17. To exit the panel, click return. 18. Go to the Trim with Plane/Surface subpanel. 19. Activate the with surfs selector and set it to solids. 20. Select the solid you created a surface for in step 11.16. 21. Activate the surfs selector. 22. Select the surface that you created in step 11.16. 23. Clear the extend trimmer check box. 24. Click trim. 25. To exit the panel, click return.

Step 12: Suppress extraneous edges on the part. 1.

To open the (Un)Suppress subpanel, click Geometry > Edit > Surface Edge > (Un)Suppress from the menu bar.

2.

Click lines >> by geoms.

3.

Verify that the solids selector is active.

4.

Select the three solids indicated in the following image. Tip:

To view a more efficient graphical representation of the solids, set the surface display mode to

.

5.

Click add to selection.

6.

In the breakangle = field, enter 45.

7.

Click suppress. HyperMesh suppresses the edges.

8.

To exit the panel, click return.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

HM-2070: Geometry and Mesh Editing Using the Quick Edit Panel This tutorial will explore the geometry and mesh editing functions available in the Quick Edit panel. The Quick Edit panel provides easy access to a number of geometry editing mesh editing tools. More than a dozen functions are presented in this single panel. Many of the functions can be found in other HyperMesh panels. These tools may be used before creating the surface mesh to simplify geometry, correct geometry errors, or add additional geometric features to control the mesh generation. Additionally, if a mesh already exists on the geometry, you have the option of automatically remeshing the geometry as you modify it.

Model Files This exercise uses the base_bracket.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Retrieve model file, base_bracket.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the base_bracket.hm model file.

Step 2: Create a baseline mesh. 1.

To open the Automesh panel, click Mesh > Create > 2D Automesh from the menu bar, or press F12.

2.

Verify that you are in the size and bias subpanel.

3.

In the element size = field, enter 0.1.

4.

Set the mesh type: to mixed.

5.

Verify that first toggle is set to elements to surf comp.

6.

Verify that entity selector is set to surfs.

7.

Click surfs >> displayed. HyperMesh selects all of the displayed surfaces.

8.

Click mesh.

Proprietary Information of Altair Engineering

p.121

Altair HyperMesh 2019 Tutorials

9.

To exit the panel, click return.

In the next step, you will start refining the geometry and improving the mesh quality. HyperMesh has the ability to automatically remesh a surface if any topology changes are made to the geometry. This function is controlled by a setting in the Preferences > Meshing Options panel under topology revision. The default option is to remesh the surface; however, you can opt to keep or delete the mesh instead. For the base component, your focus will be to improve the mesh quality around the large holes in the side surface and the mounting holes on the flanges. You will remove the oblong holes, and improve the mesh quality around the five small holes on the top surface by trimming in a "washer" surface around the holes.

Step 3: Simplify the geometry by removing unnecessary holes. 1.

To open the Quick Edit panel, click Mesh > Quick Edit from the menu bar, or press F11.

2.

Activate the unsplit surf: line(s) selector.

3.

Select the six oblong holes under the large circular holes. HyperMesh removes them and re-generates the mesh.

Proprietary Information of Altair Engineering

p.122

Altair HyperMesh 2019 Tutorials

p.123

Step 4: Modify geometry around remaining small holes. 1.

Adjust your view to zoom in to the notched area of the top surface indicated in the following image.

2.

Activate the split surf-line: node selector and select the node indicated in the following image.

3.

With the split surf-line: line selector now active, select the line indicated in the following image. HyperMesh trims the surface.

4.

Repeat steps 4.2 through 4.3 to create four more trim lines in the locations indicated in the following image. At the end, each of the four small holes is isolated in its own rectangular surface patch.

Surface trim lines isolating small holes onto individual surfaces. Note that element display has been turned off for clarity.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 5: Trim a washer layer into the surface around each of the four holes. 1.

In the offset value field, enter 0.05.

2.

Activate the washer split: line(s) selector.

3.

Select the free surface edges (red edges) around the four small holes. HyperMesh creates a washer around each hole.

4.

Activate the adjust/set density left line(s) selector.

5.

Left-click, twice, on one of the hole's inner surface edges indicated in the following image. HyperMesh adjusts the element density from 2 to 4. Tip:

Left-click a surface edge to increase the element density by one, or right-click to decrease the element' density by one.

Proprietary Information of Altair Engineering

p.124

Altair HyperMesh 2019 Tutorials

6.

Activate the adjust/set density right line(s) selector.

7.

Left-click on the inner surface edge that you just adjusted. HyperMesh sets the target density.

8.

Right-click on the hole's other inner surface edge, indicated in the following image, to apply the target density. HyperMesh adjusts the element density from 2 to 4.

9.

Repeat steps 5.4 through 5.8 to set a target density and apply it to the remaining inner surface edge's of the other three holes. All of the hole's should have a total inner element density of 8, with each inner surface edge having an element density of 4.

10. Activate the adjust/set density left line(s) selector. 11. Left-click on one of the hole's outer surface edges indicated in the following image. HyperMesh adjusts the element density from 3 to 4.

Proprietary Information of Altair Engineering

p.125

Altair HyperMesh 2019 Tutorials

12. Activate the adjust/set density right line(s) selector. 13. Left-click on the outer surface edge that you just adjusted. HyperMesh sets the target density. 14. Right-click on the hole's other outer surface edge, indicated in the following image, to apply the target density. HyperMesh adjusts the element density from 3 to 4.

15. Repeat steps 5.10 through 5.14 to set a target density and apply it to the remaining outer surface edge's of the other three holes. All of the hole's should have a total outer element density of 8, with each outer surface edge having an element density of 4. Note:

You may not have to adjust the density for every hole's outer surface edge, as some may already have an element density of 4.

16. Activate the adjust/set density left line(s) selector. 17. Left-click on one of the hole's surface trim lines as indicated in the following image. HyperMesh adjusts the trim line's element density from 3 to 4.

Proprietary Information of Altair Engineering

p.126

Altair HyperMesh 2019 Tutorials

18. Activate the adjust/set density right line(s) selector. 19. Left-click on the surface trim line that you just adjusted. HyperMesh sets the target density. 20. Right-click on the surface trim line, indicated in the following image, to apply the target density. HyperMesh adjusts the trim line's element density from 3 to 4. Note:

You do not have to adjust the element density for the other trim lines that surround the hole, as they already have an element density of 4.

21. Repeat steps 5.16 through 5.20 to set a target density and apply it to the remaining surface trim lines that surround the other three holes. Each trim line should an element density of 4.

Step 6: Adjust the mesh around the large holes on the side surfaces. In this step, you should still be in the Quick Edit panel. 1.

Adjust your view to zoom into the three large holes on one side of the model.

2.

Use the split-line function, that you learned in step 4, to trim 12 surfaces patches around the large holes as indicated in the following image.

Note that element display has been turned off for clarity.

Proprietary Information of Altair Engineering

p.127

Altair HyperMesh 2019 Tutorials

Step 7: Remesh the newly trimmed surfaces. In this step, you will use the trim surfaces that you just created around the larges holes to apply a mapped meshing algorithm to. The mapped meshing algorithms applies a mesh pattern template to a surface, and then maps that pattern to the specific surface size and shape. In order for this method to be applied, a certain criteria must be met, including element type (quads only mesh), surface shape (three, four, or five edges), and specific mesh density settings. In step 5, you trimmed the surfaces around the large holes into faces that can be meshed with the map as pentagon algorithm, provided the mesh type and density settings are correct. 1.

To open the Automesh panel, press F12.

2.

Verify that the entity selector is set to surfs.

3.

Select the 12 surface patches around the three holes that you just created.

4.

Verify that you are in the size and bias subpanel.

5.

Verify that the meshing mode is set to interactive.

6.

Set the mesh type: to quads.

7.

Click mesh. The interactive meshing module opens.

8.

In the density subpanel, verify that the selector is active.

9.

Adjust the density on the six edges across the center of the holes from 1 to 2.

10. Go to the mesh style subpanel. 11. Set the mesh method to map as pentagon, and then click set all. 12. Click mesh. HyperMesh regenerates the mesh.

Proprietary Information of Altair Engineering

p.128

Altair HyperMesh 2019 Tutorials

13. To accept the mesh and go back to the Automesh panel, click return. This completes this tutorial. For more practice using these methods, use the other components in the model.

Proprietary Information of Altair Engineering

p.129

Altair HyperMesh 2019 Tutorials

HM-2080: Modifying Models using solidThinking Inspire In this tutorial, you will: •

Open geometry in HyperMesh Desktop

•

Export your geometry

•

Import geometry in solidThinking Inspire

•

Modify geometry inside solidThinking Inspire

•

Export modified geometry

•

Import geometry back into HyperMesh Desktop

The benefit of using solidThinking is that you can apply quick geometry fixes without going back to the CAD software.

Model Files This exercise uses the rail_extrusion.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Modify model using solidThinking

Step 1: Open and view the model file, rail_extrusion.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the rail_extrusion.hm model file.

Step 2: Export model file. 1.

From the menu bar, click File > Export > Geometry.

2.

From the File type list, select Inspire.

3.

In the File field, navigate to your working directory and save the file as rail_extrusion.stmod.

4.

Click Export.

5.

Close HyperMesh.

Proprietary Information of Altair Engineering

p.130

Altair HyperMesh 2019 Tutorials

Step 3: Open and view the model file in solidThinking Inspire. 1.

Launch solidThinking Inspire.

2.

From the menu bar, click File > Open.

3.

In the Open File dialog, navigate to your working directory and open the rail_extrusion.stmod file.

Step 4: Edit the Geometry 1.

Select the Push/Pull tool.

2.

To reduce the length of the model, click on one end of the rail and push.

3.

To increase the height of the model, click on the bottom of the rail and pull it.

Proprietary Information of Altair Engineering

p.131

Altair HyperMesh 2019 Tutorials

4.

p.132

Your modified geometry might look something like the example below. It is now ready to be transferred into HyperMesh Desktop.

Step 5: Export geometry from solidThinking Inspire. 1.

From the menu bar, click File > Save As.

2.

From the Save as type list, select Inspire Model (*.stmod).

3.

From the File name field, navigate to your working directing and save the file.

4.

Exit solidThinking Inspire.

Step 6: Import geometry in HyperMesh Desktop. 1.

Open HyperMesh.

2.

From the menu bar, click File > Import > Geometry.

3.

From the Import tab, click

4.

In the Select Auto Detect file dialog, navigate to your working directory and open the rail_extrusion.stmod file.

5.

Click Import. The graphics area displays your modified geometry.

.

Step 7 (Optional): Save your model as a HyperMesh binary file. 1.

From the menu bar, click File > Save As > Model.

2.

In the Save Model As dialog, navigate to your working directory and save the file as a HyperMesh binary file.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.133

HM-2090: Dimensioning In this tutorial you will learn how to create and edit dimensions on geometry using the Dimensioning tool. This tool is used to change one or more dimensions of existing geometry, thus changing the basic shape of solids and other enclosed volumes. With the dimensioning tool, you can select dimensions of or between surfaces, and modify those dimensions as required with the use of dimension manipulators.

Model Files This exercise uses the 2_holes.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Open the model 2_holes.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the 2_holes.hm model file.

Step 2: Create a dimension for the thickness of the part. 1.

In the Model browser, right-click and select Create > Feature from the context menu.

2.

In the Feature dialog: •

For Point1, click Unspecified >> Point.

•

Select point1 as indicated in the following image, then click proceed in the panel. Tip:

If there are no visible fixed points on your model, verify that selected on the Display toolbar.

is

•

For Point2, click Unspecified >> Point.

•

Select point2 as indicated in the following image, then click proceed in the panel.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

•

For Parameterization, leave it set to the default Create Parameter value.

•

Click Create. A dimension feature (Dimension1) and an associated parameter (Dimension1) are created. A dimension manipulator with a value of 0.375 is created between the two points to represent the thickness of the part.

•

3.

Click Close.

Repeat step 2 to create a second dimension feature for the hole. Select the points indicated in the following image. A dimension feature (Dimension2) and an associated parameter (Dimension2) are created. A dimension manipulator with a value of 0.875 is created between the two points to represent the diameter of the hole.

Proprietary Information of Altair Engineering

p.134

Altair HyperMesh 2019 Tutorials

4.

Repeat step 2 to create a third dimension feature for the other remaining hole. A dimension feature (Dimension3) and an associated parameter (Dimension3) are created. A dimension manipulator with a value of 0.75 is created between the two points to represent the diameter of the hole.

Step 3: Change the dimension value. 1.

In the Model browser, Feature folder, click Dimension1.

2.

Click the dimension value (0.375) of the dimension manipulator, and enter 0.25 in the editable field. The part's thickness decreases.

3.

In the Model browser, Parameter folder, click Dimension1.

4.

In the Entity Editor, Double value field, change the value from 0.25 to 0.5. The part's thickness increases.

Proprietary Information of Altair Engineering

p.135

Altair HyperMesh 2019 Tutorials

p.136

Step 4: Modify the dimension manipulator direction. 1.

Open the Extract on Lines panel by clicking Geometry > Create > Nodes > Extract on Line from the menu bar.

2.

Verify that the lines selector is active.

3.

Select the line indicated in the following image.

4.

In the Number of nodes field, enter 2.

5.

Click create. HyperMesh creates two nodes that will be used to show the starting position of the thickness during future modifications.

6.

To exit the panel, click return.

7.

In the Model browser, Parameter folder, click Dimension1.

8.

In the Entity Editor, Double value field, change the value from 0.5 to 1.0. The part's thickness increases equally about the midpoint between the original locations.

9.

Undo the change by clicking

Proprietary Information of Altair Engineering

from the Undo/Redo toolbar.

Altair HyperMesh 2019 Tutorials

10. Select the handle at the bottom of the dimension manipulator as indicated in the following image. The bottom arrow changes to a line, which indicates that the bottom end will remain fixed.

11. Change the dimension value again from 0.5 to 1.0. The bottom end stays fixed.

12. Undo the dimension change. 13. The dimension manipulator can also be locked from the Entity Editor. •

In the Model browser, Feature folder, click Dimension1.

•

In the Entity Editor, set Lock Side to Point1.

The top arrow of he dimension manipulator changes to a line, which indicates that the top end will remain fixed. The bottom end changes to an arrow, as only one end can remain fixed.

Proprietary Information of Altair Engineering

p.137

Altair HyperMesh 2019 Tutorials

14. Change the dimension value again from 0.5 to 1.0. The top end stays fixed.

15. Undo the dimension change.

Step 5: Create and modify the diameter dimensions on the holes. 1.

In the Model browser, Feature folder, click Dimension2.

2.

Click the dimension manipulator and change the dimension value from 0.875 to .25. The hole's diameter decreases.

Proprietary Information of Altair Engineering

p.138

Altair HyperMesh 2019 Tutorials

3.

Change the dimension value again from 0.25 to .5. The hole's diameter increases.

4.

In the Model browser, Feature folder, click Dimension3.

5.

Change the dimension value from 0.75 to 1.0. The hole's diameter increases.

6.

Undo the dimension change.

Step 6: Delete a manipulator. 1.

In the Model browser, Parameter folder, click Dimension3.

2.

In the Entity Editor: •

Set Parameter type to double expression.

•

For Expression value, enter 2*Dimension2.

This expression indicates that Dimension3 is two times the value of Dimension2. The hole's diameter is updated to 1.0, which is twice the size of the first hole's diameter. The dimension manipulator displays the full expression as &Dimension3=2*Dimension2.

3.

In the Model browser, Parameter folder, click Dimension2.

Proprietary Information of Altair Engineering

p.139

Altair HyperMesh 2019 Tutorials

4.

p.140

In the Entity Editor, Double value field, change the dimension to 0.25. The first hole's diameter decreases from 0.5 to 0.25, and the second hole's diameter becomes 0.25*2=0.5.

Step 7: Parametrize and Unparametrize the dimension. 1.

In the Model browser, Feature folder, click Dimension3.

2.

In the Entity Editor, right-click on the Value field and select Unparameterize from the context menu. Dimension3 becomes unparametrized, and its corresponding dimension manipulator displays the current value of the dimension feature, instead of the parameter. All changes can now be made directly to Dimension3.

3.

In the Entity Editor, Value field, change the dimension value from 0.5 to 0.25.

4.

Right-click on the Value field and select Select Parameter/Parameterize from the context menu.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

5.

In the Select Parameter dialog, select Dimension3 and click OK. The hole updates with the Dimension3 parameter and displays the full expression in the dimension manipulator.

Step 8: Delete a manipulator. 1.

In the Model browser, Feature folder, right-click on Dimension3 and select Delete from the context menu. The feature Dimension3 and the parameter Dimension3 are deleted from the model.

Step 9: Mesh the part. 1.

Open the 2D AutoMesh panel by clicking Mesh > Create > 2D AutoMesh from the menu bar, or by pressing F12.

2.

In the element size field, enter 0.1

3.

Click surfs >> displayed.

4.

Set the toggle from interactive to automatic.

5.

Click mesh. HyperMesh meshes the part.

6.

Exit the panel by clicking return.

Proprietary Information of Altair Engineering

p.141

Altair HyperMesh 2019 Tutorials

Step 8: Modify the dimensions with automatic remeshing enabled. 1.

Open the Options panel by pressing O.

2.

Go to the mesh subpanel.

3.

From the topology revision list, select advanced remesh.

4.

Exit the panel.

5.

In the Model browser, Parameter folder, click Dimension1.

6.

In the Entity Editor, Double value field, change the value from 0.5 to 1.0.

7.

In the Model browser, Parameter folder, click Dimension2.

8.

In the Entity Editor, Double value field, change the value from 0.25 to 0.5. The part is remeshed due to the increase in the hole's diameter.

Proprietary Information of Altair Engineering

p.142

Altair HyperMesh 2019 Tutorials

Meshing

Proprietary Information of Altair Engineering

p.143

3

Altair HyperMesh 2019 Tutorials

p.144

HM-3000: Creating 1-D Elements In this tutorial, you will learn how to build 1D elements.

Model Files This exercise uses the 1d_elements.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Creating 1-D Elements

Step 1: Retrieve the model file. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the 1d_elements.hm model file.

Step 2: Create 1-D bar elements. 1.

Open the Bars panel by clicking Mesh > Create > 1D Elements > Bars from the menu bar.

2.

Go to the bar2 subpanel.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

In the ax, ay, and az fields, enter 0. These are the values for the bar offset.

4.

Click property = and select property1. HyperMesh assigns a property to the element.

5.

In the pins a and pins b fields, enter 0. These are the values for the degrees of freedom.

6.

Click the orientation switch and select components.

7.

In the x comp, y comp, and z comp fields, enter 1. These values define the local yaxis.

8.

Activate the node A selector, and select the lower node indicated in the following image.

9.

With the node B selector now active, select the upper node indicated in the previous image. HyperMesh creates the two-noded bar element.

10. Exit the panel by clicking return.

Proprietary Information of Altair Engineering

p.145

Altair HyperMesh 2019 Tutorials

Step 3: Create 1-D elements along a line. 1.

Open the Line Mesh panel by clicking Mesh > Create > Line Mesh from the menu bar.

2.

Verify that the entity selector is set to lines.

3.

Select the line indicated in the following image.

4.

Verify that the toggle is set to segment is whole line.

5.

From the element config list, select rigid.

6.

Click mesh. The Density panel opens.

7.

Activate the set segment selector.

8.

In the elem density = field, enter 20.

9.

Click set all. HyperMesh creates rigids on the selected line.

10. Go back to the main menu by clicking return twice.

Proprietary Information of Altair Engineering

p.146

Altair HyperMesh 2019 Tutorials

Step 4: Create 1-D elements from the feature in the model. 1.

In the Model browser, turn off the display of all of the geometry in the model.

2.

Turn off the display of all of the elements in the model except for the elements in the feature_elements component.

3.

Open the Features panel by clicking Mesh > Check > Components > Features from the menu bar.

4.

Verify that the entity selector is set to comps.

5.

Click comps >> feature_elements.

6.

Click select.

7.

In the feature angle = field, enter 30.

8.

Select the ignore normals check box.

9.

Verify that the create toggle is set to plot elements.

10. Click features. HyperMesh creates the plot elements as green edge lines.

11.

Exit the panel by clicking return.

Proprietary Information of Altair Engineering

p.147

Altair HyperMesh 2019 Tutorials

HM-3100: AutoMeshing In this tutorial, you will: •

Learn how to mesh all of the surfaces at once, specifying different element sizes and element types

•

Practice changing the element density along surface edges

•

Practice checking element quality and changing the mesh pattern by changing the mesh algorithm

•

Learn how to preview the mesh on all the unmeshed surfaces

•

Practice changing the element type and node spacing (biasing) along surface edges

•

Learn how to remesh surfaces

The optimal starting point for creating a shell mesh for a part is to have geometry surfaces defining the part. The most efficient method for creating a mesh representing the part includes using the Automesh panel and creating a mesh directly on the part’s surfaces.

Model Files This exercise uses the channel.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Proprietary Information of Altair Engineering

p.148

Altair HyperMesh 2019 Tutorials

p.149

Exercise

Step 1: Open and view the model file, channel.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the channel.hm model file.

4.

Observe the model using the different visual options available in HyperMesh (rotation, zooming, etc.).

Step 2: Mesh all the part’s surfaces at once using an element size of 5 and the mixed element type (quads and trias). 1.

To open the AutoMesh panel, click Mesh > Create > 2D AutoMesh from the menu bar, or press F12.

2.

Go to the size and bias subpanel.

3.

Verify that the entity selector is set to surfs.

4.

Click surfs >> displayed.

5.

In the element size= field, enter 5.

6.

Set the mesh type: to mixed.

7.

Set the active mesh model to interactive.

8.

Set the first toggle to elems to current comp.

9.

Click mesh. HyperMesh opens the density subpanel in the meshing module. The model displays node node seeding and a number on each surface edge. Note:

The number displayed in the graphics area is the number of elements that were created along the edge.

10. To accept the mesh as the final mesh, click return. At this point, you could be done using the Mesh panel to mesh the part. The mesh quality is very good. However, you will remain in the meshing module to perform the next steps, which demonstrate how to use various subpanels to interactively control the creation of the mesh.

Step 3: Delete the mesh. 1.

To open the Delete panel, click

2.

Set the entity selector to elems.

3.

Click elems >> all.

4.

Click delete entity.

Proprietary Information of Altair Engineering

on the Collectors toolbar, or press F2.

Altair HyperMesh 2019 Tutorials

5.

p.150

To go back to the AutoMesh panel, click return.

Step 4: Mesh the surface having three fixed points interior to its surface. In this step, you should be in the AutoMesh panel, size and bias subpanel. 1.

Leave all options in the subpanel as they are.

2.

Select the surface that has three fixed points interior to its surface indicated in the following image.

3.

Click mesh. HyperMesh opens the meshing module.

4.

Preview the generated mesh.

Step 5: Fit only the surface being meshed to the graphics area. 1.

To fit the surface to the graphics area, click f or click local view >> fill in the density subpanel.

Step 6: From the graphics area, specify a new element density along surface edges. 1.

From the density subpanel, activate the adjust: edge selector.

2.

To change the element density number of the edge indicated in the following image from 24 to 48: •

Left-click on the edge’s element density number to increase it by one, or right-click on the element's density number to decrease it by one.

or

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

•

3.

Click and hold the mouse pointer on the edge’s element density number and drag your mouse up to increase the number or down to decrease the number.

Click mesh. HyperMesh updates the preview mesh based on the change.

Proprietary Information of Altair Engineering

p.151

Altair HyperMesh 2019 Tutorials

Step 7: From the density subpanel, specify a new element density along surface edges. In this step, you should still be in the density subpanel. 1.

In the elem density= field, enter 10.

2.

Activate the set: edge selector.

3.

Select the element density number of the edge indicated in the following image to change its value to 10.

4.

Click mesh. HyperMesh updates the preview mesh based on the change.

5.

Click set all to. HyperMesh changes all of the edge's densities to 10.

6.

Click mesh. HyperMesh updates the preview mesh based on the change.

Proprietary Information of Altair Engineering

p.152

Altair HyperMesh 2019 Tutorials

Step 8: From the density subpanel, specify a new element size to adjust element densities along surface edges. 1.

In this step, you should still be in the density subpanel.

2.

In the elem size= field, enter 7.

3.

Activate the calculate: edge selector.

4.

Select the element density number of the edge indicated in the following image to calculate it based on an element size of 7. HyperMesh calculates the new number to create elements as close as possible to 7.

5.

Click mesh. HyperMesh updates the preview mesh based on the change.

6.

Click recalc all. HyperMesh calculates and changes all of the edge's densities based on an element size of 7.

Proprietary Information of Altair Engineering

p.153

Altair HyperMesh 2019 Tutorials

7.

Click mesh. HyperMesh updates the preview mesh based on the change.

Step 9: Change all edge element densities to reflect the initial element size of 5. 1.

In the elem size= field, enter 5.

2.

Click recalc all.

3.

Click mesh. HyperMesh updates the preview mesh based on the change.

4.

To accept the mesh and go back to the size and bias subpanel, click return.

Step 10: Preview a mesh of the channel’s rib. In this step, you should still be in the Mesh panel, size and bias subpanel. 1.

With the entity selector active and set to surfs, select the rib surface in the middle of the part as indicated in the following image.

Proprietary Information of Altair Engineering

p.154

Altair HyperMesh 2019 Tutorials

2.

Leave all options in the menu panel set as they are.

3.

Click mesh. HyperMesh opens the meshing module and generates the preview mesh.

4.

To fit the rib's surface to the graphics area, click local view >> rear.

Step 11: Check the quality of the rib’s preview mesh. 1.

Go to the checks subpanel.

2.

To identify all of the elements that have an aspect ratio greater than 5, click aspect. None of the elements fail the check, and the status bar reads, "Maximum aspect ratio found is equal to 1.75".

3.

In the jacobian < field, enter 0.8.

4.

To identify all of the elements that have a jacobian less than 0.8, click jacobian. HyperMesh identifies several elements that fail the check and outlines them in red. The status bar reads, "Minimum jacobian found is equal to 0.75."

5.

Verify that none of the elements have a jacobian less than 0.7.

Proprietary Information of Altair Engineering

p.155

Altair HyperMesh 2019 Tutorials

6.

Under quads, enter 45 in the min. angle < field.

7.

Click min angle. The minimum interior angle found among all of the quad elements is 46.46.

8.

Under quads, enter 135 in the max. angle > field.

9.

Click max angle. The maximum interior angle found among all of the quad elements is 136.58.

Step 12: Change the rib’s mesh pattern by changing the mesh method used for its surface. 1.

Go to the mesh style subpanel. The edge's element density numbers have disappeared, and there is now a small icon interior to the rib's surface. This icon indicates that HyperMesh is currently using the free (unmapped) mesh method to mesh the surface.

2.

Under mesh method, use the switch to select map as rectangle.

3.

Under mesh method, click set all. The icon changes to reflect the new mesh method.

4.

Click mesh. HyperMesh updates the preview mesh based on the change.

Proprietary Information of Altair Engineering

p.156

Altair HyperMesh 2019 Tutorials

p.157

Step 13: Check the quality of the rib’s preview mesh again. 1.

Go the checks subpanel.

2.

Check for elements having an aspect ratio greater than 5. Highest value reported is _____.

3.

Check for elements having a jacobian less than 0.7. Lowest value reported is _____. In this case, the free (unmapped) mesh has a better jacobian than the map as rectangle mesh.

4.

Check for quad elements having a min angle less than 45. Smallest value reported is _____.

5.

Check for quad elements having a max angle greater than 135. Highest value reported is _____.

Step 14: Change the rib’s mesh method back to free (unmapped). 1.

Go to the mesh style subpanel.

2.

Under mesh method, use the switch to select free (unmapped).

3.

Under mesh method, click set all.

4.

Click mesh. HyperMesh updates the preview mesh based on the change.

5.

To accept the mesh as final and go back to the Mesh panel, click return.

Step 15: Preview a mesh of all displayed, unmeshed surfaces. In this step, you should still be in the Mesh panel, size and bias subpanel. 1.

On the standard toolbar, click

2.

Accept all the default values.

3.

Click failed. The status bar reads "There are no surfaces with meshing errors". Note:

.

This is correct; all of the surfaces you selected to mesh so far have a mesh on them.

4.

To identify and select all of the displayed, unmeshed surfaces, click unmeshed.

5.

Click mesh. HyperMesh opens the meshing module and generates the preview mesh.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.158

Step 16: Change the element type for some surfaces to trias. 1.

Go to the mesh style subpanel.

2.

Under elem type, click toggle surf. HyperMesh displays interior to each surface, which indicates that the mixed element type (quads and trias) is currently being used to mesh the surface.

3.

Under elem type, use the switch to change the mesh type to trias.

4.

Under elem type, activate the set surf selector.

5.

On the two surfaces indicated in the following image, left-click on element type to trias ( ).

6.

Click mesh. HyperMesh updates the preview mesh based on the change.

, to set their

Preview of mesh with tria element type for two surfaces

Step 17: Adjust the node spacing on surface edge (biasing). 1.

Go to the biasing subpanel. The bias intensity number on each surface edge is 0.000, which is the default number.

2.

Leave the bias style set to linear. Note:

3.

This style corresponds to the positive slope of a straight line over the interval [0,1] of the real line. For a positive bias intensity, smaller elements are at the start of the edge.

Verify that the adjust: edge selector is active.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

p.159

To change the biasing intensity number of the edge indicated in the following image from 0.0 to 3.0: •

Left-click on the edge’s biasing intensity number to increase it by 0.1, or right-click on the edge's biasing intensity number to decrease it by 0.1.

or •

Click and hold the mouse pointer on the edge’s biasing intensity number and drag your mouse up to increase the number or down to decrease the number.

5.

Click mesh. HyperMesh updates the preview mesh based on the change.

6.

In the intensity= field, enter 10.

7.

Activate the calculate: edge selector.

8.

Click the same edge’s biasing intensity number to change it to 10.

9.

Click mesh. HyperMesh updates the preview mesh based on the change.

10. Set the bias style to bellcurve. This bias style distributes nodes along the edge in a pattern that is symmetric across the midpoint of the edge. Note:

For a positive biasing intensity, the smaller elements are at the start and end of the edge.

11. Activate the set: edge selector. 12. On the same edge, click bias style.

to change it from the linear bias style to the bellcurve (

13. Click mesh. HyperMesh updates the preview mesh based on the change. 14. To accept the final mesh and go back to the Mesh panel, click return.

Proprietary Information of Altair Engineering

)

Altair HyperMesh 2019 Tutorials

Step 18: Remesh the channel’s bottom two surfaces. In this step, should still be in the Mesh panel, size and bias subpanel. 1.

Switch the mesh mode from interactive to automatic. Note:

This mode is not interactive, therefore it does not take you to the meshing module. Rather, it meshes surfaces using only the basic parameters of the AutoMesh panel. Use Interactive mode to remesh the surfaces if you require the different options to control the created mesh.

2.

Verify that the entity selector is active and set to surfs.

3.

Select the two surfaces indicated in the following image.

4.

In the element size = field, enter 10.

5.

Click mesh. HyperMesh deletes the existing mesh on the selected surfaces and creates a new mesh. Observe the resulting quad mesh on the remeshed surfaces.

6.

Note: 7.

Connectivity was maintained with the surrounding, smaller mesh. This is because the break connectivity option was not used.

To exit the panel, click return.

Step 19 (Optional): Save your work. Meshing of the channel part is complete. Now is a good time to save the model. 1.

From the menu bar, click File > Save > Model.

Proprietary Information of Altair Engineering

p.160

Altair HyperMesh 2019 Tutorials

HM-3110: Meshing without Surfaces In this tutorial, you will learn about: •

The basic concepts of surfaceless meshing and how to mesh a bracket.

•

Scale (Uniform scaling)

•

2D mesh by using spline, line drag, and skin

•

Ruled mesh

Surfaceless meshing is defined as the creation of mesh using points, lines, and nodes rather than surfaces. Some parts may have missing surfaces and some parts may not have any surfaces at all and are instead defined by line data. Either way, a mesh still must be created. HyperMesh has a number of panels that you can use to create a mesh based on geometry rather than surfaces.

Model Files This exercise uses the bracket.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory. The model consists of only line data; no surfaces are present.

Proprietary Information of Altair Engineering

p.161

Altair HyperMesh 2019 Tutorials

p.162

Exercise: Meshing a Bracket

Step 1: Retrieve and view the model file. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the bracket.hm model file.

4.

Observe the model using the different visual options available in HyperMesh (rotation, zooming, etc.).

Step 2: Create a concentric circle around a hole on the top face using the scale panel. There are three circles on the upper region of the bracket, which represent three holes in the bracket. Two of the holes have concentric circles around them. This configuration allows you to create a radial mesh pattern around the holes. The following steps will show you how to create a concentric circle around the third hole. 1.

To open the Scale panel, click Geometry > Scale > Lines from the menu bar, or select Scale from the Tool page.

2.

Click uniform and enter 2.0 in the scale= field.

3.

To open the Distance panel, press F4.

4.

Go to the three nodes subpanel.

5.

Verify that the N1 node selector is active.

6.

Press and hold your left mouse button, move it over the circle representing the hole as indicated in the following image, and then release it when the cursor changes to a square with a dot in the center

Proprietary Information of Altair Engineering

.

HyperMesh highlights the circle.

Altair HyperMesh 2019 Tutorials

7.

Left-click on the highlighted circle. HyperMesh creates a node for N1.

8.

Left-click twice more at different locations on the circle to create nodes N2 and N3.

9.

Click circle center. Hypermesh creates a node at the circle's center. Note:

This node will be selected as the origin node when the circle is duplicated and scaled.

10. To go back to the Scale panel, click return. 11. Set the entity selector to lines. 12. Select the circle with the node in its center. 13. Click lines >> duplicate >> original comp. 14. Activate the origin: node selector. 15. Select the temporary node you created in the circle’s center. 16. Click scale +. HyperMesh creates a new circle, which is concentric with the original.

Proprietary Information of Altair Engineering

p.163

Altair HyperMesh 2019 Tutorials

17. To exit the panel, click return.

Step 3: Create a radial mesh between each of the concentric circles using the spline panel. 1.

To open the Spline panel, click Mesh > Create > 2D Elements > Spline from the menu bar, or select Spline from the 2D page.

2.

Verify that the entity selector is set to lines.

3.

Select all six circular lines.

4.

Switch from mesh, keep surf to mesh, dele surf. Note:

This option creates surfaces based on the selected entities, uses the surfaces to create a mesh, and then deletes the surfaces.

5.

Clear the keep tangency check box.

6.

Click create. The meshing module opens, and element edge density numbers appear on the selected lines. Note:

The numbers on a pair of concentric circular lines must be identical in order to achieve a radial mesh.

7.

In the density subpanel, enter 8 in the elem density= field.

8.

Click set all to. HyperMesh changes all of the circular line's element edge densities to 8.

Proprietary Information of Altair Engineering

p.164

Altair HyperMesh 2019 Tutorials

9.

Click mesh. HyperMesh updates the preview mesh based on the change.

10. To accept the mesh and go back to the Spline panel, click return.

Step 4: Mesh the rest of the top face using the spline panel. 1.

With the entity type set to lines, select the four lines defining the perimeter of the top face and the three circular lines defining the outside perimeter of the three radial meshes.

2. 3.

Click create. The meshing module opens. To accept the mesh and go back to the main menu, click return twice.

Final mesh on the top face of the bracket

Proprietary Information of Altair Engineering

p.165

Altair HyperMesh 2019 Tutorials

Step 5: Mesh the back face of the bracket using the line drag panel. 1.

To open the Line Drag panel, click Mesh > Create > 2D Elements > Line Drag from the menu bar, or click Line Drag from the 2D page.

2.

Go to the drag geoms subpanel.

3.

Set the drag selector to line list.

4.

Select the line that is on the perimeter of the existing mesh and adjacent to the bracket’s back face as indicated in the following image.

5. 6.

Activate the along: line list selector. Select one of the two lines defining the back face that are perpendicular to the selected line to drag as indicated in the following image.

Proprietary Information of Altair Engineering

p.166

Altair HyperMesh 2019 Tutorials

7.

Leave the toggle set to use default vector.

8.

Leave the creation method set to mesh, w/o surf.

9.

Click drag. The meshing module opens.

10. To accept the mesh and return to the main menu, click return twice.

Mesh of top and back faces

Step 6: Mesh the bottom face of the bracket using the ruled panel. 1.

To open the Ruled panel, click Mesh > Create > 2D Elements > Ruled from the menu bar, or select Ruled from the 2D page.

2.

Verify that the top entity selector is set to node list.

3.

Click node list >> by path. The entity selector changes to node path.

4.

Select the end nodes located on the back face edge that borders the bottom face, as indicated in the following image. HyperMesh selects all of the nodes between the two selected nodes.

Proprietary Information of Altair Engineering

p.167

Altair HyperMesh 2019 Tutorials

5.

Click node path >> show node order. HyperMesh highlights and numbers the nodes to show the order in which they have been selected.

6.

Set the bottom entity selector to line list.

7.

Select the line defining the opposite edge of the bottom face as indicated in the following image.

8.

Switch the creation method from mesh, keep surf to mesh, w/o surf.

9.

Select the auto reverse check box. Note:

When elements are generated, the edges used to create them can be ordered in different directions. The order of the edges is determined by the order in which the nodes are selected or the direction of the selected line(s). If the direction is different for each selection, then a mesh that crosses itself, similar to a bow tie, will be created. To prevent this, the auto reverse option ensures elements are generated with a similar order on each side of the mesh.

10. Click create. The meshing module opens. 11. To accept the mesh and return to the main menu, click return twice.

Mesh of top, back, and bottom faces of bracket

Proprietary Information of Altair Engineering

p.168

Altair HyperMesh 2019 Tutorials

Step 7: Mesh the rib using the skin panel. 1.

To open the Skin panel, click Mesh > Create > 2D Elements > Skin from the menu bar, or select Skin from the 2D page.

2.

With the line list selector active, select any two of the three lines defining the rib.

3.

Switch the creation method from mesh, keep surf to mesh, dele surf.

4.

Leave the toggle set to auto reverse.

5.

Click create. The meshing module opens.

6.

To accept the mesh and return to the main menu, click return twice.

Mesh of rib

Proprietary Information of Altair Engineering

p.169

Altair HyperMesh 2019 Tutorials

p.170

HM-3120: 2-D Mesh in Curved Surfaces In this tutorial, you will learn how to: •

Create a mesh based only on element size

•

Mesh a set of surfaces using the maximum deviation parameter

•

Reduce the maximum angle perimeter

•

Increase the maximum element size parameter

Chordal deviation is a meshing algorithm that allows HyperMesh to automatically vary node densities and biasing along curved surface edges to gain a more accurate representation of the surface being meshed.

Model Files This exercise uses the chordal_dev.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Controlling the 2-D Mesh Concentration in Curved Areas

Step 1: Open the model file, chordal_dev.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the chordal_dev.hm model file.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

Observe the model using the different visual options available in HyperMesh (rotation, zooming, etc.).

Step 2: Set the mesh parameters and create the mesh. In this step, you will create a mesh using only element size, not the chordal deviation meshing parameters. 1.

To open the Mesh panel, click Mesh > Create > 2D AutoMesh from the menu bar, or select automesh from the 2D page.

2.

Toggle the mesh mode from interactive to automatic.

3.

In the element size = field, enter 15.000.

4.

Set the mesh type to quads.

5.

Set the toggle to elems to surf comp.

6.

Select surfs >> by collector >> use size.

7.

Click select.

8.

Click mesh. HyperMesh creates the mesh.

View of the completed mesh for this step.

Step 3: Set the chordal deviation parameters and create the mesh. In this step, you will mesh a set of surfaces using the maximum deviation parameter to control the element densities and biasing. 1.

Go to the edge deviation subpanel.

2.

In the min elem size = field, enter 1.000. Tip:

To cycle through the parameter settings, press TAB after typing in a value.

Proprietary Information of Altair Engineering

p.171

Altair HyperMesh 2019 Tutorials

3.

In the max elem size = field, enter 15.000.

4.

In the max deviation = field, enter 0.500.

5.

In the max angle = field, enter 90.000 for the maximum angle parameter to be neglected.

6.

Set the mesh type to quads.

7.

Select surfs >> by collector >> deviation ctrl.

8.

Click select.

9.

Click mesh. HyperMesh create the mesh.

View of the completed mesh for this step.

Step 4: Set the chordal deviation parameters and create the mesh. In this step, you will use the same chordal deviation settings from the previous step, but reduce the maximum angle parameter to compare the effects. 1.

In the max angle = field, enter 20.000.

2.

Select surfs >> by collector >> angle ctrl.

3.

Click select.

Proprietary Information of Altair Engineering

p.172

Altair HyperMesh 2019 Tutorials

4.

Click mesh. HyperMesh creates the mesh on the surfaces.

View of the completed mesh for this step.

Step 5: Set the chordal deviation parameters and create the mesh. In this step, you will use the same chordal deviation parameters from the previous step except for the maximum element size parameter. The maximum element size parameter is increased to allow the algorithm to create larger and fewer elements along planer and less curved surface edges. 1.

In the max elem size = field, enter 30.000.

2.

Select surfs >> by collector >> max size ctrl.

3.

Click select.

4.

Click mesh. HyperMesh creates the mesh.

View of the completed mesh for this exercise.

Proprietary Information of Altair Engineering

p.173

Altair HyperMesh 2019 Tutorials

p.174

HM-3130: QI Mesh Creation In this tutorial, you will learn how to create and optimize a 2D mesh based on user-defined quality criteria. HyperMesh has a set of features designed to help you achieve good element quality more efficiently. These features use settings from the qualityindex panel to generate or modify a mesh. This allows HyperMesh to give results that account for your preferences for which element quality checks are more or less important than others. The quality index (Q.I.) optimization features are found in the Automesh, Smooth, and Qualityindex panels. You can use these functions separately or in unison.

Model Files This exercise uses the planar.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise 1: Creating and Optimizing a 2D Mesh Based on UserDefined Quality Criteria

Step 1: Open the model file, planar.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the planar.hm model file.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

p.175

Observe the model using the different visual options available in HyperMesh (rotation, zooming, and so on).

Step 2: Working with node and element quality optimization. Within the qualityindex panel, there are tools you can use to select individual nodes or elements, and then alter the position or shape of the node/element to optimize the element quality for the surrounding elements. The element qualities are optimized according to the settings in the qualityindex panel. These features are very useful for improving element qualities in local areas of the mesh. 1.

Open the qualityindex panel by clicking Mesh > Check > Elements > Quality Index from the menu bar, or selecting qualityindex from the 2D page.

2.

On the right-hand side of the panel, note the value for comp. Q.I.=. It should read 85.09. Tip:

Keep this number in mind so that you can judge how much progress you make in improving the element quality.

3.

Click cleanup tools. The QI criteria is replaced by a series of yellow buttons, each representing a tool for element cleanup.

4.

Experiment with the modify hole and washers tool. •

Use these options on the hole in the mesh to reposition nodes on the hole's edges, change the radius of the holes, and link holes with their washers so that the washers rotate or resize along with changes made to the holes. radial

Use this option to alter the radius of a hole (and, optionally, the washer). To alter the radius of the hole, click and drag a node in the graphics area. The element orientation remains constant, but the hole may become larger or smaller based on the input. There are additional controls to enable or disable automatic remeshing when altering the hole dimensions.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.176

radius: (and This field displays the current radius of the hole that the edit check box) selected node belongs to. By default it is a display-only field. If you do not want to click and drag a node in the graphics area, you can select the edit check box and specify a desired radius. Once you click a node in the desired hole, the radius will change to the specified value. angular

Use this option to move the nodes around the edges of the hole without changing the hole diameter or the spacing between nodes.

angle: (and This field displays the current angle of the hole that the edit check box) selected node belongs to, relative to its original (unmodified) starting position. By default it is a a display-only field. If you do not want to click and drag a node in the graphics area, you can select the edit check box and specify a desired angle. Once you click a node in the desired hole, the angle will change to the specified value.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.177

radial & angular

Use this option to simultaneously change the hole's radius and the orientation of nodes around its edge. Like the angular option, the node spacing remains proportionally consistent, though actual spacing will be scaled in accordance with changes in the hole radius.

radial and angular: (and edit check boxes)

These fields display the current angle and radius of the hole that the selected node belongs to. By default they are both a display-only field. If you do not want to click and drag a node in the graphics area, you can select both edit check boxes and specify a desired angle and radius. Once you click a node in the desired hole, the angle and radius will simultaneously change to the specified values.

circumferential Used primarily on openings like slots, this option rotates the nodes along the circumference of the slot without altering the hole's size or shape/orientation. The capability works on enclosed slots or holes, it is not designed to work on slots with an opening.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.178

circumferential This field displays the current arc length of the hole that the (and edit check selected node belongs to. By default it is a display-only field. box) If you do not want to click and drag a node in the graphics area, you can select the edit check box and specify a desired arc length. Once you click a node in the desired hole, the arc length will change to the specified value. link washers

To change the radial or angular position of nodes, as well as drag and scale the washer nodes along with them, select this check box. In order for the link washers option to work, you must select the allow to move fixed and shared nodes check box in page 3 of the quality index panel.

Starting point (no changes Link Washers option made yet) turned off.

remesh number of layers: 5.

Link Washers option turned on.

To specify the number of washer layers to automatically remesh after you alter the node position, select this check box.

Experiment with the place node tool. •

Use the following place node options to reposition some of the nodes in the mesh and change the shape of the surrounding elements. To reposition a node in the mesh, click and drag it.

•

The affected elements will change color as you reposition the node to indicate their quality grade at the node's current position. Observe how the comp. Q.I. changes. along surface / normal to surface

Use this toggle to determine which direction the node will move. To move the node along the plane or curvature of the surface, select along surface. To move the node directly away from the surface in a normal direction, select normal to surface.

Movement along surface; note that the node cannot normally exceed the edge of the mesh.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.179

Movement normal to surface

With the place node tool highlighted, click-and-drag a node in the graphics area to relocate it. The elements that depend on that node will dynamically adjust as you drag, resulting in a QI change. allow movement out of boundary

To move the nodes past the edges of a mesh boundary, select this check box. This option is only available when along surface is selected.

Movement along surface, allowing movement out of boundary.

move midnodes 6.

To move the midnodes associated with the node you are moving, select this check box. This option is useful when you are working with second order elements.

Experiment with the swap edge tool. Use the Swap Edge tool to consider the elements to which the edge belongs, and find alternative orientations for it.

Each time you click an edge in the graphics area, it switches to the next valid configuration. If an edge swap will not improve element quality, a message to that effect displays in the status bar. To force the swap anyways, click the edge a second time. Additional clicks will cycle through the possible edge positions. The number of possible edge positions depends on the types of elements involved. For a pair of trias, there are two possible positions for their shared edge. For a pair of quads, there are three possible positions. For a quad and a tria, there are six possible positions.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

7.

8.

9.

Experiment with the node optimize tool. •

Use the Node Optimize tool to automatically move a selected node to optimize the overall quality of its surrounding elements. The options along surface, normal to surface, and along and normal to surface work exactly as described for the place node tool. The only difference is that node optimize moves the node automatically, while place node requires you to choose the location manually.

•

To move the midnodes attached to the node you are optimizing, select the with attached midnodes check box. This option is useful when you are working with second order elements.

•

Try selecting some of the nodes on the mesh. In particular, select nodes of elements that are highlighted red, since these have the worst quality. You should see each node move as it is selected, improving the surrounding mesh quality. Notice what happens to the value of the comp. Q.I., it should improve as you select more nodes.

Experiment with the element optimize tool. •

Use the Element Optimize tool to automatically optimize the shape of the selected element and the elements surrounding it. It is similar to Node Optimize, except that its effects are wider-spread.

•

To move the midnodes attached to the element you are optimizing, select the with attached midnodes check box. This option is useful when you are working with second order elements.

•

Try selecting some of the elements on the mesh. In particular, select elements that are highlighted red, since these have the worst quality. You should usually see the shape of the element change as it is selected, improving the surrounding mesh quality. Notice what happens to the value of the comp. Q.I. , it should improve as you select more elements.

To exit the panel, click return.

Step 3: Resetting the part by remeshing. In this step, you will use the AutoMesh panel to regenerate the original mesh so you can try to fix the element quality using a different method. 1.

To open the Automesh panel, click Mesh > Create > 2D AutoMesh from the menu bar, or select Automesh from the 2D page.

2.

Go to the size and bias subpanel.

3.

Verify that the entity selector is active and set to surfs.

4.

Select surfs >> all.

5.

In the element size= field, enter 15.

6.

Set the mesh type to quads.

7.

Set the meshing mode to automatic.

Proprietary Information of Altair Engineering

p.180

Altair HyperMesh 2019 Tutorials

p.181

8.

Switch the connectivity option from keep connectivity to previous settings.

9.

Click mesh. HyperMesh regenerates the mesh.

10. To exit the panel, click return.

Step 4: Using QI optimization smoothing. The Smooth panel also has quality index optimization features. In this step, you will use these features to adjust the element quality according to the settings in the qualityindex panel for an entire group of selected elements. Once you have adjusted the element quality, you will compare the smooth function to the node and element optimization used in the step 2. 1.

To open the Smooth panel, click Mesh > Cleanup Elements > Smooth from the menu bar, or select smooth from the 2D page.

2.

Go to the plates subpanel.

3.

Select smooth: elems >> displayed.

4.

Switch the mesh algorithm from autodecide to QI optimization.

5.

There are several optional controls that are enabled when you select QI optimization, that you should understand, but are not needed for this tutorial: Controls

Function

target quality index=

The target value you would like the quality index to be after the smoothing operation. This value is not guaranteed from smoothing. The smooth operation will attempt to hit this target.

time limit

If you are working with large models, select this check box to ensure the smoothing routine does not take more time than you want to allow.

feature angle

The Smooth panel evaluates the angle between the normals of two adjacent elements. If this angle is equal to or greater than the value specified in this field, HyperMesh will not allow the nodes shared by the elements to move.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

use current criteria / criteria file

p.182

If use current criteria file is selected, HyperMesh will use the current criteria file for your Q.I. settings. If criteria file is selected, you can select and use a different criteria file for your Q.I. settings. If a criteria file is specified, leave this option blank.

recursive optimization procedure / single optimization step

If recursive optimization procedure is selected, the automesher takes more than one pass in generating the best quality mesh it can. This option make take longer than single optimization step. If single optimization step is selected, the automesher will only take one pass in generating the best quality mesh it can. It is suggested that you use this option for larger models.

6.

Click smooth. The status bar displays a message that says “result selection approximate quality index = 0.11”

7.

Compare this value to 85.10, which is the quality index value you had after creating the original mesh. In this case you should see that it is significantly lower, which indicates that the element quality is much better.

8.

To exit the panel, click return.

Step 5: Using the QI settings in the Mesh panel. The AutoMesh panel is capable of using the quality index settings to automatically decide what pattern of mesh it should generate. 1.

Open the AutoMesh panel.

2.

Go to the batchmesh/QI optimize subpanel.

3.

Set the toggle to QI optimize.

4.

Verify that the entity selector is set to surfs.

5.

Select surfs >> all.

6.

In the elem size= field, enter 18.

7.

Set the mesh type to quads.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

8.

p.183

The QI optimize subpanel has several controls that you should understand, but are not needed for this tutorial Controls

Function

use current criteria If use current criteria file is selected, HyperMesh will in QI panel use the current criteria file for your Q.I. settings. If criteria file is selected, you can select and use a different criteria file for your Q.I. settings. If a criteria file is specified, leave this option blank. Smooth across common edges

Select this check box if you would like the nodes generated on a surface edge to be moved off the surface edge when the algorithm smoothes the mesh.

feature angle

The QI optimize subpanel evaluates the angle between the normals of two adjacent elements. If this angle is equal to or greater than the value specified in this field, HyperMesh will not allow the nodes shared by the elements to move.

Keep/ Redo / Break connectivity

Keep Connectivity creates a new mesh with node seeding at its edges to match any existing adjacent meshes. Redo Connectivity redoes existing adjacent meshes at the same time as it meshes the current selection, to ensure that each surface's mesh matches up along the shared edges. Break connectivity allows the Mesher to mesh without affecting surrounding mesh.

9.

Click mesh. HyperMesh regenerates the mesh.

10. To exit the panel, click return. 11. Use the qualityindex panel to check the quality index of this mesh, and compare it to the previous mesh. 12. Look at the value for the comp. Q.I.= field. It should be 0.12, which is much lower that the 85.10 value of the mesh you originally generated.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.184

HM-3140: Batch Meshing In this tutorial, you will learn how to: •

Define a configuration for the batch mesh

•

Edit the criteria and parameter files

•

Setup a simple user procedure for a post-batch mesh run

Batch Mesher is a tool that can perform geometry cleanup and automeshing (in batch mode) for given CAD files. Batch Mesher performs a variety of geometry cleanup operations to improve the quality of the mesh created for the selected element size and type. Cleanup operations include: equivalencing of "red" free edges, fixing small surfaces (relative to the element size), and detecting features. Batch Mesher also performs specified surface editing/defeaturing operations such as: removal of pinholes (less than specified size), removal of edge fillets, and addition of a layer of washer elements around holes. All user-defined criteria determines the quality index (QI) of a model. The QI value is used to assess the potential of each geometry cleanup and meshing tool, and apply them accordingly. QI optimized meshing and node placement optimization are performed to obtain the best quality meshing. Final results are stored in a HyperMesh database file.

Tools To start Batch Mesher on Windows: •

Click on the Start menu > All Programs > Altair HyperWorks > BatchMesher.

Or •

Type hw_batchmesh with the full path (~altairhome\hm\batchmesh\hw_batchmesh).

To start Batch Mesher on UNIX: •

Type the hw_batchmesh command to invoke the user interface or hw_batchmesh nogui… to perform the batch mesh without a user interface.

Model Files This exercise uses the following files found in the hm.zip file. Copy the file(s) from this directory to your working directory. •

part1.hm

•

part2.hm

•

bm_housing.hm

•

bm_housing.criteria

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

•

bm_housing.param

•

bm_housing.tcl

p.185

Exercise

Step 1: Open BatchMesher. 1.

Start BatchMesher as described above.

2.

In the Input model directory field, click Note:

and navigate to your working directory.

In this exercise, you will use files located in the hm.zip file.

3.

In the Output directory, click from the Input model directory.

4.

Optional: Move all of the .hm output files to the corresponding directory of the input model by selecting the Relocate .hm files to input model directory checkbox.

5.

On the right-hand side of BatchMesher, click appears.

6.

From the Type of Geometry list, select the appropriate CAD data type. For this tutorial, use the geometry already loaded in HyperMesh, therefore select HyperMesh. Note:

and navigate to the appropriate directory if different

. The Select Model Files dialog

A filter will help select applicable HyperMesh models for batch meshing.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

7.

Select the following model files: part1.hm, part2.hm and bm_housing.hm. Tip:

8.

p.186

Select multiple files by pressing CTRL while selecting files.

Click Select.

Step 2: Define a configuration for the batch mesh run. 1.

Click the Configurations tab. BatchMesh displays several common configurations already available.

2.

On the right-hand side of BatchMesher, click table of configurations.

3.

Double-click the Mesh Type field, and then enter a name for the mesh type.

4.

Double-click the Criteria File field, and then click

5.

In the Select Criteria File dialog, select the bm_housing.criteria file.

6.

Double-click the Parameter File field, and then click

7.

In the Select Parameter File field, select the bm_housing.param file.

8.

Click the Run Setup tab.

9.

Click the Mesh Type field. The new mesh type you created is now available for selection.

. BatchMesher adds a new entry to the

.

.

Step 3: On the User Procedures tab, set up a simple script to perform a tetramesh on the housing. 1.

Click the User Procedures tab.

2.

On the right-hand side of BatchMesher, click table of user procedures.

Proprietary Information of Altair Engineering

. BatchMesher adds a new entry to the

Altair HyperMesh 2019 Tutorials

p.187

3.

Double-click the TCL File field, and then click

.

4.

In the Select Tcl File dialog, select the bm_housing.tcl file.

5.

Click the TCL Procedure field, and then select tet_all from the list of procedures.

6.

Double-click the Name field, and then enter a name for the procedure. For example, tetmesh.

7.

Click the Run Setup tab.

8.

Click the Post-Mesh field. The new post-batch meshing script you created in now available for selection.

Step 4: On the Run Setup tab, begin defining a configuration for the batch mesh run. 1.

2.

For each geometry file, click the Mesh Type field and select the predefined mesh types as follows: •

bm_housing.hm: use the mesh type you defined in Step 2.

•

part1.hm: use Crash 5mm.

•

part2.hm: use Crash 5mm.

For the Geometry file bm_housing.hm, click the Post-Mesh field and select the procedure you created in Step 3. Note:

This will run the tetramesher on all available shell elements after batch meshing.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

Click Submit to initiate the run, or click Submit At to submit the job at a specified time. BatchMesher switches to the Run Status tab. As the three jobs run, the Status changes from Working to Pending to Done.

4.

Obtain more details on a single job when its status is Working by selecting the job and then clicking Show Details. A detailed summary appears with a table containing information about the model during each step of the batch meshing process, such as the number of failed elements and the quality index.

5.

Once a job's status is Done, click Load Mesh. BatchMesher loads the mesh into HyperMesh for model interrogation.

6.

Obtain an overall run status of all the jobs by clicking Run Details once all of the jobs have been meshed.

7.

While the jobs are running, you can pause or cancel them. If you pause a job, it can be resumed immediately or you can have it resume at a specific time.

8.

Once the BatchMesher session has been setup with file directories and mesh types, you can save it as a config file and load it at a future time.

9.

It is also possible to load an entire set of models that have already been batch meshed in order to take advantage of the Load Mesh option in the Run Status tab.

10. If you make modifications to your criteria or parameter files, you can submit a run again. BatchMesher will place the new files in a separate sub-directory.

Step 5 (Optional): Edit the criteria and parameter files. 1.

Click the Configurations tab.

2.

Right-click on the Criteria File or Parameter File field that you wish to edit and select Edit File from the context menu. The Criteria and Parameters Files Editor dialog appears.

Proprietary Information of Altair Engineering

p.188

Altair HyperMesh 2019 Tutorials

•

From the Criteria tab, you can set the target element size, element criteria, and the method that is used to calculate the values. You can also select the Advanced Criteria Table check box to enabled additional options that give you more control over the intermediate QI values, however, it is usually not necessary to edit these options in order to obtain a good quality mesh. The Use min length from timestep calculator check box is also available for explicit solver models. If you select this check box, the overall minimum element size will be set by this option and the top element checks will be disabled.

•

From the Parameters tab, you can set all of the meshing controls over various geometric features. Parameters are grouped into sections; you can click the small downward-arrows next to each section to show and hide that section. The number of parameters is extensive; for more details, see the Parameters Editor topic in the BatchMesher help.

Proprietary Information of Altair Engineering

p.189

Altair HyperMesh 2019 Tutorials

p.190

HM-3150: Meshing a Model Using Shrink Wrap In this tutorial you will learn how to mesh a component using the: •

loose shell shrink wrap.

•

tight shell shrink wrap.

•

tight solid shrink wrap.

You can use the Shrink Wrap tool to generate an enclosed volume or solid mesh. This tools is typically used to approximate and simplify an existing model.

Model Files This exercise uses the shrinkwrap.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Meshing a Model Using Shrink Wrap In HyperMesh, you can shrink wrap elements, components, surfaces, or solids. The shrink wrap allows for wrapping of multiple components if they are selected. The selection provides the option to wrap all nodes, elements, components, surfaces, points, or solids, or only a certain portion of the model if desired. The input to the shrink wrap (that is, the model parts that you wish to wrap) can consist of 2D or 3D elements along with surfaces or solids. The shrink wrap is able to stitch over very bad geometry to generate an enclosed volume mesh for tetra-meshing. The shrink wrap tool can work from elements (whether 2D or 3D) or geometry. Thus, in the case of an "unclean" geometry model with many released (free) edges, you can either generate any arbitrary mesh on the unclean geometry using the automesh functionality beforehand and then create shrink wrap or you can simply select the surface or solid without meshing the geometry first; either of these steps will yield good output mesh. The key in such cases is to ensure that the element size used for the shrink wrap is large enough to stitch over the unclean surface edge splits so that an enclosed volume can be created. The element size affects the ability of the shrink wrap to follow the geometry of the model. The larger the element size, the more simplified the model will appear. With a smaller element size, the shrink wrap will more closely follow the model. The jacobian value for the solid mesh follows the same type of pattern. As the jacobian value gets smaller, the shrink wrap more closely follows the profile of the model. The smaller the jacobian value, the longer it takes to generate the mesh. Shrink wrap mesh can be generated as a surface mesh, or as a full-volume hex mesh, by use of the Shrink Wrap panel. The distinction between surface or volume mesh is a check box labeled generate solid mesh.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.191

Step 1: Open the model shrinkwrap.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the shrinkwrap.hm model file.

Step 2: Create a loose shell shrink wrap mesh in the loose_gap component. 1.

If the model's geometry and surface edges are not shaded, click Visualization toolbar.

2.

From the graphics area, review the surface geometry.

3.

Open the Shrink Wrap panel by clicking Mesh > Create > Shrink Wrap Mesh from the menu bar.

4.

Switch the tight wrap toggle to loose wrap.

5.

Verify that the entity selector is active and set to comps.

6.

From the graphics area, select the component. HyperMesh highlights the entire component.

7.

In the element size= field, enter 4.

8.

Click mesh. HyperMesh generates the shrinkwrap.

Proprietary Information of Altair Engineering

on the

Altair HyperMesh 2019 Tutorials

9.

In the Model browser, Component folder, right-click on surfaces and select Hide from the context menu.

Step 3: Review the solid geometry. 1.

In the Model browser, Component folder, right-click on loose_gap and select Hide from the context menu.

2.

Right-click on the block component and select Show from the context menu.

3.

From the graphics area, review the model to see the features.

4.

Right-click on the block component and select Hide from the context menu.

Step 4: Create a loose shell shrink wrap mesh in the loose component. 1.

In the Model browser, Component folder, right-click on loose and select Make Current from the context menu.

2.

Click comps >> block. Note:

Deselect any other components, if necessary.

Proprietary Information of Altair Engineering

p.192

Altair HyperMesh 2019 Tutorials

3.

Click select.

4.

In the element size= field, enter 10.

5.

Click mesh. HyperMesh generates the shrinkwrap.

6.

Reject the mesh by clicking reject.

7.

In the element size= field, enter 5.

8.

Click mesh. HyperMesh generates the shrinkwrap.

9.

Reject the mesh by clicking reject.

10. In the element size= field, enter 3.

Proprietary Information of Altair Engineering

p.193

Altair HyperMesh 2019 Tutorials

11.

p.194

Click mesh. HyperMesh generates the shrinkwrap.

The shrink wrap mesh with the geometry hidden

Step 5: Create a tight shell shrink wrap in the tight_shell component. 1.

In the Model browser, Component folder, right-click on loose and select Hide from the context menu.

2.

Right-click on the tight_shell component and select Make Current from the context menu.

3.

Switch the loose wrap toggle to tight wrap.

4.

Click comps >> block. Note:

Deselect any other components, if necessary.

5.

Click select.

6.

In the element size= field, enter 3.

7.

Click mesh. HyperMesh generates the shrinkwrap. Note:

The tight mesh conforms much more closely to the model's geometry than the loose mesh did, even at the same element size.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 6: Create a tight solid shrink wrap in the tight_solid component 1.

In the Model browser, Component folder, right-click on tight_shell and select Hide from the context menu.

2.

Right-click on the tight_solid component and select Make Current from the context menu.

3.

Select the generate solid mesh checkbox.

4.

Click comps >> block. Note:

Deselect any other components, if necessary.

5.

Click select.

6.

In the minimum jacobian= field, enter 1.

7.

Click mesh. HyperMesh generates the shrinkwrap. Note:

The resulting mesh is very blocky, due to the high jacobian value.

8.

Reject the mesh by clicking reject.

9.

In the minimum jacobian= field, enter 0.7.

10. Click mesh. HyperMesh generates the shrinkwrap. Note:

This mesh is smoother than it was when the minimum jacobian was set at 1.0.

11. Open the Mask panel by pressing F5.

Proprietary Information of Altair Engineering

p.195

Altair HyperMesh 2019 Tutorials

12. Set the entity selector to elems. 13. Select a group of elements by pressing SHIFT while left-clicking to draw a box. 14. Click mask. HyperMesh masks the elements. 15. Rotate the model to verify that the mesh generation was a solid mesh, with 3D elements throughout the model.

The 3D mesh fills the model's volume, rather than only covering its outer surfaces.

Step 7 (Optional): Change the minimum jacobian to 0.3 for optimized mesh. In this step, you should still be in the mask panel. 1.

Click unmask all.

2.

Open the Delete panel by pressing F2.

3.

Click elems >> displayed.

4.

Click delete entity.

5.

Open the Shrink Wrap panel.

6.

Click comps >> block. Note:

Deselect any other components, if necessary.

7.

Click select.

8.

In the minimum jacobian field, enter 0.3.

9.

Click mesh. HyperMesh generates the shrinkwrap. Note: This mesh is smoother than it was when the minimum jacobian had higher values.

Proprietary Information of Altair Engineering

p.196

Altair HyperMesh 2019 Tutorials

p.197

HM-3200: Tetrameshing In this tutorial, you will learn about: •

Volume tetra mesher

•

Standard tetra mesher

•

Checking tetra element quality

•

Remeshing tetra elements

HyperMesh provides two methods for generating a tetrahedral element mesh. The volume tetra mesher works directly with surface or solid geometry to automatically generate a tetrahedral mesh without further interaction with you. Even with complex geometry, this method can often generate a high quality tetra mesh quickly and easily. The standard tetra mesher requires a surface mesh of tria or quad elements as input, and then provides you with a number of options to control the resulting tetrahedral mesh. This offers a great deal of control over the tetrahedral mesh, and provides the means to generate a tetrahedral mesh for even the most complex models. You can use the Tetramesh panel to fill an enclosed volume with first or second order tetrahedral elements. A region is considered enclosed if it is entirely bounded by a shell mesh (tria or quad elements), where each element has material on one side and open space on the other.

Model Files This exercise uses the housing.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Retrieve and view the model file. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the housing.hm model file.

4.

Observe the model using the different visual options available in HyperMesh (rotation, zooming, and so on). Only the geometry in the component cover is currently displayed. The file contains two parts defined by a volume of surfaces. The geometry has been cleaned such that surface connectivity is proper and surface edges that would cause sliver elements are suppressed.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.198

Step 2: Use the volume tetra mesher and equilateral triangles to create a tetra mesh for the cover. 1.

Open the Tetramesh panel by clicking Mesh > Create > Tetra Mesh from the menu bar.

2.

Go to the Volume tetra subpanel.

3.

Set the Enclosed volume selector to surfs .

4.

Select one of the surfaces in the model.

5.

Verify that the 2D type is set to trias and the 3D type is set to tetras. These options control the type of elements that HyperMesh creates for the surface mesh and solid mesh of the part.

6.

Verify that the toggle is set to Elems to Current Comp. This option allows HyperMesh to place the newly created elements in the current component collector.

7.

Verify that the Use curvature and Use proximity checkboxes are clear.

8.

In the Element size field, enter 10.

9.

Click mesh. HyperMesh creates the tetra mesh.

10. If the model's mesh lines and elements are not shaded, click toolbar.

on the Visualization

11. Inspect the mesh pattern that the volume tetra mesher created.

Tetra mesh created in the volume tetra subpanel using equilateral triangles (2D: trias)

12. Reject the mesh by clicking reject.

Step 3: Use the volume tetra mesher and right triangles to create a tetra mesh for the cover. In this step, you should still be in the Volume tetra subpanel.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

1.

Select one of the surfaces in the model.

2.

Set the 2D type to R-trias.

3.

Click mesh. HyperMesh creates the tetra mesh.

4.

Inspect the mesh pattern that the volume tetra mesher created and compare it to the first mesh that you created. Note:

The 2D type: R-trias setting tends to create tetra elements with triangular faces that are right triangles (90-45-45 angles), while the 2D type: trias setting tends to create equilateral triangles (60-60-60 angles).

Tetra mesh from the volume tetra subpanel and right triangles (2D type: R-trias)

5.

Reject the mesh by clicking reject.

Step 4: Use the volume tetra mesher to create a tetra mesh with more elements along curved surfaces. In this step, you should still be in the Volume tetra subpanel. 1.

Select one of the surfaces in the model.

2.

Select the Use curvature checkbox. The option causes more elements to be created along areas of high surface curvature. Thus, curved areas such as fillets will have more and smaller elements, which capture those features with higher resolution.

3.

In the Min elem size field, enter 1.0.

4.

Verify that the Feature angle is set to 30.

5.

Click mesh. HyperMesh creates the tetra mesh.

Proprietary Information of Altair Engineering

p.199

Altair HyperMesh 2019 Tutorials

6.

Inspect the mesh pattern that the volume tetra mesher created and compare it to the previous meshes you created. You can see that more small elements are created around the fillets.

Tetra mesh from the volume tetra subpanel with the use curvature check box selected

7.

Reject the mesh by clicking reject.

Step 5: Use the volume tetra mesher to create a tetra mesh with more elements around small features. In this step, you should still be in the Volume tetra subpanel. 1.

Select one of the surfaces in the model.

2.

Select the Use proximity checkbox. This option causes the mesh to be refined in areas where surfaces are smaller, which results in a nice transition from small elements on small surfaces to larger elements on larger, adjacent surfaces.

3.

Click mesh. HyperMesh creates the tetra mesh.

Proprietary Information of Altair Engineering

p.200

Altair HyperMesh 2019 Tutorials

4.

p.201

Inspect the mesh pattern that the volume tetra mesher created and compare it to the previous meshes you created. You can see that more elements are created around the surfaces with small angles.

Tetra mesh from the volume tetra subpanel with the Use curvature and Use proximity check boxes selected.

Step 6: Prepare the display to tetra mesh the hub component using the standard tetra mesher. 1.

In the Model browser, turn off the display of every component's geometry except for hub.

2.

Turn off the display of every component's elements except for hub and tetras. Note:

3.

There are tria shell elements in the hub component, and no elements in the tetras component.

Return to the main menu by clicking return.

Step 7 (Optional): Review the connectivity and quality of the tria mesh to validate its integrity for the standard tetra mesher. In this step you will use the Edges and Check Elems panels to make sure that there are no free edges or very small angles in the tria shell mesh. 1.

Open the Edges panel by clicking Mesh > Check > Components > Edges from the menu bar.

2.

Verify that the entity selector is set to comps.

3.

Select a tria element on the hub component. HyperMesh highlights the entire component.

4.

Click find edges. The status bar displays a message that reads, "No edges were found. Selected elements may enclose a volume." Note:

5.

The tetra mesher requires a closed volume of shell elements.

Return to the main menu by clicking return.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

Open the Check Elements panel by clicking Mesh > Check > Elements > Check Elements from the menu bar.

7.

Verify that you are in the 2-d subpanel.

8.

Identify the elements that have an aspect ratio greater than 5.

p.202

Aspect ratio is the ratio of the longest edge of an element to its shortest edge. This check helps you to identify sliver elements. All of the hub’s shell elements pass the check; all of the elements have an aspect ratio less than 5. 9.

Identify the tria elements that have an angle less than 20. This check helps identify sliver elements. All of the hub’s shell elements pass the check; all the elements have angles greater than 20. The surface mesh is suitable for creating a tetra mesh.

10. Return to the main menu by clicking return.

Step 8: Create a tetra mesh for the hub using the standard tetra mesher. 1.

In the Model browser, Component folder, right-click on tetras and select Make Current from the context menu.

2.

Open the Tetra Mesh panel.

3.

Go to the Tetra mesh subpanel.

4.

Verify that the Float trias/quads to tetra mesh entity selector is set to comps. Note:

By using this entity selector, HyperMesh will swap the diagonal for any pair of surface trias, which will result in a better tetra mesh quality. If you would rather keep the diagonal, see step 8.6.

5.

Select a shell element on the hub component. HyperMesh highlights the entire component.

6.

Optional: Keep the diagonal as is by activating the Fixed trias/quads to tetra mesh entity selector and setting it to comps.

7.

Click mesh. HyperMesh generates the tetrahedral elements.

Cut-away view of tetrahedral elements using the Masks panel

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.203

Step 9: Check the quality of the hub’s tetra elements. 1.

In the Model browser, only display the tetras component elements.

2.

Open the Check Elements panel.

3.

Go to the 3-d subpanel.

4.

Identify the smallest element length among the displayed elements. If the minimum length is acceptable for a target element size of 5.0, then no further action is necessary.

5.

Identify the smallest angle (tria faces: min angle) among the displayed elements. If the minimum tria face angle is no less than 10°, then the mesh quality should be acceptable.

6.

Identify elements that have a tet collapse smaller than 0.3. The status bar indicates that three elements have a tetra collapse smaller than 0.3. Note:

The tet collapse criteria is a normalized volume check for tetrahedral elements. A value of 1 indicates a perfectly formed element with maximum possible volume. A value of 0 indicates a completely collapsed element with no volume.

Step 10: Isolate the element with the tetra collapse smaller than 0.2 and find the elements surrounding it. In this step, you should still be in the Check Elements panel. 1.

With 0.3 still specified in the tet collapse< field, click tet collapse.

2.

Click save failed. HyperMesh saves the elements that failed the tetra collapse check in the user mark. Note:

You can retrieve the saved elements that failed the check from any panel by selecting retrieve in the extended selection menu.

3.

Return to the main menu by clicking return.

4.

Open the Mask panel by pressing F5.

5.

Set the entity selector to elems.

6.

Click elems >> retrieve. HyperMesh retrieves the elements that were saved in the Check Elements panel.

7.

Click elems >> reverse.

8.

Click mask. HyperMesh masks the elements and displays the three tetra element that failed the tetra collapse check.

9.

Return to the main menu by clicking return.

10. On the Display toolbar, click . HyperMesh identifies and displays the layer of elements that are attached to the three displayed element. 11. Click two more times. HyperMesh identifies and displays the layers of elements that are attached to the displayed elements. Note:

You can duplicate the functionality of unmask adjacent using the Find panel, find attached subpanel in the Tool page.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

12. In the Model browser, turn off the display of the hub elements that were unmasked.

Step 11: Remesh the hub’s displayed tetra elements to improve their tetra collapse. 1.

Open the Tetra Mesh panel.

2.

Go to the Tetra remesh subpanel.

3.

Click 3D elements: elems >> displayed.

4.

Click remesh. HyperMesh regenerates this area of the mesh.

5.

Return to the main menu by clicking return.

6.

Open the Check Elements panel.

7.

Find out if the tetra collapse has improved for the displayed elements by clicking tet collapse. The status bar indicates that the minimum tetra collapse is larger than the value reported before the tetra elements were remeshed.

8.

Return to the main menu by clicking return.

Step 12 (Optional): Save your work. Now that the tetra mesh is complete, it is a good time to save the model. 1.

From the menu bar, click File > Save > Model.

Summary You have created a tetra mesh for both parts in the model using different tetra meshing procedures. Either method can be used to mesh parts, depending on the needs of the analysis. The tetra remesh function was used in this tutorial to show how to quickly fix the quality of tetra elements.

Proprietary Information of Altair Engineering

p.204

Altair HyperMesh 2019 Tutorials

HM-3210: Creating a Hex-Penta Mesh using Surfaces In this tutorial, you will learn how to: •

Create solids using different functions

•

Check and fix improper model connectivity

For some analyses, it is desirable to use a mesh of hexahedral and pentahedral elements. This is especially true for parts which have a large thickness compared to the element size being used, or for parts that have many features and/or changes in thickness. Castings or forgings are good examples.

Model Files This exercise uses the arm_bracket.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Creating a Hex-Penta Mesh using Surfaces The objective of this exercise is to introduce you to a number of HyperMesh functions that are used to create hexa-penta meshes. The arm_bracket.hm model is organized into four IGES layers, consisting of 1) the base, 2) the first section of the arm, with a constant cross section and curvature, 3) the second section of the arm, with a tapered cross section, and 4) the boss.

Step 1: Retrieve and review model file. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the arm_bracket.hm model file.

Proprietary Information of Altair Engineering

p.205

Altair HyperMesh 2019 Tutorials

p.206

Step 2: Mesh the top surface of the base, including the L-shaped surface. 1.

In the Model browser, Component folder, right-click on base and select Make Current from the context menu.

2.

Right-click on base again and select Isolate from the from the context menu. HyperMesh hides all of the components except for base.

3.

Open the AutoMesh panel by clicking Mesh > Create > 2D AutoMesh from the menu bar.

4.

Go to the size and bias subpanel.

5.

Shade the model's geometry and surface edges by clicking toolbar.

6.

Verify that the entity selector is set to surfs.

7.

Select the surfaces on the top of the base, including the L-shaped surface at the intersection of the base and the arm.

8.

Set the meshing mode to automatic.

9.

In the element size field, enter 10.

10. Set the mesh type to quads only. 11. Click mesh. HyperMesh meshes the selected surface.

Resulting quad mesh on base surfaces

Proprietary Information of Altair Engineering

on the Visualization

Altair HyperMesh 2019 Tutorials

12. Return to the main menu by clicking return.

Step 3: Create layers of hex elements for the base. 1.

Open the Elem Offset panel by clicking Mesh > Create > 3D Elements > Element Offset from the menu bar.

2.

Go to the solid layers subpanel.

3.

Click elems to offset: elems >> displayed. HyperMesh selects the elements on the base.

4.

In the number of layers = field, enter 5.

5.

In the total thickness = field, enter 25.

6.

Click offset+. HyperMesh creates the hexa mesh.

Hex mesh on base

Step 4: Prepare the display for meshing the arm’s curved segment. 1.

In the Model browser, Component folder, right-click on arm_curve and select Show from the context menu.

2.

Open the Mask panel by pressing F5.

3.

Click elems >> by config.

4.

Click config= and select the hex8 configuration.

5.

Click select entities. HyperMesh selects all of the elements with a configuration of hex8 in the model.

6.

Click mask. HyperMesh masks the elements.

7.

Return to the main menu by clicking return.

Step 5: Create a node at the center of the arm radius. The first segment of the arm can be meshed using the Spin panel. This requires a node to be selected as the center point of rotation. In this step, you will use the distance panel, 3 nodes subpanel to create a node that will be used as the center point of rotation.

Proprietary Information of Altair Engineering

p.207

Altair HyperMesh 2019 Tutorials

p.208

1.

Open the Distance panel by pressing F4.

2.

Go to the three nodes subpanel.

3.

Verify that the N1 node selector is active.

4.

While pressing the left mouse button, move it over the curved line as indicated in the following image, and then release it when the cursor changes to highlights the line.

.

HyperMesh

5.

Click three locations along the selected line. The active selector advances from N1 to N2 to N3, and HyperMesh create the temporary nodes on the selected curved line of the arm.

6.

Click circle center . HyperMesh creates the node at the center. Note:

You will use this node in the next step when you mesh the arm.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

7.

Return to the main menu by clicking return.

Step 6: Create hexa elements in the curved portion of the arm using spin. 1.

In the Model browser, Component folder, right-click on arm_curve and select Make Current from the context menu.

2.

Open the Spin panel by clicking Mesh > Create > 3D Elements > Spin from the menu bar.

3.

Go to the spin elems subpanel.

4.

Click 2d elems: elems >> by window.

5.

Select the plate elements within the L-shaped cross section of the arm as indicated in the following image.

6.

Click select entities.

7.

In the angle = field, enter 90 degrees.

8.

Set the orientation vector to x-axis (Y-Z plane).

9.

Select the center node you created in step 5 for the base node (B).

10. In the on spin = field, enter 24. Note:

This option determines how many layers of hex elements HyperMesh creates when the plate elements are spun.

11. Click spin -.

Proprietary Information of Altair Engineering

p.209

Altair HyperMesh 2019 Tutorials

12. Return to the main menu by clicking return.

spin panel results

Step 7: Create faces on the hex elements. 1.

Open the Faces panel by clicking Mesh > Check > Components > Faces from the menu bar.

2.

Set the entity selector to comps.

3.

Click comps >> arm_curve.

4.

Click select.

5.

Click find faces. HyperMesh creates 2D shell elements on the free faces of every 3D solid element in the component, and places them in a new component named ^faces. Note:

6.

The ^faces component is created with its visualization set to wireframe, therefore you will not be able to see the new elements right away if the arm_curve component is displayed and in shaded mode.

Shade the model's elements and mesh lines by clicking on the Visualization toolbar. The graphics area now displays the elements in the ^faces component.

Step 8: Prepare the display for meshing the second arm segment. 1.

From the Model browser, turn on the display of the arm_straight and ^faces components.

Proprietary Information of Altair Engineering

p.210

Altair HyperMesh 2019 Tutorials

p.211

Step 9: Mesh the L-shaped set of surfaces between the arm_straight and boss components. 1.

In the Model browser, Component folder, right-click on arm_straight and select Make Current from the context menu.

2.

Open the Automesh panel.

3.

Select the three surfaces lying on the intersection between the arm_straight and boss components as indicated in the following image. Note:

These surfaces are all in the arm_straight component.

4.

Set the meshing mode to interactive.

5.

Click mesh. The meshing module opens.

6.

Go to the density subpanel.

7.

Adjust the density of each edge to obtain a mesh that matches the following image. Note:

This mesh pattern matches the mesh pattern at the intersection of the two arm segments. This is necessary for the next step.

Densities to correspond to the mesh on the end face

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

8.

Click mesh. HyperMesh updates the mesh density.

9.

Create the elements and go back to the main menu by clicking return twice.

Step 10: Use linear solid to build the mesh between the two sets of shell elements. 1.

Open the Linear Solid panel by clicking Mesh > Create > 3D Elements > Linear 3D from the menu bar.

2.

Activate the from: elems selector.

3.

Select the ^faces elements lying on the intersection between the first and second arm segments as indicated in the following image. Tip:

Quickly select all of the necessary elements by selecting one of the elements and then clicking from: elems >> by face.

4.

Activate the to: elems selector.

5.

Select the shell elements, between the arm and boss, that you created using the Automesh panel in step 9.

6.

Activate the from: alignment: N1 selector.

7.

Select three nodes on one of the "from elements" that you selected in step 10.3 as indicated in the following image.

8.

Activate the to: alignment: N1 selector.

Proprietary Information of Altair Engineering

p.212

Altair HyperMesh 2019 Tutorials

9.

Select three nodes on the "to element" that corresponds to the "from element" with the three "from nodes" as indicated in the following image.

Example selection for alignment nodes

10. In the density = field, enter 12. 11. Click solids. HyperMesh creates the mesh.

Linear solid mesh

12. Return to the main menu by clicking return.

Proprietary Information of Altair Engineering

p.213

Altair HyperMesh 2019 Tutorials

Step 11: Prepare the display for meshing the boss. 1.

In the Model browser, Component folder, right-click on boss and select Show from the context menu.

Step 12: Create a shell mesh on the bottom of the boss. 1.

In the Model browser, Component folder, right-click on boss and select Make Current from the context menu.

2.

Open the Automesh panel.

3.

Select the five surfaces on the bottom face of the boss as indicated in the following image.

4.

Click mesh. The meshing module opens.

Proprietary Information of Altair Engineering

p.214

Altair HyperMesh 2019 Tutorials

5.

Adjust the density of each edge to obtain a mesh that matches the following image.

Mesh densities on the bottom of the boss

6.

Click mesh. HyperMesh updates the mesh density.

7.

Return to the main menu by clicking return twice.

Step 13: Project a node to the bottom face of the boss. 1.

Open the Project panel by clicking Mesh > Project > Nodes from the menu bar.

2.

Go to the to line subpanel.

3.

Select the node on the rightmost top vertex as indicated in the following image.

4.

Click nodes >> duplicate.

5.

Activate the to line: line list selector.

6.

Select the line on the boss’ top face as indicated in the following image.

Projecting a node to a line

Proprietary Information of Altair Engineering

p.215

Altair HyperMesh 2019 Tutorials

7.

Set the along vector to x- axis.

8.

Click project. The node projects to the line.

9.

Return to the main menu by clicking return.

Step 14: Generate hexas for the boss using the Solid Map panel. 1.

Open the Solid Map panel by clicking Mesh > Create > Solid Map Mesh from the menu bar.

2.

Go to the general subpanel.

3.

Click the source geom switch and select none.

4.

Activate the dest geom: surf selector.

5.

Select the top surface of the boss as indicated in the following image.

6.

Click the along geom switch and select mixed.

7.

Activate the along geom: mixed lines selector.

8.

Select the line indicated in the following image.

9.

Activate the along geom: mixed node path selector.

10. Select the 13 nodes as indicated in the following image, to define the exact location of the solid element layers. Note:

A total of 13 nodes should be selected, starting at the boss mesh, and then using all of the nodes along the edge of the arm_straight component, ending with the node projected to the top of the boss.

Proprietary Information of Altair Engineering

p.216

Altair HyperMesh 2019 Tutorials

Along nodes for solid map

11. Click elems to drag: elems >> by collector >> boss. 12. Click select. 13. Click mesh. HyperMesh creates the elements and completes the mesh on this part.

Completed mesh of the arm bracket

14. Return to the main menu by clicking return.

Proprietary Information of Altair Engineering

p.217

Altair HyperMesh 2019 Tutorials

Step 15 (optional): Check the connectivity of the model. 1.

Go to the Faces panel.

2.

Click comps. HyperMesh displays a list of components.

3.

Select every component from the list, or select comps >> all.

4.

Click select.

5.

Click find faces.

6.

From the Model browser, turn off the geometry display of all components.

7.

Turn off the element display of all components except ^faces.

8.

Exit the the panel by clicking return.

9.

From the Post page, select hidden line.

10. Select the xz plane and trim plane checkboxes. 11. Click show plot. HyperMesh displays the faces with a plane cutting the model in half. Note:

This allows you to review the interior of the model.

12. Click near the cutting plane, hold the left mouse button down, and move your mouse back and forth. The cutting plane moves through the model, allowing you to see if any face elements exist on the interior of the model. Note:

You should see that there are face elements interior to the model, between the boss and arm. You need to perform some corrections on the connectivity.

Hidden line view of faces

13. Return to the main menu by clicking return.

Proprietary Information of Altair Engineering

p.218

Altair HyperMesh 2019 Tutorials

p.219

Step 16 (Optional): Correct the connectivity of the model. 1.

In the Model browser, display the elements for all of the components except for ^faces.

2.

Display the model's elements as transparent by clicking toolbar.

3.

Go to the Faces panel.

4.

Set the entity selector to elems.

5.

Click elems >> displayed.

6.

Click preview equiv. HyperMesh highlights coincident nodes on the intersection between the arm and the boss.

7.

Specify a slightly larger value in the tolerance = field, and then click preview equiv. Hypermesh identifies more more coincident nodes on the intersection.

8.

Repeat step 16.7 until all 60 coincident nodes have been found.

9.

Click equivalence. HyperMesh replaces the nodes to the location of the lowest node ID.

on the Visualization

10. Switch all the components to the shaded visual mode.

Step 17 (Optional): Recheck the connectivity of the model. Repeat Step 15 to make sure the model is now equivalenced. If you find errors, repeat Step 16.

Step 18 (Optional): Save your work. Now that the 3D solid mesh has been completed, it is a good time to save your model. 1.

From the menu bar, click File > Save > Model.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.220

HM-3220: Creating a Hexahedral Mesh using the Solid Map Function In this tutorial, you will learn how to create a hexahedral mesh using the Solid map function by one volume and multisolid method. Solids are geometric entities that define a three-dimensional volume. The use of solid geometry is helpful when dividing a part into multiple volumes. For example, divide a part into simple, mappable regions to hex mesh the part. Use the Solid Map panel to create a mesh of solid elements in a solid geometric volume.

Model Files This exercise uses the solid_map.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Hex-meshing Solid Geometry

Step 1: Retrieve model file, solid_map.hm. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the solid_map.hm model file.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.221

Step 2: Mesh the 1/8th sphere-shaped region. on the Visualization

1.

Shade the model's geometry and surface edges by clicking toolbar.

2.

Open the Solid Map Mesh panel by clicking Mesh > Create > Solid Map Mesh from the menu bar.

3.

Go to the one volume subpanel.

4.

Under along parameters, enter 1 in the elem size= field.

5.

Activate the volume to mesh: solid entity selector.

6.

Select the small cube-shaped solid, as indicated in the following image.

7.

Click mesh.

8.

Shade the model's elements and mesh lines by clicking toolbar.

9.

Select the solid as indicated in the following image.

Proprietary Information of Altair Engineering

on the Visualization

Altair HyperMesh 2019 Tutorials

10. Click mesh. 11. Return to the main menu by clicking return.

Step 3: Create a shell mesh with the Automesh panel to control a mesh pattern. 1.

Open the Automesh panel by clicking Mesh > Create > 2D AutoMesh from the menu bar.

2.

Go to the size and bias subpanel.

3.

Select the surface as indicated in the following image.

4.

Set the meshing mode to interactive.

5.

In the element size = field, enter 1.000.

6.

Set the mesh type to mixed.

7.

Click mesh. The meshing module opens.

8.

Verify that you are in the density subpanel.

9.

In the elem density = field, enter 4.

10. Click set all to. HyperMesh sets all the edge densities to 4. 11. Click mesh. 12. Return to the main menu by clicking return twice.

Proprietary Information of Altair Engineering

p.222

Altair HyperMesh 2019 Tutorials

Step 4: Mesh the solid volume on which the surface mesh was created in Step 3. 1.

Open the Solid Map Mesh panel.

2.

Go to the one volume subpanel.

3.

Select the volume shown in the following image.

4.

Under along parameters, toggle elem size= to density= .

5.

In the density= field, enter 10.

6.

Click mesh.

7.

Rotate the part and note how the mesh pattern created with the Automesh panel has been used for the solid elements.

Proprietary Information of Altair Engineering

p.223

Altair HyperMesh 2019 Tutorials

p.224

Step 5: Mesh the remaining solid volumes. In this step, you should still be in the Solid Map Mesh panel, one volume subpanel. 1.

Select one of the remaining unmeshed solid volumes. Note:

Make sure to select a solid adjacent to one that has already been meshed so that connectivity is maintained.

2.

Set the source shells to mixed.

3.

Under along parameters, toggle density= to elem size=

4.

In the elem size= field, enter 1.5.

5.

Click mesh.

6.

Repeat until all solid volumes are meshed.

7.

Return to the main menu by clicking return.

Step 6 (Optional): Save your work. With this section of the exercise completed, it is a good time to save the model. 1.

From the menu bar, click File > Save > Model.

Automated Solid Map Meshing The capability to automate the solid map meshing process is now available. Using the “Mappable” visualization mode in conjunction with the multi-solids feature will inform you that the solid(s) are ready for solid meshing. Using the multi-solids feature will allow for all solids within the model to be meshed in one step, provided that they are mappable. In this section of the tutorial, you will delete all of the elements from the previous section. You will then use the Mappable visualization mode with multi-solids to solid mesh the part.

Step 7: Delete the elements within the model. 1.

Open the Delete panel by pressing F2.

2.

Click elems >> all.

3.

Click delete entity.

4.

Return to the main menu by clicking return.

Step 8: Use the mappable visualization mode. 1.

Shade the model's geometry and surface edges by clicking toolbar.

2.

From the Geometry Visualization list, select each solid to represent its mappable state. Note:

on the Visualization . HyperMesh color codes

The goal is to ensure that each solid is either 1-directional or 3-directional mappable.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

From the menu bar, click Preferences > Colors.

4.

In the Color dialog click the Geometry tab.

5.

Optional: Under By mappable display mode (solids), click the color swatches to adjust the display color of the following: •

1dir. map: Visualization for solids that can be mapped, for 3D meshing, in one direction.

•

3dir. map: Visualization for solids that can be mapped, for 3D meshing, in three directions.

•

ignored map: Default visualization for solids that require partitioning to become mappable.

•

not mappable: Visualization for solids that have been edited, but still require further partitioning to create mappable solids.

p.225

Once in the mappable visualization mode, it is clear that there is one 3-directional mappable solid and the rest are 1-directional mappable.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 9: Use the multi-solid feature to mesh the part. 1.

Open the Solid Map Mesh panel.

2.

Go to the multi solids subpanel.

3.

Click solids >> all. HyperMesh selects all of the solids in the model.

4.

Set the source shells to mixed.

5.

In the elem size field, enter 1.

6.

Click mesh. HyperMesh opens the interactive mesh mode.

7.

Accept the shell elements and create solid elements by clicking mesh. Note:

The solids will be sequentially solid meshed.

8.

Inspect the model and note that the mesh within all of the solids is correctly equivalenced.

9.

Accept the solid element mesh and return to the Solid Map Mesh panel by clicking return.

Proprietary Information of Altair Engineering

p.226

Altair HyperMesh 2019 Tutorials

Step 10 (Optional): Save your work. With this exercise completed, you can save the model if desired. 1.

From the menu bar, click File > Save > Model.

Proprietary Information of Altair Engineering

p.227

Altair HyperMesh 2019 Tutorials

HM-3270: Using the TetraMesh Process Manager In this tutorial, you will learn how to use the TetraMesh Process Manager to: •

Import geometry or a HyperMesh File

•

Clean up geometry

•

Organize the model (holes and features)

•

Establish mesh size and pattern for the organized geometry

•

Create a 2D Mesh

•

Clean up the 2D mesh

•

Create a 3D TetraMesh

The Process Manager contains a step-by-step checklist of procedures that allow you to quickly organize and tetramesh a geometric model. Each step is formatted in a hierarchical list that provides the order in which the process must be performed. Specialized tools are also provided at each step to simplify the process. You can perform these steps manually, but it is generally faster to perform them in the Tetramesh Process Manager.

Model Files This exercise uses the tetmesh_pm.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Initiate the Process Manager. 1.

Start a new session in the TetraMesh Process Manager by clicking Mesh > Create > TetraMesh Process > Create New from the menu bar.

2.

In the Create New Session dialog, enter a name for the session in the New Session Name field. Note:

Creating a session name and saving the session allows you to stop the process before completion and then load it again at a later time, picking up the process at the point it was left off.

3.

In the Working Folder field, navigate to the location of your working directory.

4.

Click Create. The Process Manager opens in the tab area.

Proprietary Information of Altair Engineering

p.228

Altair HyperMesh 2019 Tutorials

p.229

2: Import geometry. At this point, the TetraMesh Process Manger automatically assembles the TetraMesh process flow. The first step, Geometry Import, is highlighted in the tab area, and the panel area has been configured with specific panels for aiding the Tetramesh Process Manager template. If you need to access standard HyperMesh panels, undock the Process Manager panels to a separate dialog by clicking the Process Manager panels, click

in the panel area. To re-dock

in the Process Manager dialog.

1.

In the panel area, set Import Type to HM Model.

2.

In the Import Filename field, open the file tetmesh_pm.hm.

3.

Click Import. Hypermesh imports the model. Note:

A green checkmark appears next to the Geometry Import step in the Process Manager tab, which indicates that the step is complete.

Step 3: Clean up the geometry. 1.

On the Visualization toolbar, select modes, and click

from the list of geometry color

to shade the model's geometry and surface edges.

2.

In the panel area, select the Edge Tools tab.

3.

Click Isolate. HyperMesh isolates the surfaces with free edges on them.

Isolated Surfaces with free edges.

4.

Select the Free Edges tab.

5.

Click Equivalence. HyperMesh fixes all of the free edges. Tip:

If this did not correct all of the free edges, increase the Tolerance value until all of the free edges are equivalenced.

6.

Select the Edge Tools tab.

7.

Click Isolate. A dialog appears with a message that reads, "No edges found..." Note:

This confirms that all of the edges have been fixed.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

8.

Click Display All. HyperMesh displays the entire model.

9.

Click ACCEPT.

p.230

Step 4: Organize and Clean up holes. In the Organize and Cleanup Holes step, you will organize the surfaces that form holes in the model. The TetraMesh Process Manager can automatically sort and organize holes into separate component collectors based upon their diameter. This will allow you to specify a mesh type, circumference element count, and longitudinal element size for different hole groups. 1.

In the Hole Parameters Table, D< column, enter 5 in the first row and 10 in the second row. Note:

This will organize the holes into two collectors that will include holes ranging from 0 - 5 units and 5 - 10 units collectively.

2.

Click Auto Organize. HyperMesh organizes all of the holes in the model less than 10 units into two component collectors, each with a different color.

3.

From the Model browser, expand the Components folder. Note:

Two new component collectors, with the name solidholes followed by the numerical average of the diameter range of the holes, are created.

Transparent view of model showing all holes and bores organized

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

In the Hole Parameters Table, Num Circumference Elems column, enter 12 in each row. Note:

5.

p.231

The Num Circumference Elems field governs the number of elements that will be meshed around the hole.

In the Longitudinal Elem Size column, enter 1 in each row. Note:

The Longitudinal Elem Size field dictates the unit size of the elements through the length of the hole.

6.

Click Auto Organize.

7.

Click ACCEPT.

Step 5: Mesh holes. 1.

In the Hole Parameters Table, Mesh Type column, select R-tria regular in each row.

2.

Click Mesh All. HyperMesh creates a perfectly straight tria mesh down the length of the holes with no twisting.

3.

Click ACCEPT.

Step 6: Organize and clean up features. In the Organize and Cleanup Features step, you will highlight and organize features that require specific mesh controls beyond the overall mesh pattern that will be applied to the remainder of the part in a later step. You will use the organizational tool to place the required surfaces into their own collector or collectors, and set a mesh size and pattern requirements for each. 1.

In the panel area, click

.

2.

In the Define New dialog, enter Faces in the text field.

3.

Click OK.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

Select all five of the flat faces around the circumference of the part as indicated in the following image.

Isolated view of the five flat faces

5.

Click proceed. The Organize panel opens with the surfaces pre-selected and ready to move into a new component called grp_Faces.

6.

Click move.

7.

Click return.

8.

Click

9.

In the Define New dialog, enter TopHole in the text field.

.

10. Click OK. 11. Rotate the model so you are looking at it from underneath into the center. 12. Select the five surfaces that are shaded gray, as indicated the following image. Note:

You only need to select one of the two surfaces that make up a cylinder; when you click proceed HyperMesh automatically selects the other surfaces.

Proprietary Information of Altair Engineering

p.232

Altair HyperMesh 2019 Tutorials

p.233

13. Click proceed. 14. In the Organize panel, click move. 15. Click return. Note:

Your model should look similar to the following image, with the faces in one collector and the top hole in another. Your colors may vary slightly.

16. Click ACCEPT.

Step 7: Organize and clean up filets. Often a better mesh can be achieved if your fillets are split down the center. In the Organize and Cleanup Fillets step, you will split your fillets based on a minimum and maximum radius criteria. 1.

Click Components.

2.

Select the part in an area that has not been organized into a new component so that the large purple part is selected.

3.

Click proceed.

4.

Verify that the Min Radius is 0, and the Max Radius is 5.

5.

Select the Suppress fillet tangent edges checkbox.

6.

Click Cleanup. Note:

7.

Many of the fillets now have an edge running down the center and the original edges are suppressed.

Click ACCEPT.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.234

Step 8: Mesh features. In the Mesh Features step, you will mesh the features that you organized in step 6. The panel area will contain a table with your organized features. In the table, you will be able to select a mesh type and specify an element size for each feature. 1.

In the Feature Parameters Table, set the Mesh Type for Faces to trias.

2.

For TopHole, set the Mesh Type to R-tria union jack.

3.

For both features, enter 0.5 in the Elem Size field.

4.

Click Mesh All. Note:

5.

Notice the distinctive Union Jack mesh pattern ( ) in the top hole area and the connectivity of the mesh to the previously meshed holes.

Click ACCEPT.

Step 9: Organize and clean up. In the Organize and Cleanup step, you will organize and clean up the remaining portion of the model that will then fall under the global meshing parameters. As the remaining surfaces are already in the component you wish them to be in, there is no need for further organization. 1.

Click ACCEPT.

Step 10: Mesh/remesh. In the Mesh/Remesh step, you will globally mesh the remaining model. You can select a mesh type and specify an element size for all of the components that remain unmeshed. 1.

In the panel area, enter 1 in the Element Size field.

2.

Set Mesh Type to trias.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

Click Mesh.

4.

Click ACCEPT.

p.235

Step 11: Clean up elements. At this point the model should be entirely surface meshed. Proper adherence to the previous steps ensures a surface mesh that is properly connected and controlled by the previously entered values. In the Element Cleanup step, you will verify a proper mesh and clean up any issues that are found. 1.

In the panel area, click Components.

2.

Click comps.

3.

Select all of the components.

4.

Click select.

5.

Click proceed.

6.

Leave all of the values at their default (Min Size = 0.25, Max FeatureAngle = 60.0, and Normals Angle = 150.0).

7.

Click AutoCleanup. A dialog appears with a message that reads, "Cleanup process performed on 32 failed elements. No failed elements remain." Note:

This confirms that all failed edges have been fixed and there are no further errors in the model.

8.

Optional: Use the Manual tab to manually check the model for free edges and tjunctions, and fix any that are found. There is also an option to display normals. Use these options to find and fix any errors.

9.

Click ACCEPT. Note:

The Tetramesh Process Manager automatically places any elements that fail the AutoCleanup procedure in the user mark. This allows for easy retrieval of problem elements. You can employ the tools from the standard HyperMesh panels to fix these remaining elements.

Step 12: Tetra mesh. Tetra Meshing is the final step in the TetraMesh Process Manager Template. During this step, the model will be Tetra meshed. The Process Manager automatically opens the TetraMesh panel and pre-selects all of the float and fixed elements. 1.

Under Float trias/quads to tetra mesh, click elems. HyperMesh selects the surface elements under the general mesh selection option. Note:

This option defines the selected elements as “floatable”, meaning that the diagonals of the underlying tetra elements can be flipped from the generated shell elements if HyperMesh determines a better element quality will result.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

p.236

Under Fixed trias/quads to tetra mesh, click elems. HyperMesh selects the elements that represent the interior of holes and bores. Note:

The option defines the selected elements as “fixed”, meaning HyperMesh will always adhere to the shell mesh pattern when generating the tetra elements.

3.

Click mesh.

4.

From the Model browser, expand the Components folder.

5.

Right-click on tetmesh, and select Isolate Only from the context menu. Hypermesh displays the tetra mesh.

6.

Open the Mask panel by clicking

7.

Press Shift + left-click, and then drag a box to include roughly half of the model.

8.

Click mask. Note:

on the Display toolbar.

Your tetra mesh should look similar to the following image.

Step 13 (Optional): Save your work. You can now save your model if you wish. 1.

From the menu bar, click File > Save > Model.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Quality

Proprietary Information of Altair Engineering

p.237

4

Altair HyperMesh 2019 Tutorials

HM-3300: Checking and Editing Mesh In this tutorial, you will learn how to: •

Identify shell element connectivity problems

•

Correct shell element connectivity problems

•

Review the model’s shell elements to ensure connectivity problems were corrected

•

Remesh the elements along the rib

•

Use element quality Cleanup tools

Model Files This exercise uses the cover.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Retrieve and view the HyperMesh model file. 1.

Start HyperMesh Desktop.

2.

From the menu bar, click File > Open > Model.

3.

In the Open Model dialog, open the file cover.hm.

Step 2: Review the model’s free edges to identify shell element connectivity problems. 1.

To open the Edges panel, do one of the following: •

From the menu bar, click Mesh > Check > Components > Edges.

Proprietary Information of Altair Engineering

p.238

Altair HyperMesh 2019 Tutorials

p.239

•

On the Checks toolbar, click

•

From the main menu, go to the Tool page and click edges.

•

Press SHIFT + F3.

(Edges).

2.

Set the entity selector to comps.

3.

In the graphics area, select any element. HyperMesh selects the component containing the element you selected.

4.

Click find edges. HyperMesh creates a red 1D element along each shell element edge that is free (one or more of the nodes on the element's edges are not shared by the adjacent elements), and organizes them into a new component named ^edges. Note:

5.

If the first character of a component's name is ^, the component and its contents will not be written to the input file when the model is exported.

Observe the red, 1D elements (free edges), and try to identify gaps in the continuity of the mesh. Tip:

Look closely at the free edges interior to the model.

6.

In the Model browser, Component folder, click element display.

7.

Continue to identify which red, free edges do not belong in the model.

All of the red, free edges in the model

Proprietary Information of Altair Engineering

next to shells to turn off its

Red, free edges that belong in the model

Altair HyperMesh 2019 Tutorials

8.

Turn the element display back on for the shells component.

Step 3: Correct the shell element connectivity problems using the Edges panel. 1.

In the tolerance= field, enter 0.01.

2.

In the graphics area, select any element. HyperMesh selects the component containing the element you selected.

3.

Click preview equiv. HyperMesh creates a sphere ( ) on the nodes that have a distance between each other that is equal to or less than the specified tolerance. Note:

4.

The Status bar reads, "81 nodes were found." A sphere was not created on every node along all of the red, free edges. To identify the rest of the nodes, you must specify a larger tolerance.

In the tolerance = field, increase the value until you have identified all 96 nodes. Note:

Do not increase the tolerance too much. Although you will identify the 96 nodes, an excessively large tolerance value may collapse elements when the identified nodes are equivalenced.

Tip:

Find the maximum tolerance value that you can safely use without collapsing the elements by pressing F10 to go to the Check Elems panel, 2d subpanel, and clicking length. The Status bar reads "… The min length is 1.49." This message indicates that you can safely use a tolerance value < 1.49, without causing any elements to collapse when identified nodes are equivalenced. Return to the Edges panel by clicking return.

The nodes identified with preview equivalence

5.

Click equivalence. HyperMesh equivalenced 96 coincident nodes.

6.

Rotate and observe the model to see that the mesh still looks as it should, and that none of the elements are collapsed.

7.

Click delete edges. HyperMesh deletes the red, free edges and their component, ^edges.

Proprietary Information of Altair Engineering

p.240

Altair HyperMesh 2019 Tutorials

p.241

Step 4: Review the model’s free edges again to confirm that all of the shell element connectivity problems have been corrected. In this step, you should still be in the Edges panel. 1.

Click find edges. HyperMesh creates a red, 1D element along each shell element edge that is free.

2.

Observe the red, 1D elements (free edges). Are there any red, free edges that should not belong if the mesh was continuous, or if all of the elements were connected? Note:

Red, free edges should only exist on the perimeter of the part and on the periphery of the internal holes.

3.

In the Model browser, turn off the element display of the shells component.

4.

Verify that all of the free, red edges belong in the model.

Red, free edges that belong in the model

5.

Click delete edges.

6.

Turn the element display back on for the shells component.

7.

Click return.

Step 5: Display the element normals and adjust them to point in the same direction. 1.

2.

To open the Normals panel, do one of the following: •

From the menu bar, click Mesh > Check > Elements > Normals.

•

On the Checks toolbar, click

•

From the main menu, go to the Tool page, then click normals.

•

Press SHIFT + F10.

Go to the elements subpanel.

Proprietary Information of Altair Engineering

(Normals).

Altair HyperMesh 2019 Tutorials

3.

Set the toggle to vector display.

4.

Set the top switch to comps.

5.

In the graphics area, select any element. HyperMesh selects the component containing the element you selected.

6.

Click display. HyperMesh draws vectors from the element centroids, which indicate the direction of the element normals. Note:

7. 8.

The arrows do not all point from the same side of the part. For some analyses, the element normals should point from the same side.

In the size = field, enter the size which the normal should be in model units. Note:

p.242

When size = is set to 0, the vector will be 10% of the screen.

Click display.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

9.

Toggle vector display to color display.

10. Click display. HyperMesh displays, on each side of the part, the element normals using the colors red and blue. Note:

The red side of the elements is the positive normal direction, while the blue side is the negative normal direction.

11. Under orientation, set the switch to elem. 12. In the graphics area, select an element as indicated in the following image.

13. Click adjust. All of the elements on both sides of the part are the same color, red or blue. Note:

The Status bar reads: "[X] elements have been adjusted."

Proprietary Information of Altair Engineering

p.243

Altair HyperMesh 2019 Tutorials

p.244

14. Optional: If after adjusting the normals there are still elements on one side of the part which are of different color, set the switch to elem under Orientation, select the elements that are of a different color, and then click reverse. 15. Click return.

Step 6: Review the quality of the elements using the check elems panel. 1.

To open the Check Elems panel, do one of the following: •

From the menu bar, click Mesh > Check > Elements > Check Elements.

•

On the Checks toolbar, click

•

From the main menu, go to the Tool page, then click check elems.

•

Press F10.

(Check Elements).

2.

Go to the 2-d subpanel.

3.

Verify that the jacobian < field is set to 0.7.

4.

Click jacobian. HyperMesh highlights the elements that have a jacobian of less than 0.7, and the Status bar displays a message indicating how many elements failed this check. Note:

There are several elements on the triangular rib and around the smaller of the two holes that have a jacobian of less than 0.7.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

5.

In the graphics area, click an element. A window appears that lists each quality check result for the element.

6.

Close the pop-up window by right-clicking.

7.

On the right side of the panel, switch from standard to assign plot.

8.

Click jacobian. A legend for jacobian values appears and each element is colored accordingly. Note:

The red elements have a jacobian less than the threshold, 0.7.

Proprietary Information of Altair Engineering

p.245

Altair HyperMesh 2019 Tutorials

9.

Under quads, verify that the min angle < is set to 45.

10. Click min angle to determine if any quad elements have an angle of less than 45. Note:

A couple of the elements on the rib have an angle of less than 45.

11. Under quads, verify that the max angle > field is set to 135. 12. Click max angle. Note:

Several elements on the rib have an angle greater than 135.

Proprietary Information of Altair Engineering

p.246

Altair HyperMesh 2019 Tutorials

13. Click return.

Proprietary Information of Altair Engineering

p.247

Altair HyperMesh 2019 Tutorials

Step 7: Remesh the elements on the rib using the Automesh panel. 1.

To open the Automesh panel, do one of the following: •

From the menu bar, click Mesh > Create > 2D AutoMesh.

•

From the main menu, go to the 2D page and click automesh.

•

Press F12.

2.

Go to the size and bias subpanel.

3.

Set the entity selector to elems.

4.

At the bottom of the panel, set the toggle to interactive.

5.

In the element size= field, enter 3.5.

6.

In the graphics area, select one rib element as indicated in the following image.

7.

Select one element on the plane of elements perpendicular to the rib and in the same plane as the rib’s shortest edge as indicated in the following image..

Example of elements to select

8.

Complete your selection of elements by clicking elems >> by face.

Elements selected using by face

Proprietary Information of Altair Engineering

p.248

Altair HyperMesh 2019 Tutorials

9.

Click mesh. The meshing module opens.

10. In the density subpanel, left-click on the rib’s hypotenuse edge density number to increase it to 9 as indicated in the following image.

11. Left-click on the rib’s shortest edge density number to increase it to 5 as indicated in the following image.

Proprietary Information of Altair Engineering

p.249

Altair HyperMesh 2019 Tutorials

12. Keep all of the other element edge densities the same. 13. Go to the mesh style subpanel. 14. Under mesh method, set the last option to free (unmapped). 15. Under mesh method, click set all. 16. Preview the mesh by clicking mesh.

17. Go to the checks subpanel. 18. Check the jacobian, quads: min angle, and quads: max angle. Note:

None of the elements failed the minimum and maximum angle checks, and only a couple of the elements have a jacobian of less than 0.7. The smallest jacobian is 0.68, which can still be considered good quality.

19. Accept the mesh and return to the main menu by clicking return.

Proprietary Information of Altair Engineering

p.250

Altair HyperMesh 2019 Tutorials

Step 8: Use the Smooth panel to adjust the node placement on the rectangular plane of the remeshed elements. 1.

Open the Smooth panel by clicking Mesh > Cleanup Elements > Smooth.

2.

Go to the plates subpanel.

3.

Activate the smooth: elems selector.

4.

Select an element on the rectangular plane of the remeshed elements.

5.

Click elems >> by face.

6.

In the iterations= field, enter 10.

7.

Switch the smoothing algorithm from autodecide to shape corrected.

8.

Click smooth.

9.

Click return.

Proprietary Information of Altair Engineering

p.251

Altair HyperMesh 2019 Tutorials

Step 9: Remove tria elements from another area of the model using the edit element panel, split and combine subpanels. 1.

Go to the 2D page.

2.

Click edit element.

3.

Go to the split subpanel.

4.

Verify that the splitting line: points selector is active.

5.

Click the four screen points as indicated in the following image. HyperMesh draws temporary line segments to connect the points. Tip:

6.

Right-click to undo the last line segment drawn, or click delete line to start over and reselect points.

Click split. HyperMesh splits the elements that have a line passing through them. Note:

The resulting mesh should look like the mesh in the following image, with two pairs of adjacent tria elements.

Proprietary Information of Altair Engineering

p.252

Altair HyperMesh 2019 Tutorials

7.

Go to the combine subpanel.

8.

Set the toggle to combine to quad.

Proprietary Information of Altair Engineering

p.253

Altair HyperMesh 2019 Tutorials

9.

Select the two adjacent tria elements as indicated in the following image.

10. Click combine. HyperMesh combines the two tria elements into one quad element.

11. Repeat 11.9 and 11.10 to combine the other two tria elements into one quad element.

Proprietary Information of Altair Engineering

p.254

Altair HyperMesh 2019 Tutorials

12. Click return.

Step 10: Modify washer radius and optimize element quality by using Cleanup tools. 1.

From the 2D page, click qualityindex.

2.

Click cleanup tools.

3.

Click modify hole & washers.

4.

Clear the edit checkbox.

5.

Select a node on the washer as indicated in the following image. The radius field displays a value of 5.98.

6.

Select the edit check box.

7.

In the radius field, enter 7.

8.

Select the link washers checkbox.

9.

Select the remesh number of layers checkbox, and then enter 3 in the editable field.

Proprietary Information of Altair Engineering

p.255

Altair HyperMesh 2019 Tutorials

p.256

10. Select a node on the washer as indicated in the previous image. HyperMesh changes the washer's radius to 7. Note:

Because you selected the link washers checkbox, the hole's radius will change accordingly (approx. 4.68). Due to the change in the hole's and washer's dimensions, elements around the washer will be distorted and will fail in quality. You can correct all of the failed elements in the model using the node optimize and element optimize cleanup tools.

11. Click node optimize. 12. Select a few nodes on the elements that you modified in step 9. When you select a node, HyperMesh repositions it so that the elements attached to the node will have the best possible quality based on the criteria specified in the Quality Index panel. 13. Click element optimize. 14. Select the red and yellow elements in the model. When you select an element, HyperMesh adjusts it to have the best quality possible based on the criteria specified in the Quality Index panel. Note:

If you select a red element, it may turn yellow or it may no longer have a color assigned. If you select a yellow element, it may no longer have a color assigned.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

15. Click drag tria element. Note:

Use the drag tria element tool to drag a tria element toward a different location in the model, or out of the model completely.

16. Left-click on a tria element and drag it toward the bottom edge of the model until it is out of the model completely. HyperMesh highlights the selected tria element in pink.

17. Click return.

Step 11: Add a ring of radial elements around the smaller of the two holes. 1.

Open the Utility tab by clicking View > Browsers > HyperMesh > Utility from the menu bar.

2.

Click Geom/Mesh.

3.

Click Add Washer.

4.

In the Add Washer along Circular Holes dialog, double-click Nodes.

Proprietary Information of Altair Engineering

p.257

Altair HyperMesh 2019 Tutorials

5.

Select one of the nodes on the edge of the smaller hole as indicated in the following image.

Proprietary Information of Altair Engineering

p.258

Altair HyperMesh 2019 Tutorials

6.

Click proceed. HyperMesh selects nodes around the hole.

7.

Under Selection, set the toggle to Width.

8.

Under Value, enter 3.0.

9.

Select the Minimum number of nodes around the hole checkbox.

10. In the Density field, enter 12.

Settings in the Add Washer along Circular Holes dialog

Proprietary Information of Altair Engineering

p.259

Altair HyperMesh 2019 Tutorials

p.260

11. Click Add. HyperMesh creates a washer around the hole.

12. Click Close.

Step 12: Imprint Mesh to different destinations. 1.

In the Model browser, Component folder, right-click on IMPRINT1 and select Show from the context menu.

2.

Go to the 2D page.

3.

Click mesh edit.

4.

Go to the imprint subpanel. Note:

Use the imprint subpanel to sync or line up different, overlapping component's meshes in order to facilitate a better connection modeling between the components.

5.

Verify that the source selector is set to comps, and then select the IMPRINT1 component.

6.

Verify that the destination selector is set to comps, and then select the shells component.

7.

From the remain drop-down list, select destination. Note:

This option takes existing elements/components that can be imprinted into destination elements/components, and changes their direction and destination.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Original: Violet elements are offset from yellow.

8.

Clear the elems to destination comp checkbox.

9.

Click create.

Violet source elements are imprinted in destination (yellow).

10. Click reject. 11. Repeat steps 12.5 and 12.6 to select the IMPRINT1 component as the source and the shells component as the destination. 12. From the remain drop-down list, select destination. 13. Select the elems to destination comp check box.

Violet source elements are imprinted in destination (yellow), element organized into yellow component.

Proprietary Information of Altair Engineering

p.261

Altair HyperMesh 2019 Tutorials

14. Click reject. 15. Repeat steps 12.5 and 12.6 to select the IMPRINT1 component as the source and the shells component as the destination. 16. From the remain drop-down list, select source. 17. Select the elems to destination comp checkbox. 18. Click create.

Yellow destination elements are imprinted to Violet elements, and elements are organized into the yellow component.

19. Click reject 20. Click return.

Step 13: Extend Mesh to different destinations. 1.

In the Model browser, Component folder, right-click on IMPRINT1 and select Hide from the context menu.

2.

Right-click on the EXTEND component and select Show from the context menu.

3.

From the 2D page, click mesh edit.

4.

Go to the extend subpanel. Note:

5.

Use the extend subpanel to create smoothly-meshed connections between different components that do not quite touch, but are meant to. Mesh can be imprinted such that both components are remeshed to match, or the source component is remeshed to match the destination component, and vice-versa. In addition, you can merge the elements of the source component into the destination component.

Click source: nodes >> by path.

Proprietary Information of Altair Engineering

p.262

Altair HyperMesh 2019 Tutorials

6.

On the EXTEND component, select the source nodes indicated in the following image.

7.

Verify that the destination selector is set to comps, and then select the shells component.

8.

From the projection list, select along vector.

9.

Activate the N1 selector.

10. Select N1 and N2, as indicated in the following image, to define the direction.

11. Clear the remesh extension checkbox.

Proprietary Information of Altair Engineering

p.263

Altair HyperMesh 2019 Tutorials

12. Click create. HyperMesh connects the two parts with one element along the projection, because the remesh extension checkbox was clear.

13. Click reject. 14. Repeat step 13.5 and 13.11, but select the remesh extension checkbox. 15. Click create. HyperMesh connects the two parts with remeshed elements along the projection, because the remesh extension option was selected.

Step 14 (Optional): Save your work. With this exercise completed, you can save the model if desired. 1.

From the menu bar, click File > Save > Model.

Proprietary Information of Altair Engineering

p.264

Altair HyperMesh 2019 Tutorials

p.265

HM-3320: Penetration In this tutorial, you will learn how to: •

Run the penetration check

•

Review the intersection results

•

Fix the intersection results

•

Interrogate the penetration results

•

Fix the penetration results

Tools To access the Penetration panel: •

From the menu bar, click Mesh > Check > Components > Penetration.

•

From the Tool page, select penetration.

Use the Penetration panel to check the integrity of your model, visualize problem areas, and fix problem areas. You can check elements, components and groups. Typically you would use the group check to check contact definitions (for example, Abaqus/LS-DYNA).

You can also use this panel to check components for element penetration and intersection. Penetration and intersection can be used individually or collectively. Penetration is defined as the overlap of the material thickness of shell elements, while intersection is defined as elements passing completely through one another.

Example of penetration

Proprietary Information of Altair Engineering

Example of intersection

Altair HyperMesh 2019 Tutorials

Strategy Use the following guidelines for conducting checks: •

Checks can be run on both 2D and 3D elements, 2D elements only, or 3D elements only.

•

Select include self interference to include components that bend and pass through themselves. This occurs rarely and is expensive when running the check. By default, this checkbox is cleared.

•

By default the check is set to all interferences, meaning both intersection and penetration. The intersections only option and the penetrations only option are also available.

•

Select allowable interference depth to ignore penetrations and intersections that are less than the value specified. By default, this checkbox is cleared.

•

Select uniform thickness to assign a global thickness to all components.

•

Select thickness multiplier to multiply the existing thicknesses in the model.

When the penetration check is invoked, a new penetration tab opens in the browser area.

The results are split into intersections and penetrations with the number of components that are clashing in brackets. In the example below, two components are intersecting

Proprietary Information of Altair Engineering

p.266

Altair HyperMesh 2019 Tutorials

and eleven components have material penetration. Expand each section for more detail as to which components have failed. The ID, Elems, Depth, and Comps columns provide information on which components' IDs are involved, the number of failed elements, the depth of penetration (not applicable for intersections), and the number of components affected in the penetration/intersection. Each of the columns can be sorted by clicking the column header. At the bottom of the tab area there is a message bar which will detail the status of the check, the number of failed elements, and any warnings and errors as the checks are invoked.

Access additional options and tools within the penetration and intersection check by right-clicking in the Penetration tab. A context menu will appear and provide additional options to fix either penetrations or intersections, depending on whether the penetration parent/child folder or intersection folder has been highlighted.

Proprietary Information of Altair Engineering

p.267

Altair HyperMesh 2019 Tutorials

Click Options to configure the display of the tab, fix intersections and penetrations, and change the display of depenetration vector.

The fixing of penetrations and intersections falls into two categories: automatic and manual. These capabilities will be discussed in more detail in the tutorial.

Model Files This exercise uses the penetration_check.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Proprietary Information of Altair Engineering

p.268

Altair HyperMesh 2019 Tutorials

p.269

Exercise

Step 1: Retrieve the model file, penetration_check.hm. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select LsDyna. Note:

This model is a LS-DYNA model, therefore, it is important to select the appropriate user profile so that HyperMesh can access the actual thickness values of the shell components. The thickness values are required for material penetration check.

3.

Click OK.

4.

From the menu bar, click File > Open > Model.

5.

In the Open Model dialog, open the penetration_check.hm file. A model appears in the graphics area.

6.

On the Visualization toolbar, click lines.

7.

Observe the model using various visualization options available in HyperMesh (rotation, zooming, and so on).

to shade the model's elements and mesh

Step 2: Run the penetration check. 1.

Open the Penetration panel by clicking Mesh > Check > Components > Penetration from the menu bar.

2.

Click comps.

3.

Select all of the components listed.

4.

Click select.

5.

Click check. Once the check is complete, the Penetration tab populates with two intersections and 11 penetrations. The tab is populated by a parent/child or master/slave relationship. As an example, looking at the intersections, the top line shows the component Rocker Fwd Top Panel RH (parent), and then below is component Rocker Inner Panel RH (child). It is important to understand that there is always a reciprocal relationship; the second entry is Rocker Inner Panel RH (parent) and then the component Rocker

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Fwd Top Panel RH (child). In this case there is a one-to-one relationship. It is especially important to understand this when there is a one-to-many relationship (for example, Rocker Inner Panel RH under penetrations). Clicking the parent component will always show that component plus all the components below (children). Clicking a child component will show that component with the parent component only.

Step 3: Review the intersection results. 1.

View all of the intersections by expanding Intersections in the Penetration tab. Note: Mod e

Based on which mode is chosen, certain components are displayed on the screen. Description

Fit View to Failed Elements Display All Elements Display Components with Failed Elements Display Only Failed Elements

Proprietary Information of Altair Engineering

p.270

Altair HyperMesh 2019 Tutorials

p.271

2.

Select (Display Components with Failed Elements) and Failed Elements).

(Fit View to

3.

Under Intersections, in the Rocker Fwd Top Panel RH folder, select the Rocker Inner Panel RH component. HyperMesh automatically fits the screen to the failed intersecting elements.

4.

Review other visualization modes by clicking (Review Failed Elements). The contour and vector displays are only applicable to intersections. The intersecting elements display as follows:

Step 4: Fix the intersection results. HyperMesh includes two methods for fixing intersections: manual and automatic. To fix intersections manually: 1.

Under Intersections, in the Rocker Inner Panel RH folder, select the Rocker Fwd Top Panel RH component.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

3.

Ensure that the intersecting entities can be fixed by clicking Note:

Additional tools display for intersection fixing.

Click

(Elements from Tree Selection).

Note:

You will not pick any additional elements.

p.272

(Manual Fix Tools).

(Move in Normal Direction) for the direction of movement.

4.

Click

5.

For distance value, enter 2.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

Click

twice. HyperMesh moves the selected elements in the chosen direction.

Note:

After the elements have been moved by a value of 4, they no longer intersect.

7.

Click

(Recheck).

8.

In the dialog that appears, which reads "Current intersection/penetration results will be lost by rechecking the model. Would you like to continue?", click Yes. Note:

There are no intersections, and only 11 penetrations remain.

Alternatively, you can use the automatic fixing tools: 1.

Reload the file, penetration_check.hm, again.

2.

Go to the Penetration panel.

3.

Click comps.

4.

Select all of the components listed.

5.

Click select.

6.

Click check. Once the check is complete, the Penetration tab populates with two intersections and 11 penetrations.

7.

In the Penetration tab, right-click on the Intersections and select Automatic Recursive Intersection Fix from the context menu.

Proprietary Information of Altair Engineering

p.273

Altair HyperMesh 2019 Tutorials

8.

In the dialog that appears asking if you would like to continue, click Yes. Note:

Automatic Recursive Intersection Fix automatically runs through all of the passes, whereas the Automatic Intersection Fix runs through one pass at a time. Most fixes require multiple passes.

Step 5: Interrogate the penetration results. 1.

Expand Penetrations.

2.

Select the component, C-Pillar Bot Inner Panel RH. The penetration results will look as follows:

Proprietary Information of Altair Engineering

p.274

Altair HyperMesh 2019 Tutorials

3.

View different types of display results for penetration by clicking the following visualization options: .

contour

vectors

Remember that the columns can be sorted. For example, if you were only interested in the worst offending penetrations then sorting by the depth column will reorganize the tree structure, while still retaining the parent/child relationship. In this particular example, for component C-Pillar Bot Inner Panel RH, there are 18 elements that have failed (parent and child), the maximum penetration depth is 0.159, and there is only one component penetrating.

Step 6: Fix the penetration results. Within the checking tool there is an automatic penetration fix that will remove the penetrations within the model. This works by physically moving the failed nodes to new locations to remove the material penetration. There are two options: automatic penetration fix and automatic recursive penetration fix. Both will do the same thing, but the automatic option often requires you to use it several times successively to eliminate all penetrations, while the automatic recursive completes the fix in one click. However, the iterative option will take longer to complete, because it is essentially

Proprietary Information of Altair Engineering

p.275

Altair HyperMesh 2019 Tutorials

automatically repeating the automatic fix until it reaches a point at which no further improvements can be made. You also have the option to either fix individual penetrations by clicking on a single parent branch of the tree, or fix all penetrations at once by clicking and highlighting the complete Penetrations tree. In some circumstances, there may be the need to lock or freeze a component that cannot be adjusted or moved by the fixing tool. To achieve this, right-click on the component and select Lock Component from the context menu. Once a component is locked, a symbol will appear by the folder indicating that the component is locked.

In the previous example, you locked the component, C-Pillar Bot Inner Panel RH. The lock symbol appears multiple times to correspond with the multiple references to the same component. To unlock the component, right-click again on the locked component and select Unlock Component from the context menu. For the purpose of this tutorial you will not be using the lock functionality. To fix the penetrations in the model you will use the Iterative Fix:

Proprietary Information of Altair Engineering

p.276

Altair HyperMesh 2019 Tutorials

1.

In the Penetrations tab, right-click on Penetrations and select Automatic Recursive Penetration Fix from the context menu.

2.

In the dialog that appears, asking if you would like to continue, click Yes. Note:

After the process has finished, a majority of the penetrations have been fixed. Three penetrations remain which require manual editing to fix.

Proprietary Information of Altair Engineering

p.277

Altair HyperMesh 2019 Tutorials

Assembly

Proprietary Information of Altair Engineering

p.278

5

Altair HyperMesh 2019 Tutorials

HM-3400: Creating Connectors In this tutorial, you will learn how to: •

Weld the two front trusses to each other by creating connectors at pre-defined weld points

•

Weld the two front trusses to the reinforcement plate by creating connectors between shell elements

•

Weld the right rails to each other and to the front trusses by creating connectors from a master connectors file

•

Update weld type of NASTRAN/OPTISTRUCT ACM (area contact method) welds, which already connect the rear trusses to each other, by first creating connectors from these welds and then realizing the connectors into two-noded weld elements.

Model Files This exercise uses the frame_assembly.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise Weld the two front trusses by creating connectors between geometry surfaces at predefined weld points.

Proprietary Information of Altair Engineering

p.279

Altair HyperMesh 2019 Tutorials

p.280

Step 1: Retrieve and view the model file. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select OptiStruct.

3.

Click OK.

4.

Open a model file by clicking File > Open > Model from the menu bar, or click the Standard toolbar.

5.

In the Open Model dialog, open the frame_assembly.hm file. A model appears in the graphics area.

6.

On the Visualization toolbar, click edges.

7.

Observe the model using various visualization options available in HyperMesh (rotation, zooming, and so on).

on

to shade your model's geometry and surface

Step 2: Display only the assembly assem_1 for elements and geometry. 1.

In the Model browser, click

2.

Expand the Assembly Hierarchy folder and sub-folders.

3.

Set the entity selection to Note:

4.

(Model View).

(Elements and Geometry).

This options turns on/off both elements and geometry when you perform rightclick operations in the Model browser.

Right-click on assem_1 and select Isolate from the context menu. HyperMesh only displays the components that are in the assem_1 assembly.

Step 3: Load the Connector Browser. 1.

Open the Connectors browser by clicking View > Browsers > HyperMesh > Connector from the menu bar.

2.

Review the layout of the Connector browser. Currently there are no components or connectors listed because there are no connectors in the model. Note:

Use the Connector browser to view and manage connectors. The top portion of the browser is referred to as the Link Entity browser, and it displays information about linked entities. The middle portion is referred to as the Connector Entity browser, and it contains a list of the connectors in your model. The bottom portion of the browser is referred to as the Connector Entity Editor, and it displays attributes assigned to the connector(s) selected in the Connector Entity browser. HyperMesh groups the connectors based on their connection type.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.281

Step 4: Create welds between the geometry for the two front trusses at the pre-defined weld points. Connectors can be created automatically or manually. The automatic approach creates and realizes connectors automatically. The manual approach allows you to create and realize connectors manually. Realization is the process in which the connector creates the weld entity. Use the Spot, Bolt, Seam, and Area panels to create connectors automatically within the Connector browser, and use the create and realize subpanels to create connectors manually. 1.

Verify that the current component is Con_Frt_Truss. Note:

The current component is always boldfaced in the Model browser, Component folder.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

Open the Spot panel by right-clicking in the Connector Entity browser and selecting Create > Spot from the context menu.

3.

Go to the spot subpanel.

4.

Set the location selector to points.

5.

Select the six pre-defined weld points by clicking points >> by collector.

6.

Select the component Con_Frt_Truss.

7.

Click select.

8.

Set the connect what selector to comps.

9.

Click comps.

p.282

10. Select the components Front_Truss_1 and Front_Truss_2. 11. Click select. 12. In the tolerance = field, enter 5. Note:

The connector will connect any selected entities within this distance of itself.

13. Click type= and select weld. 14. Under connect what, switch the toggle from elems to geom.

Spot panel settings for steps 4.4 through 4.14.

15. Click create. HyperMesh automatically creates and realizes six connectors (Status bar reads, "6 spot connectors created, 6 realized."), and organizes them as geometry (not elements) in the current component collector, Con_Frt_Truss. Note:

Green connectors indicate that the creation of the weld entity was successful. There are four states of connectors: realized (green ), unrealized (yellow ), failed (red ), and modified ( ). If connectors were created manually, the color of the connectors changes from yellow to green, which indicates that they are realized into weld elements. As mentioned above, if you create connectors automatically they will be green immediately as there is no interim unrealized (yellow) state.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.283

HyperMesh also adds fixed points to the surfaces at the ends of the weld elements to guarantee connectivity between the weld elements and the shell mesh that will be created on the surfaces.

Weld element with fixed points created on the surfaces

16. Click return.

Step 5: Review the Connector Browser. 1.

In the Connector Entity browser, expand the RBAR folder. Note:

The RBAR folder contains the six connectors that you just created. HyperMesh grouped all of them under RBAR because that is the type of connector created. Notice the IDs of the connectors in the Entities column, the Links of the connectors, and the State of the connectors. You may need to increase the size of the tab area to see the State column.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

In the Link Entity browser, right-click on Front_Truss_1 and select Find from the context menu. HyperMesh isolates the component in the graphics area and highlights the six connectors in the Connector Entity browser to indicate that these connectors have Front_Truss_1 as a link.

3.

Right-click on Front_Truss_1 and select Find Attached from the context menu. HyperMesh finds the components that are attached to Front_Truss_1 through the connectors. Note:

Front_Truss_1 and Front_Truss_2 are now both highlighted in the Link Entity browser, which indicates that they are displayed in the graphics area.

Proprietary Information of Altair Engineering

p.284

Altair HyperMesh 2019 Tutorials

p.285

Step 6: Create a shell mesh on the two front truss components. 1.

Open the AutoMesh panel by pressing F12.

2.

Go to the size and bias subpanel.

3.

Set the mesh mode to automatic. Note:

It may currently be set to interactive.

4.

Set the entity selector to surfs.

5.

Click surfs >> displayed.

6.

In the elem size = field, enter 10.

7.

Set the mesh type to mixed.

8.

Set the elems to surf comp/elems to current comp toggle to elems to surf comp.

9.

Click mesh. HyperMesh meshes the surfaces.

10. Zoom into the area with a connector and note how the fixed point created from the weld has ensured that the mesh seeding passes through the weld. 11. Click return.

Step 7: Display only the assembly assem_2 for elements and geometry. In this step you will display the reinforcement plate that needs to be welded to the two front trusses. 1.

In the Model browser, set the entity selection to

(Elements and Geometry).

2.

Right-click on assem_2 and select Isolate from the context menu.

Weld the two front trusses to the reinforcement plate.

Step 8: Create connectors between the shell mesh of the front trusses and the reinforcement plate at pre-defined points. In this step you will manually create connectors between the shell elements of the front trusses and reinforcement plate at pre-defined weld points. 1.

In the Model browser, Component folder, right-click on Con_Truss_Plate and select Make Current from the context menu.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

Open the Spot panel.

3.

Go to the create subpanel.

4.

Set the location selector to points.

5.

Click points >> by collector

6.

Select the component Con_Truss_Plate.

7.

Click select.

8.

Set the connect what selector to comps.

9.

Click comps.

10. Select the components: Front_Truss_1, Front_Truss_2, and Reinf_Plate. 11. Click select. 12. Under connect what, switch the toggle from geom to elems. 13. Set the num layers to total 2. 14. Set connect when to now. 15. Click create. HyperMesh creates eight spot connectors with comp links (Status bar reads "8 spot connectors created with comps links.") at the selected weld points, and organizes them into the current component collector, Con_Truss_Plate. Note:

In the Connector Entity browser, these eight connectors are currently grouped as undefined.

16. In the Connector Entity browser, expand the undefined folder. Note:

The connectors in this folder are colored yellow, which indicates that they are unrealized.

Step 9: Realize the connectors in the component Con_Truss_Plate into weld elements. In this step you will realize the undefined, unrealized connectors and assign them a connector type. 1.

In the Connector Entity browser, select the following unrealized connectors: 7, 8, 11, and 12. Hint:

These connectors are displayed along the top of the Reinf_Plate component.

Proprietary Information of Altair Engineering

p.286

Altair HyperMesh 2019 Tutorials

2.

In the Entity Editor: •

Set Config Name to weld.

•

For Tolerance, enter 7.

•

Set Connectivity to mesh dependent.

•

Set Adjust Option to adjust realization.

•

Set Adjust Realization to project and find nodes Note:

3.

The mesh has not been remeshed to connect the two components.

In the Connector Entity browser, select the four remaining unrealized connectors (9, 10, 13, 14). Hint:

5.

When this option is active, the nodes will be equivalenced if the realized finite element of the connector is coincident to a node of the shell mesh it is being connected to. If there are no suitable nodes present, the closest node of the element the projection is landing is connected.

In the Connector Entity browser, right-click on the selected connectors and select Rerealize from the context menu. The selected connectors realize into the weld elements. Note:

4.

p.287

These connectors are displayed along the bottom of the Reinf_Plate component.

In the Entity Editor: •

Set Config Name to weld.

•

For Tolerance, enter 7.

•

Set Connectivity to mesh dependent.

•

Set Adjust Option to adjust mesh.

•

Set Adjust mesh to remesh.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

p.288

In the Connector Entity browser, right-click on the unrealized connectors and select Rerealize from the context menu. HyperMesh realizes the selected connectors, and remeshes the mesh to connect the two components.

The two front trusses welded to the reinforcement plate with weld elements at the connectors

Step 10: Display only the assembly assem_3 for elements and geometry. 1.

In the Model browser, set the entity selection to

(Elements and Geometry).

2.

On the Visualization toolbar, click lines.

3.

Right-click on assem_3 and select Isolate from the context menu.

to shade your model's elements and mesh

Weld the two right rails to each other and to the two front trusses by creating connectors from a master connectors file.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.289

Step 11: Create connectors to connect the right rails to each other and to the front trusses by importing a master connectors file. 1.

From the menu bar, click File > Import > Connectors.

2.

In the Import tab, click

3.

In the Select connector file dialog, open the rails_frt_truss.mwf file.

4.

Click Import. HyperMesh imports connectors and organizes them into a new component, CE_Locations. Note:

in the File field.

It will take a few seconds for HyperMesh to import the connectors.

Step 12: Realize the connectors in the component CE_Locations into weld elements. 1.

In the Model browser, Component folder, right-click on CE_Locations and select Make Current from the context menu.

2.

In the Connector Entity browser, click the undefined folder. The Entity Editor opens and displays the undefined connector’s corresponding data.

3.

In the Entity Editor: •

Set Config Name to Weld.

•

For Tolerance, enter 7.

•

Set Connectivity to mesh dependent.

•

Set Adjust Option to adjust realization.

•

Set Adjust Realization to project and find nodes.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

p.290

In the Connector Entity browser, right-click on the selected connectors and select Rerealize from the context menu.

Right rails welded to each other and to the front trusses with weld elements at the connectors

Step 13: Display only the assembly assem_4 for elements and geometry. 1.

In the Model browser, set the entity selection to

(Elements and Geometry).

2.

Right-click on assem_4 and select Isolate from the context menu.

Weld to the two front trusses by duplicating and reflecting selected connectors created from the master connectors file

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 14: Create a new component collector to hold new connectors. 1.

In the Model browser, right-click and select Create > Component from the context menu. HyperMesh creates and opens a component in the Entity Editor. Note:

HyperMesh makes this new component, the current component.

2.

For Name, enter CE_Locations_Dup.

3.

Click the Color icon, and select a color.

Step 15: Duplicate the connectors created from the master connectors file and reflect them. 1.

In the Model browser, Component folder, right-click on CE_Locations and select Show from the context menu.

2.

Open the Reflect panel by clicking Connectors > Reflect > Connectors from the menu bar.

3.

Set the entity selector to connectors.

4.

Click connectors >> by collector.

5.

Select CE_Locations.

6.

Click select.

7.

Click connectors >> duplicate >> current comp. HyperMesh duplicates the displays the connectors, and organizes them into the current component, CE_Locations_Dup.

8.

Set the orientation selector to x-axis. Note:

9.

This is the axis normal to the plane of interest.

Specify a base node to reflect about by double-clicking B.

10. Click x=. HyperMesh activates the x=, y=, and z= fields. Note:

Their values are all 0.000 by default, which is the base point you want to reflect about.

11. Return to the reflect panel by clicking return. 12. Click reflect. HyperMesh reflects the connectors. 13. Click return. Note:

The connectors are yellow, which indicates that they are unrealized.

Proprietary Information of Altair Engineering

p.291

Altair HyperMesh 2019 Tutorials

Step 16: Update the connectors for the left rails to link them to the left rail components. 1.

In the Connector Entity browser, expand the RBAR folder.

2.

Sort the connectors by their state by clicking State. HyperMesh organizes all of the realized connectors at the top of the list. Tip:

You may need to increase the size of the tab area to see the State column.

3.

Click State again. HyperMesh organizes all of the unrealized connectors at the top of the list.

4.

In the Link1 and Link2 columns, review the the unrealized connectors. Note:

Some of the connectors are linked to the components, Right_Rail_1 and Right_Rail_2. This data is from the rails_frt_truss.mwf file that you imported. These links need to be updated to reflect the components, Left_Rail_1 and Left_Rail_2.

5.

Select all of the unrealized connectors in the list.

6.

In the Entities column, right-click on the selected connectors and select Update Link from the context menu.

7.

In the Update window, Search column, set the Link Type to comps.

8.

In the Search column, click the Link Select field.

9.

In the panel area, click component.

10. Select the component, Right_Rail_1. 11. Click proceed. HyperMesh inserts Right_Rail_1 into the Link Select field. 12. In the Replace column, set the Link Type to comps. 13. In the Replace column, click the Link Select field.

Proprietary Information of Altair Engineering

p.292

Altair HyperMesh 2019 Tutorials

p.293

14. In the panel area, click component. 15. Select the component, Left_Rail_1. 16. Click proceed. HyperMesh inserts Left_Rail_1 into the Link Select field.

17. Click Update. HyperMesh updates the connectors' links. 18. Repeat 16.7 through 16.17, except search for the Right_Rail_2 component and replace it with the Left_Rail_2 component. 19. Scroll through the list of unrealized connectors to make sure that none of the connectors are linked to the right rail components. 20. Close the Update window by clicking X next to Update.

Step 17: Realize the connectors in the component CE_Locations_Dup into weld elements. 1.

In the Connector Entity browser, select all of on the unrealized connectors, which are organized in the CE_Locations_Dup component. The Entity Editor opens and displays selected connector’s common attributes.

2.

In the Entity Editor:

3.

•

Set Config Name to weld.

•

For Tolerance, enter 7.

•

Set Connectivity to mesh dependent.

In the Connector Entity browser, right-click on the selected unrealized connectors and select Rerealize from the context menu. HyperMesh realizes the selected connectors into weld elements.

Step 18: Verify that all connectors are realized and identify the pairs of adjacent connectors. 1.

In the Connector Entity browser, expand the RBAR folder.

2.

From the State column, verify that all of the connectors are realized.

3.

Zoom into one of the two areas where the front trusses are connected to the rail components. Note: At these two areas, there are pairs of adjacent connectors.

4.

On the Visualization toolbar, click

Proprietary Information of Altair Engineering

(Visualization Options).

Altair HyperMesh 2019 Tutorials

p.294

5.

In the Visualization tab, click

6.

Under Color by, select Layer. HyperMesh changes the connectors color to purple because under Layers, 2t is defined by the color purple. Note:

(Connectors).

This option indicates that each of these connectors link two components. Because each pair of connectors creates a series of two weld elements, you can combine each pair into a single connector, which links the three components together.

Step 19: Isolate the pairs of adjacent 2t connectors identified in the previous step. 1.

In the Model browser, turn off the geometry display for all of the components.

2.

In the Link Entity browser, select Front_Truss_1, Front_Truss_2, Right_Rail_1, and Left_Rail_1.

3.

Right-click and select Find Between from the context menu. HyperMesh finds and displays 12 connectors between the four components you selected.

Step 20: Unrealize the displayed connectors. 1.

Open the Unrealize panel by clicking Connectors > Unrealize from the menu bar.

2.

Click connectors >> displayed. Note:

The Status bar reads "12connectors added by 'displayed'. Total selected 12."

3.

Click unrealize. HyperMesh unrealizes the connectors, and deletes the weld elements associated to them.

4.

Click return.

Step 21: Combine the pairs of adjacent 2t connectors into 3t connectors. 1.

Open the Connector Quality panel by clicking Connectors > Check > Connector Quality from the menu bar.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.295

2.

Go to the connectors (unrealized) subpanel.

3.

Click connectors >> displayed.

4.

In the tolerance = field, enter 7.

5.

Click preview combine. HyperMesh finds 12 connectors that need to be combined. Note:

6.

The status bar reads, "12 connector(s) found that need to be combined."

Click combine. HyperMesh combines the connectors, and displays them in a dark blue color to indicate that they have three layers. Note:

The status bar reads, "6 connectors deleted."

7.

Optional: If the connectors are not visible, right-click in the Link Entity browser and select Find Between.

8.

Click return.

Step 22: Realize the 3t connectors in the component Con_Frt_Truss into weld elements. 1.

In the Model browser, Component folder, right-click on Con_Frt_Truss and select Make Current from the context menu.

2.

In the Connector Entity browser, select the 6 unrealized connectors. The Entity Editor opens and displays the selected connector’s common attributes.

3.

In the Entity Editor: •

Set Config Name to weld.

•

For Tolerance, enter 10.

•

Set Connectivity to mesh dependent.

4.

In the Connector Entity browser, right-click on the selected connectors and select Rerealize from the context menu. HyperMesh realizes the connectors.

5.

Verify that there are now three links for the six connectors you just updated.

6.

On the Visualization toolbar, click

7.

In the Visualization tab, click

8.

Under Color by, select State.

(Visualization Options).

(Connectors).

Step 23: Display only the assembly assem_5 for elements and geometry. 1.

In the Model browser, set the entity selection to

(Elements and Geometry).

2.

Right-click on assem_5 and select Isolate from the context menu.

Step 24: Create connectors from existing ACM welds. In this step you will use the Fe Absorb tool to obtain connectors from the existing ACM welds (elements) in the component, Con_Rear_Truss.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

1.

From the menu bar, click Connectors > Fe Absorb.

2.

In the Automated Connector Creation and FE Absorption dialog, set FE configs to custom.

3.

Set FE type to optistruct 5 sealing.

4.

Toggle the Elem filter from All to Select.

5.

Double-click Elements.

6.

In the panel area, click elems >> by collector.

7.

Select the component, Con_Rear_Truss.

8.

Click select.

9.

Click proceed.

10. Select the Move connectors to FE component checkbox. 11. Click Absorb. HyperMesh absorbs the elements into realized, 2t connectors at the locations of the ACM welds, and organizes them into the Con_Rear_Truss component, the same component to which the ACMs belong.

12. Click Close.

Proprietary Information of Altair Engineering

p.296

Altair HyperMesh 2019 Tutorials

p.297

HM-3410: Creating Area Connectors In this tutorial, you will learn how to apply an adhesive connection to the left rails. S

Model Files This exercise uses the frame_assembly_1.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise Area connectors must be meshed in order to work properly. When the connector’s location is existing FE mesh elems, the connector automatically gets meshed to match the elements chosen. However, after creating an area connector on surfs, lines, or along nodes, you must use the automesh options (which display when you select one of these locations types) to create a mesh on the connector area. •

area

Create and realize area connectors in a single process.

•

create

Create, but not realize, area connectors.

•

realize

Create FE representations of previously-created area connectors.

Step 1: Retrieve and view the model file. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select OptiStruct.

3.

Click OK.

4.

Open a model file by clicking File > Open > Model from the menu bar, or clicking on the Standard toolbar.

5.

In the Open Model dialog, open the frame_assembly_1.hm file. A model appears in the graphics area.

6.

Observe the model using various visualization options available in HyperMesh (rotation, zooming, and so on).

Step 2: Load the Connector Browser. 1.

Open the Connectors browser by clicking View > Browsers > HyperMesh > Connector from the menu bar.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

Review the layout of the Connector browser. Currently there are no components or connectors listed because there are no connectors in the model. Note:

You can use the Connector browser to view and manage the connectors in your model. The top portion of the browser is referred to as the Link Entity browser, and it displays information about the linked entities in your model. The middle portion is referred to as the Connector Entity browser, and it contains a list of the connectors in your model. The bottom portion of the browser is referred to as the Connector Entity Editor, and it displays attributes assigned to the connector(s) selected in the Connector Entity browser. HyperMesh groups the connectors based on their connection type.

Step 3: Create an adhesive connection between component Left_Rail_1 and Left_Rail_2 on the top flange. 1.

In the Model browser, Components folder, isolate Left_Rail_1 and Left_Rail_2.

2.

Zoom into an area displaying the two flanges and inspect the elements to be joined.

3.

In the Model browser, right-click and select Create > Component from the context menu. HyperMesh creates and opens a component in the Entity Editor. Note:

HyperMesh makes this new component, the current component.

Proprietary Information of Altair Engineering

p.298

Altair HyperMesh 2019 Tutorials

4.

For Name, enter area_edit_panel.

5.

Open the Area panel by right-clicking in the Connector Entity browser and selecting Create > Area from the context menu.

6.

Set the location selector to elems.

7.

Select one element on the top flange of the Left_Rail_1 component as indicated in the following image.

8.

Click elems >> by face. HyperMesh selects the entire flange.

9.

Set the connect what selector to comps.

10. Click comps.

Proprietary Information of Altair Engineering

p.299

Altair HyperMesh 2019 Tutorials

11. Select the components, Left_Rail_1 and Left_Rail_2.

12. Click select. 13. In the tolerance= field, enter 10. Note:

The connector will connect any selected entities within this distance of itself.

14. Click type= and select adhesives. 15. Set the hexa thickness to shell gap. Note:

This option projects directly to the shell component and takes no account of the thickness of the shell components.

16. Click create. HyperMesh creates a new adhesive area connector. 17. Click return. 18. Inspect the new adhesive. 19. In the Connector Entity browser, right-click on the adhesive connector and select Unrealize from the context menu. The connector becomes unrealized, and the Entity Editor opens and displays the selected connectors corresponding attributes. 20. In the Entity Editor: •

Set Hexa Thickness Option to (T1+T2)/2. Note:

•

(T1+T2)/2 takes into account the thickness of each shell part.

For Coats, enter 3. Note:

This option increases the number of hexas through thickness from 1 to 3.

Proprietary Information of Altair Engineering

p.300

Altair HyperMesh 2019 Tutorials

21. In the Connector Entity browser, right-click on the unrealized adhesive connector and select Rerealize from the context menu.

For the other set of flanges you will manually create an area connector and mesh it accordingly.

Step 4: Create an adhesive connection between component Left_Rail_1 and Left_Rail_2 on the bottom flange. 1.

Go to the area panel.

2.

Set the location selector to nodes.

3.

Click node list >> by path.

4.

Select the row of nodes on the outer flange of the Left_Rail_1 component by first selecting the left most node on the bottom flange of Left_Rail_1 and then selecting the right-most node on the bottom flange as indicated in the following image.

5.

In the width= field, enter 10.

6.

In the offset= field, enter 3.

7.

Next to connect what, click comps.

8.

Select Left_Rail_1 and Left_Rail_2.

Proprietary Information of Altair Engineering

p.301

Altair HyperMesh 2019 Tutorials

9.

Click select.

10. Click create. Note:

The default mesh size for these mesh independent area connectors (when choosing by nodes/lines/surfs) is 10. However, you can specify a different elem size if needed.

11. Go to the edit subpanel. 12. Select remesh. 13. Use the location: connectors selector to select the area connector you just created in step 4.10. 14. In the element size= field, enter 3.

15. Click mesh. Note:

Connector unrealizes if there is a pre-exising mesh.

16. In the Connector Entity browser, select the unrealized connector. 17. In the Entity Editor: •

Set Hexa Thickness Option to const_thickness.

•

For Const Thickness, enter 0.3.

18. In the Connector Entity browser, right-click on the unrealized connector and select Rerealize from the context menu. 19. Inspect the new adhesive created. Note:

When creating area connectors from elements, HyperMesh automatically meshes the area connector using the current mesh. If the area connector is created from nodes, lines, or surfaces and the default mesh is unsuitable from the area subpanel, then you can apply a manual mesh.

Proprietary Information of Altair Engineering

p.302

Altair HyperMesh 2019 Tutorials

p.303

HM-3420: Creating Bolt Connectors In this tutorial, you will learn how to apply a bolted connection to two rear trusses.

Model Files This exercise uses the frame_assembly_2.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise The Bolt panel creates connectors based on holes within the connected components, using spiders or washers at each end of an RBE connector. When the Bolt panel is active, only bolt-type connectors display in the graphics area; graphics for other connector types are suppressed until you exit the panel. The Bolt panel contains three subpanels: •

bolt

Create and realize bolt connectors in a single process.

•

create

Create, but not realize, bolt connectors.

•

realize

Create FE representations of previously-created bolt connectors.

Step 1: Retrieve and view the model file. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select OptiStruct.

3.

Click OK.

4.

Open a model file by clicking File > Open > Model from the menu bar, or clicking on the Standard toolbar.

5.

In the Open Model dialog, open the frame_assembly_2.hm file. A model appears in the graphics area.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

p.304

Observe the model using various visualization options available in HyperMesh (rotation, zooming, and so on).

Create a bolted connection between the two rear truss parts.

Step 2: Display only the assembly assem_5 for elements and geometry. 1.

In the Model browser, click

2.

Expand the Assembly Hierarchy folder and sub-folders.

3.

Set the entity selection to Note:

(Model View).

(Elements and Geometry).

This options turns on/off both elements and geometry when you perform rightclick operations in the Model browser.

4.

Right-click on assem_5 and select Isolate from the context menu. HyperMesh only displays the components that are in the assem_5 assembly.

5.

Right-click on the Con_Rear_Truss component and select Make Current from the context menu.

Step 3: Load the Connector Browser. 1.

Open the Connectors browser by clicking View > Browsers > HyperMesh > Connector from the menu bar.

2.

Review the layout of the Connector browser. Currently there are no components or connectors listed because there are no connectors in the model. Note:

You can use the Connector browser to view and manage the connectors in your model. The top portion of the browser is referred to as the Link Entity browser, and it displays information about the linked entities in your model. The middle portion is referred to as the Connector Entity browser, and it contains a list of the connectors in your model. The bottom portion of the browser is referred to as the Connector Entity Editor, and it displays

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

attributes assigned to the connector(s) selected in the Connector Entity browser. HyperMesh groups the connectors based on their connection type.

Step 4: Create a bolt connector. 1.

Open the Bolt panel by right-clicking in the Connector Entity browser and selecting Create > Bolt from the context menu.

2.

Set the location selector to nodes.

3.

Select a node on the edge of the hole in the Rear_Truss_1 component as indicated in the following image.

Proprietary Information of Altair Engineering

p.305

Altair HyperMesh 2019 Tutorials

4.

Set the connect what selector to comps.

5.

Click comps.

6.

Select the components, Rear_Truss_1 and Rear_Truss_2.

7.

Click select.

8.

In the tolerance= field, enter 50. Note:

9.

The connector will connect any selected entities within this distance of itself.

Click type= and select bolt (general). Note:

Re-realizing the connector will allow you to see the different bolt types.

10. Click realize & hole detect details. 11. In the max dimension = field, enter 60 to ensure that the diameter of the picked hole will be captured. 12. Click return.

13. Click create. Note:

Ensure the display of the current component is turned on.

Bolted connection

Proprietary Information of Altair Engineering

p.306

Altair HyperMesh 2019 Tutorials

14. To access the main menu, click return.

Proprietary Information of Altair Engineering

p.307

Altair HyperMesh 2019 Tutorials

p.308

HM-3430: Part Replacement Through Connectors In this tutorial, you will learn how to: •

Replace the rear truss component, Rear_Truss_1, with a new, similar part and then update the affected connectors.

•

Export the connector information

•

Export the FE deck and view the connector information in the deck

After the modeling of the assembly is complete, a design change might be made to any one of the parts. When this occurs, you must replace the current part(s) in the model with the new, similar one(s) and update the affected connections (welds).

Model Files This exercise uses the frame_assembly_3.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise A new part is needed in the assembly. In this tutorial you will learn how to delete the original component, import a new part, and update the connections. You will also export the connector information to a single file, and then export the entire FE input deck and observe how the connector information is preserved.

Step 1: Retrieve and view the model file. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select OptiStruct.

3.

Click OK.

4.

Open a model file by clicking File > Open > Model from the menu bar, or clicking on the Standard toolbar.

5.

In the Open Model dialog, open the frame_assembly_3.hm file. A model appears in the graphics area.

6.

Observe the model using various visualization options available in HyperMesh (rotation, zooming, and so on).

Step 2: Load the Connector Browser. 1.

Open the Connectors browser by clicking View > Browsers > HyperMesh > Connector from the menu bar.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

Review the layout of the Connector browser. Currently there are no components or connectors listed because there are no connectors in the model. Note:

You can use the Connector browser to view and manage the connectors in your model. The top portion of the browser is referred to as the Link Entity browser, and it displays information about the linked entities in your model. The middle portion is referred to as the Connector Entity browser, and it contains a list of the connectors in your model. The bottom portion of the browser is referred to as the Connector Entity Editor, and it displays attributes assigned to the connector(s) selected in the Connector Entity browser. HyperMesh groups the connectors based on their connection type.

Step 3: Import rear_truss_1_new.hm to set up the link update. 1.

In the Model browser, Component folder, right-click on Rear_Truss_1 and select Isolate from the context menu.

Proprietary Information of Altair Engineering

p.309

Altair HyperMesh 2019 Tutorials

p.310

2.

From the menu bar, click File > Import > Model.

3.

Under File selection, click

4.

In the Open dialog, open the file, rear_truss_1_new.hm.

5.

Click Import. HyperMesh imports rear_truss_1_new on top of rear_truss_1.

.

Step 4: Using the Connector Browser, update the connector links to the new component. 1.

In the Connector browser, Link Entity browser, right-click on Rear_Truss_1 and select Find Attached from the context menu.

2.

In the Connector Entity browser, right-click on any of the highlighted connector names and select Update Link from the context menu.

3.

In the Update window, click the Link Select field in the Search column.

4.

In the panel area, click component.

5.

Select the component, Rear_Truss_1.

6.

Click proceed. HyperMesh inserts Rear_Truss_1 into the Link Select field.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.311

7.

In the Replace column, click the Link Select field.

8.

In the panel area, click component.

9.

Select Rear_Truss_1.1.

10. Click proceed. HyperMesh inserts Rear_Truss_1.1 in the Link Select field.

11. Click Update. HyperMesh updates the connector links. 12. Close the Update window by clicking X next to Update.

Step 5: Realize the connectors in the component Con_Rear_Truss. 1.

In the Model browser, Component folder, right-click on Con_Rear_Truss and select Make Current from the context menu.

2.

Open the Spot panel by right-clicking in the Connector Entity browser and selecting Create > Spot from the context menu.

3.

Go to the realize subpanel.

4.

Click connectors >> displayed.

5.

Click type= and select weld.

6.

In the tolerance = field, enter 10.

7.

Set the mesh dependent/mesh independent toggle to mesh dependent.

8.

Under mesh dependent, set the adjust realization/adjust mesh toggle to adjust realization.

9.

Click realize. HyperMesh realizes the connectors.

10. Return to the main menu by clicking return.

Step 6: Save the connector information to an XML file. 1.

At the bottom of the Connector browser, click

2.

In the Export to file dialog, navigate to the location where you would like to save the XML file and click Save.

3.

In a text editor, open the XML file.

4.

Inspect the file and observe how the connector information has been saved. Note:

(Export connectors -XML).

In the future, you can use the XML file to import connectors.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.312

Step 7: Export the finite element deck and observe how the connector information is preserved. 1.

From the menu bar, click File > Export > Solver Deck.

2.

From the File type list, select OptiStruct.

3.

From the Template list, select standard format.

4.

In the File field, click

5.

In the Save OptiStruct file dialog, select a name and location for the file to be saved to. Note:

.

Be sure to use the .fem extension. next to Export Options.

6.

To view additional export options, click

7.

Select the Include connectors check box.

8.

Click Export.

9.

In a text editor, open the .fem file you just saved.

10. Scroll to the very bottom. This is where all of the connector information has been saved. The information has been saved as comment cards so that when you run the analysis, the connector information is not read. When you import the input deck back into HyperMesh, the connector information is read.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

HM-3440: Model Build and Assembly In this tutorial, you will learn how to: •

Import a PLMXML file.

•

Load and create a Common representation and NVH representation for modal analysis

•

Import connector parts, add connector representations, and realize connectors

•

Edit part attributes using the Entity Editor to reflect design changes

•

Activate configurations

•

Import and Export an assembly as a Solver Deck

•

Renumber entities using the ID-Manager

•

Check for errors using the Model Checker

Model Files This exercise uses the files located in the HM-3440 folder, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Start HyperMesh Desktop and Load the OptiStruct User Profile 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select OptiStruct.

3.

Click OK.

Step 2: Import the PLMXML File 1.

Open the Import - BOM tab by clicking File > Import > BOM from the menu bar.

2.

In the File field, open the BOM_input.xml file.

Proprietary Information of Altair Engineering

p.313

Altair HyperMesh 2019 Tutorials

3.

Click Import. Part assemblies and parts are imported into the session.

Step 3: Load and Create a Common Representation Steps 3.4 - 3.6 below are optional as the Common representation can be created without loading the CAD into the session. Since the Common representation forms the basis of subsequent discipline specific mesh representations, its creation is a prerequisite for the next steps. 1.

Open the Part browser by clicking View > Browsers > HyperMesh > Part from the menu bar.

Proprietary Information of Altair Engineering

p.314

Altair HyperMesh 2019 Tutorials

2.

In the Part browser, right-click and on one of the column headers and enable the following columns from the context menu: PDM PID, PDM MID, PDM Material, PDM Thickness, and PDM MeshFlag. These columns show the PDM metadata that is parsed upon importation of the PLMXML file. This information is also shown in the Entity Editor, PDM Data pane.

3.

Right-click on the Frame_Assembly_000495 part assembly and select Representations > Load > from Session from the context menu.

4.

In the Change Representations dialog, Load tab, select the CAD representation.

Proprietary Information of Altair Engineering

p.315

Altair HyperMesh 2019 Tutorials

5.

Click OK. All available CAD representations are imported into the session.

6.

Right-click on the Frame_Assembly_000495 part assembly and select Representations > Create from the context menu.

7.

In the Change Representations dialog, Create tab, select Common (0/8).

Proprietary Information of Altair Engineering

p.316

Altair HyperMesh 2019 Tutorials

8.

Click OK. Available CAD representations are sent to the BatchMesher for processing. Note:

9.

p.317

In the case of sheet metal parts, the BatchMesher extracts the midsurface from the solid CAD representation. You can choose a Midsurface method, include Skin, Offset, Offset + Planes, Offset + Planes + Sweeps.

In the BatchMesh dialog, click Yes to load the new representations for the eight parts.

10. Repeat steps 3.7 - 3.10 to create NVH10 and NVH15 representations.

Step 6: Add Connector Representations 1.

In the Part browser, right-click on the Connectors_000481 part assembly and select Representations > Load > from Session from the context menu.

2.

In the Change Representation dialog, Load tab, select the Connector representation.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

Click OK. Connectors are loaded, and the Representation column shows the Connector representation loaded.

Step 7: Design change - modify Center Rail part attributes 1.

In the Part browser note the PID of parts CenterInner_var2_A_000431_Safety and CenterOuter_var2_A_000432_Safety.

2.

In the Model browser, switch the view mode to Properties.

Proprietary Information of Altair Engineering

p.318

Altair HyperMesh 2019 Tutorials

p.319

3.

Select PID 103 and 104. The EntityEditor opens and displays the two properties common corresponding attributes.

4.

In the Entity Editor, T field, enter 3.0.

5.

In the Part browser, notice the attribute modification you made is updated in the Thickness columns. Save these changes to ensure that they are available if the current representation is unloaded.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 8: Create Part Sets Create part sets Var1 and Var2 for Variant 1 and Variant 2 in the Part Set view. 1.

In the Part browser, enable the Part Set view.

2.

Create two part sets.

3.

a.

In the Part Set view, right-click and select Create > Part Set from the context menu.

b.

Name the part sets Var1 and Var2.

Group common and unique parts by dragging-and-dropping parts from the Part view onto the part set. Var 1: •

Center_Rail_Connectors_var1_000484

•

CenterInner_A_000428_Safety

•

CenterOuter_A_000429_Safety

Var2: •

Center_Rail_Connectors_var2_000485

•

CenterInner_var2_A_000431_Safety

•

CenterOuter_var2_A_000432_Safety

Step 9: Create Configurations Create configurations Var1 and Var2 for part sets Var1 and Var2 in the Configuration view. 1.

In the Part browser, enable the Configuration view.

2.

Create two configurations.

Proprietary Information of Altair Engineering

p.320

Altair HyperMesh 2019 Tutorials

3.

In the Part Set view, right-click and select Create > Configuration from the context menu.

4.

Name the configurations Var1 and Var2.

5.

Group part sets that are unique by dragging-and-dropping part sets from the Part Set view onto the configuration. a.

Group the Var1 part set into the Var 1 configuration.

b.

Group the Var2 part set into the Var 2 configuration.

Step 10: Activate the Var 2 Configuration 1.

In the Part browser's Configuration view, Active column, enable the checkbox for Var 2. All of the parts, part assemblies, components, and part sets not associated with Var 2 become inactive.

Proprietary Information of Altair Engineering

p.321

Altair HyperMesh 2019 Tutorials

Step 11: Export Assembly as a Solver Deck 1.

Open the Export – Solver Deck tab by clicking File > Export > Solver Deck from the menu bar.

2.

In the File field, enter frame_var2_model.fem.

3.

Under Export Options: •

Set Export to Custom to ensure that inactive parts are not written to the solver deck.

•

Under Comments, select the Part Assemblies/Parts checkbox.

4.

Click Export.

5.

Save the model as frame_assembly.hm.

Step 12: Import Assembly Solver Deck 1.

Start a new HyperMesh Desktop session.

2.

Open the Import – Solver Deck tab by clicking File > Import > Solver Deck from the menu bar.

3.

In the File field, locate the frame_var2_model.fem solver deck.

4.

Click Import.

5.

In the Part browser, verify that the BOM was imported correctly. Note:

All part assembly and part metadata in the original model should be present, with the exception of the Representation name.

Step 13: Import Realizations 1.

Open the Import - Model tab.

2.

Click

3.

The Spotweld component, in the Realizations.hm file, references a material that has the same ID as a material that already exists in the current session, therefore under Entity Management, set Materials to Keep Existing Attributes.

, then open the Realizations.hm file.

Proprietary Information of Altair Engineering

p.322

Altair HyperMesh 2019 Tutorials

4.

p.323

Click Import. Connector parts are imported.

Step 14: Realize Connectors 1.

In the Part browser, right-click on the Spotwelds component and select Make Current from the context menu.

2.

In the Part browser, right-click on the Longitudinal_Rail_Connectors and select Hide from the context menu. The display of the component’s connectors is turned off in the graphics area enabling you to get a better visual of each component's connectors.

3.

Open the Connector browser by clicking View > Browsers > HyperMesh > Connectors from the menu bar.

4.

In the Connector Entity browser, select the acm (shell gap) connector folder.

5.

In the Entity Editor, set Property Script to no/skip post script. Note:

Connector links are defined via Parts to ensure that connectors realize even if you, accidentally, renumber all of the entities in the model.

6.

In the Connector Entity browser, select all of the connectors.

7.

Right-click on the selected connectors and select Rerealize from the context menu.

8.

In the Part browser, right-click on the Spotwelds part and select Isolate Only from the context menu. Verify that the realized FE resides in the Spotwelds component.

Step 15: Renumber Nodes and Elements 1.

Open the ID-Manager by clicking Tools > ID-Manager from the context menu.

2.

In the ID-Manager, select Components, Properties, and Materials then right-click and select Exclude from the context menu.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.324

3.

For the Master Model, enter 1,000,000 in the Min field and 1,500,000 in the Max field.

4.

Correct ID overflow by right-clicking on the Master Model and selecting Correct > Overflow from the context menu.

Step 16: Run the Model Checker 1.

Open the Model Checker by clicking Tools > Model Checker > OptiStruct.

2.

In the Model Checker, right-click and select Run from the context menu.

3.

Verify that the model is error free.

Step 17: Export the Solver Deck 1.

From the menu bar, click File > Export > Solver Deck.

2.

In the Export – Solver Deck tab, File field, enter the file name frame_var2_assembled.fem.

3.

Under Export options, Comments, select the Part Assemblies/Parts checkbox.

4.

Click Export.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.325

HM-3450: Multi-Component Replacement In this tutorial, you will learn how to simultaneously replace multiple components in your current model using the Part Replacement tool. You will be replacing six related components (bumper, front frame, and radiator frame) in the Pr_Inc.k Include file with components that contain a finer mesh.

Model Files This exercise uses the files located in the hm-3450 folder, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Start HyperMesh Desktop and Load the LS-DYNA User Profile 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select LS-DYNA.

3.

Click OK.

Step 2: Import the Solver Deck File 1.

Open the Import - Solver Deck tab by clicking File > Import > Solver Deck from the menu bar.

2.

In the File field, open the Master.k file.

3.

Click Import.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.326

Step 3: Replace Parts in the Pr_Inc.k Include File 1.

In the Model browser, right-click on the Pr_Inc.k Include file and select Replace > Manual from the context menu.

The Part-Replace dialog opens.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

Set the Replace using field to Comp in File, then open the Incoming_idclash.k file, which contains the target, replacement parts.

3.

In the Tolerance field, field, enter a tolerance to search for closest nodes and elements to re-establish the connections and other references between the target part and the model. For this tutorial, you can leave the default tolerance of 0.01.

5.

Click Preview.

6.

In the Component Pairing dialog, check the component pairing. a.

In the second row, note that there is one –two mapping. If it does not come up display, click on the second row to add the new pairing.

b.

Click OK.

Note:

7.

p.327

When performing Manual part replacement, you have the flexibility to modify the component pairing using add/remove pairing option in component pairing window; whereas, when performing Automatic part replacement, you cannot modify component pairing.

In the Entities Selection dialog, specify replacement methods for incoming/existing entities and click OK. External entities are shared with other components, along with the selected components that are being replaced (example: sets, groups, output blocks, and so on). Internal entities are specific to the components being replaced (example: sets, groups, output blocks, and so on). •

Accept incoming entities (existing entities deleted) deletes all of the internal entities on accept.

•

Accept existing entities (Incoming entities deleted) deletes all of the incoming entities on accept.

•

Merge existing and incoming entities (no entities deleted) retains both existing and incoming entities on accept.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Note:

8.

When performing Automatic part replacement, HyperMesh automatically selects the Accept incoming entities (existing entities deleted) method.

Check the status of each entities. Note:

All internal entities are deleted, and all external entities are updated.

Step 4: Review ID Ranges 1.

Click ID Manager to invoke the ID-Manager, from which you can review existing ID ranges defined for the components.

2.

Modify ID ranges as needed.

3.

Click Close.

Step 5: Run Model Checker Post Part Replacement 1.

Under Advanced options, enable the Invoke Model Checker after Accept checkbox to automatically run the Model Checker after you click Accept in the Part-Replace dialog.

Proprietary Information of Altair Engineering

p.328

Altair HyperMesh 2019 Tutorials

Step 6: Accept Part Replacement Changes 1.

Click Accept. The source part is deleted and the connection of the new part to the model is accepted.

Proprietary Information of Altair Engineering

p.329

Altair HyperMesh 2019 Tutorials

Morph

Proprietary Information of Altair Engineering

p.330

6

Altair HyperMesh 2019 Tutorials

p.331

HM-3510: Freehand Morphing Model Files This exercise uses the propeller.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Translating Nodes to Increase the Length of a Propeller Blade In this tutorial, you will increase the length of a propeller blade by 100 units, using freehand morphing.

Figure 1: Original blade

Figure 2: Blade after morphing

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 1: Load the model. 1.

Start HyperMesh Desktop.

2.

Open a model file by clicking File > Open > Model from the menu bar, or clicking on the Standard toolbar.

3.

In the Open Model dialog, open the propeller.hm file. A model appears in the graphics area.

Step 2: Morph the blade. Method 1: Fixed value based 1.

Open the move nodes subpanel by clicking Morphing > Free Hand from the menu bar.

2.

Set the morphing method to translate.

3.

In the z= field, enter -100.

4.

In the Model browser, View folder, right-click on View1 and select Show from the context menu.

5.

Use the moving nodes and fixed nodes selectors to select the nodes indicated in the following image.

Figure 3: Node and element selections.

6.

Use the affected elements selector to select the elements between the fixed nodes and moving nodes.

7.

In the mv bias and fx bias fields, keep the default values (1.00).

Proprietary Information of Altair Engineering

p.332

Altair HyperMesh 2019 Tutorials

8.

Click morph. HyperMesh alters the blade of the propeller. Note:

9.

The length of the propeller blade increased by 100. The fixed nodes did not move. HyperMesh stretched the affected elements evenly to maintain element quality. The stretching of the elements took place between the moving nodes and the fixed nodes.

Restore the propeller back to its original shape by clicking undo.

Method 2: Interactive graphic manipulator base 10. In the move nodes subpanel, set the morphing method to manipulator.

11. Leave the other parameters and options set to their default values. 12. In the Model browser, View folder, right-click on View1 and select Show from the context menu. 13. Use the moving nodes and fixed nodes selectors to select the nodes indicated in the following image.

Figure 3: Node and element selections.

14. Use the affected elements selector to select the elements between the fixed nodes and moving nodes. A manipulator appears.

Proprietary Information of Altair Engineering

p.333

Altair HyperMesh 2019 Tutorials

15. Optional: Move the manipulator to a different location by activating the origin: nodes selector and selecting another node as the origin.

16. Zoom in and rotate close the manipulator area.

17. Translate the nodes by clicking and dragging one of the three yellow arrows of the manipulator.

18. Rotate the nodes about the center of the manipulator by clicking and dragging one of the three yellow arcs of the manipulator.

Proprietary Information of Altair Engineering

p.334

Altair HyperMesh 2019 Tutorials

19. Click undo. 20. Move the nodes in a plane by clicking and dragging one of the three yellow right angles of the manipulator.

21. Create more than one manipulator at a time by setting the single manipulator/multiple toggle to multiple.

22. Create a new manipulator by clicking new manip and selecting one or more moving nodes. Note:

The different manipulators may have different selected entities and different parameters, and can be moved independently of one another.

23. Move a manipulator by clicking a manipulator or simply moving your mouse over a manipulator. HyperMesh updates the panel to the parameters associated to that manipulator. You can change the parameters or the entities associated with them if you desire. 24. Make manipulators active or inactive by switching the manip:active/manip:inactive toggle. When active, the manipulators morph the model when you move them. When inactive, the manipulators will only change their own position and orientation when you move them.

Proprietary Information of Altair Engineering

p.335

Altair HyperMesh 2019 Tutorials

Summary Method 1: The length of the propeller blade increased by 100. The fixed nodes did not move. The affected elements were stretched evenly to maintain element quality. The stretching of the elements took place between the moving nodes and the fixed nodes. Method 2: The length of the propeller blade increased depending on how you dragged the handles along the three arrows, arcs, or right angles of the manipulator to respectively translate, rotate, or move the nodes. The fixed nodes did not move. The affected elements were stretched evenly to maintain element quality. The stretching of the elements took place between the moving nodes and the fixed nodes.

Proprietary Information of Altair Engineering

p.336

Altair HyperMesh 2019 Tutorials

HM-3520: Sculpting Model Files This exercise uses the dummy_position_solid.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Conforming a Seat to a Dummy Profile The objective of this exercise is to take a dummy pelvis profile and imprint it onto a seat.

Figure 1: Seat before and after sculpting

Step 1: Load and review the model. Open the HyperMesh file, dummy_position_solid.hm.

Step 2: Morph the seat. 1.

From the menu bar, click Morphing > Free Hand.

2.

Go to the sculpting subpanel.

3.

Set the sculpting tool to mesh.

4.

For the sculpting tool, select all of the elements in the dummy collector (Figure 2).

5.

For affected elements, select all of the elements in the seat collector (Figure 2).

6.

For the base point as well as the tool path: node list, choose a node on the dummy (Figure 2).

7.

Define a sculpt direction for your seat using N1 N2 (Figure 2).

8.

Set your taper angle to 85 (degrees).

9.

Verify that mesh compression is set to compress by factor.

10. Set mesh compr= to 0.5.

Proprietary Information of Altair Engineering

p.337

Altair HyperMesh 2019 Tutorials

Figure 2: Setting up the model for morphing

10. Click move+ to complete the morphing operation.

Figure 3: Seat after sculpting

11. Review the obtained mesh quality.

Summary Using just a few steps you have been able to take a fairly complicated profile and impose it on to another mesh.

Proprietary Information of Altair Engineering

p.338

Altair HyperMesh 2019 Tutorials

HM-3530: Changing a Curvature Using Map to Geometry Model Files This exercise uses the bumper_morphing.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Changing the Curvature of a Bumper to a Curved Line In this exercise, you will use the line difference approach to morph a bumper to conform to a new section line.

Figure 1: Bumper before and after morphing

Step 1: Load and review the model. Open the HyperMesh file, bumper_morphing.hm.

Step 2: Morph the bumper. 1.

Open the map to geom panel by clicking Morphing > Map to Geometry from the menu bar.

2.

Change the geometry selector to line difference.

3.

Select the from line (Line A) and the to line (Line B) as shown in figure 2.

4.

Toggle the morphing entity (2nd column) from map domains to map nodes.

5.

Select nodes >> displayed.

6.

Use no fixed nodes (2nd column, 2nd row).

Proprietary Information of Altair Engineering

p.339

Altair HyperMesh 2019 Tutorials

7.

Use map by line axis morphing with a 1.0 mvbias and fxbias (column 3).

Figure 2: The from line and the to line

8.

Click map.

Summary The profile of the bumper is changed to follow the new section line.

Proprietary Information of Altair Engineering

p.340

Altair HyperMesh 2019 Tutorials

HM-3540: Changing a Profile Using Map to Sections Model Files This exercise uses the car_section.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Changing the Profile of the Roof of a Car In this tutorial, you will use map to sections to change the profile of the car roof.

Figure 1: Car model.

Step 1: Load and review the model. Open the HyperMesh file, car_section.hm.

Step 2: Morph the roof. 1.

Click Morphing > Map to Geometry to access the Map to geom panel.

2.

Change the mapping section type to map to sections.

3.

Under map to sections, toggle lines to line list.

4.

Switch map domains to map elements (2nd column).

5.

Toggle no fixed nodes to fixed nodes (2nd column).

6.

Keep blend all option selected.

7.

Keep rotate nodes active.

Proprietary Information of Altair Engineering

p.341

Altair HyperMesh 2019 Tutorials

p.342

8.

Keep the 3rd column selector set to map by line normal.

9.

Click first line list button and select Line A and Line B on the model.

10. Under to: click the second line list button and select Line A’ and Line B’ on the model. Lines should be selected in the same order. 11. Under map to elements click the elems button and select elements by collector. 12. Pick collector Roof. (This may be located on the second page of collectors) 13. Click select. 14. Click the XZ Right Plane View (

) icon to set the view

15. For fixed nodes use Shift + Left Mouse Button to select all the nodes as shown in figure 2.

Figure 2: Selection for fixed nodes

16. Click map.

Summary The roof of the car has been morphed while the mesh quality has been maintained.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.343

HM-3550: Morph Volume Model Files This exercise uses the body_side.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Changing the Shape of the B-pillar with the Help of Morph Volume This exercise shows how to smoothly change the shape of a B-pillar via morph volumes.

B-Pillar before and after morphing

Step 1: Load and review the model. 1.

Start HyperMesh Desktop.

2.

To open a model file, click File > Open > Model from the menu bar, or click the Standard toolbar.

3.

In the Open Model dialog, open the body_side.hm file. A model appears in the graphics area.

on

Step 2: Create morph volumes. 1.

To open the Morph Volumes panel, click Morphing > Create > Morph Volumes from the menu bar.

2.

Set the creation method to pick on screen.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.344

3.

Set handle placement to corners only.

4.

Select the auto-tangent check box.

5.

On the Standard Views toolbar, click

6.

Click the four red circles indicated in the image below to draw a window. HyperMesh creates a morph volume, which encloses the area.

.

Points for creating the morph volume

Step 3: Split the morph volumes. 1.

Go to the split/combine subpanel.

2.

Set the by nodes/by edge toggle to by edges

3.

Select an edge of the morph volume close to location 1 as indicated in the following image. A green colored cross moves to the location of the black dot.

Locations to split the morph volume

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

Click split. HyperMesh splits the morph volume into two.

5.

Repeat steps 3.3 and 3.4, except select an edge of the morph volume close to location 2 as indicated in the previous image.

Step 4: Change the profile of the b-pillar. Method 1: Fixed value based 1.

To open the Morph panel, click Morphing > Morph from the menu bar.

2.

Go to the move handles subpanel.

3.

Set the morphing method to translate.

4.

Set the orientation selector to along xyz.

5.

In the y val= field, enter 100.

6.

Leave the x val= and z val= fields set to 0.

7.

Press and hold SHIFT, then drag your mouse around the the eight handles indicated in the image below.

Select handles for morphing

8.

Click morph.

Proprietary Information of Altair Engineering

p.345

Altair HyperMesh 2019 Tutorials

9.

p.346

To verify that the b-pillar is morphed, rotate the model.

10. To restore the model's original shape, click undo. Method 2: Interactive graphic manipulator base 11. In the move nodes subpanel, set the morphing method to interactive and manipulators.

12. Leave the other parameters and options set to their default values. 13. On the Standard Views toolbar, click

.

14. Press and hold SHIFT, then drag your mouse around the the eight handles indicated in the image below. A manipulator appears.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.347

15. Optional: You can select another node as the origin to set the manipulator in a different position.

16. Zoom in and rotate close to the manipulator area.

17. To translate the nodes, click and drag, graphically, one of the three yellow arrows of the manipulator.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

18. Click undo. 19. To rotate the nodes about the center of the manipulator, click and drag, graphically, one of the three yellow arcs of the manipulator.

20. Click undo. 21. To move the nodes in a plane, click and drag, graphically, one of the three yellow right angles of the manipulator.

Proprietary Information of Altair Engineering

p.348

Altair HyperMesh 2019 Tutorials

22. Click undo. 23. To create more than one manipulator at a time, set the single manipulator/multiple toggle to multiple.

24. To create a new manipulator, click new manip and then graphically select one or more moving nodes. Note:

The different manipulators may have different selected entities and different parameters, and can be moved independently of one another.

25. To move a manipulator, click a manipulator or simply move your mouse over a manipulator. HyperMesh updates the panel to the parameters associated to that manipulator. You can change the parameters or the entities associated with them if you desire. 26. To make manipulators active or inactive, switch the manip:active/manip:inactive toggle. When active, the manipulators morph the model when you move them. When inactive, the manipulators will only change their own position and orientation when you move them.

Summary In both methods, you morphed the b-pillar in a smooth fashion with minimum distortion to the elements.

Proprietary Information of Altair Engineering

p.349

Altair HyperMesh 2019 Tutorials

p.350

HM-3560: Basics of Domains and Handles Model Files This exercise uses the morphing_1.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Using Domains and Handles In this exercise you will create domains and handles, and morph the model.

Step 1: Load and review the model. Open and review the HyperMesh model morphing_1.hm.

Step 2: Auto generate 2-D domains and handles. 1.

Click the Morphing menu in the menu bar and select Create > Domains.

2.

Change the create method to auto functions.

3.

Click generate. Based on the model’s geometric features, all of the model’s elements are organized into various domains and local handles are created and associated with the domains.

Step 3: Move elements into a new 2-D domain. 1.

Set the selector to 2D domains. Toggle to the elems selector if not already there.

2.

Click

3.

Using elems >> by window, select the elements indicated in figure 1.

to clear the elements that were already selected.

Figure 1: Elements to select to move into a new domain

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

Verify that partition 2D domains is active.

5.

Click create to create the domain. Local handles are created for the new domain. You should now have two local domains. Elements can only belong to one domain at a time. Thus, the elements you selected were moved into the new domain. This functionality makes it very easy to group elements into different domains.

Step 4: Split the edge domain of the radius to have more control when morphing. 1.

Click the edit edges subpanel in the Morphing > Domains panel.

2.

Verify that the split option is selected.

3.

With the domain selector active, select the edge domain of the part’s radius as indicated in the Figure 2. The node selector automatically becomes active once the edge domain is selected. Click the domain selector to make it active and see that you selected the desired edge domain.

Figure 2: Edge domain to select

4.

Click the node selector to make it active.

Proprietary Information of Altair Engineering

p.351

Altair HyperMesh 2019 Tutorials

5.

p.352

Select the node on the positive Y-axis end of the radius, as indicated in the image Figure 3.

Figure 3: Node selection to split the edge domain of the radius

6.

Click split to split the edge domain at the node.

7.

Repeat the above process to further split the edge domain of the radius, this time at the node indicated in the Figure 4.

Figure 4: Node selection to further split the edge domain of the radius

8.

When complete, click return to exit the panel.

Step 5: Add local handles to the 2-D domain on the part’s left side. 1.

Click the Morphing menu, and pick Create > Handles.

2.

For name=, enter local.

3.

Click the attached to: domain selector to make it active.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

Select the 2-D domain on the part’s left side by selecting its red icon, as indicated in the following image.

Figure 5: Adding handles to a 2-D domain

5.

Click the by nodes: nodes selector to make it active.

6.

Select the two nodes as indicated in the previous image.

7.

Click create to create the handles and add them to the 2-D domain.

8.

Click return to exit the panel.

Step 6: Perform basic morphing to understand how domains and handles interact with each other and the mesh. 1.

Click the Morphing menu, and select Morph.

2.

Select the move handles subpanel if not already there.

3.

Change the mode to interactive if not already set.

4.

With the handles selector active, select the two handles on the right-hand end of the part, as indicated in figure 6. If you select one or more handle, those handles follow the handle you drag (in Step 6.10, following).

5.

Switch from manipulator to on plane.

6.

Click the N1 selector to make it active.

7.

For N1, N2, and N3, select any three nodes on the model to define a plane.

8.

Click morph. The message, “pick handles and move to new location” appears in the status bar.

Proprietary Information of Altair Engineering

p.353

Altair HyperMesh 2019 Tutorials

9.

p.354

Click on and drag one of the selected handles to morph the part. As you drag the handle, the mesh’s size and shape is adjusted. Notice that the following occurs as the selected local handle is moved: •

The handles selected in step 6.2 above follow the handle you are dragging.

•

All of the elements belonging to the selected local handle’s 2-D domain are affected by moving that local handle.

•

The 2-D domain’s non-selected local handles act like anchors (they do not move).

•

The nodes on the edge domains and between any two non-selected local domains do not move.

•

None of the elements in the other 2-D domain are affected.

10. Release the mouse button to complete the morphing operation.

Figure 6: Example result of morphing the model

11. Click undo. The HyperMorph module allows for multiple levels of undo and redo for all morphing operations. This functionality is available for any particular HyperMesh session and its current model as long as the session and its model remain open. 12. Click

to clear the selected handles.

13. With the handles selector active, select one or more global handles. 14. Click morph. 15. Click on and drag any global handle to morph the part.

Summary The following occurs as the selected global handle is moved: •

The handles selected in Step 6.2 above follow the handle you are dragging.

•

The non-selected global handles act like anchors (they do not move).

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

•

All of the elements, local handles and edge domains are affected.

Proprietary Information of Altair Engineering

p.355

Altair HyperMesh 2019 Tutorials

p.356

HM-3570: Altering Cross-Sections Using Domains Model Files This exercise uses the spring.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Increasing the Gauge Thickness of the Spring Wire In this tutorial, you will use domains and handles to increase the gauge thickness.

Figure 1: Before and after morphing

Step 1: Load and review the model. Open the HyperMesh file, spring.hm.

Step 2: Change the gauge thickness. 1.

Click the Morphing menu and pick Create > Domains.

2.

Switch domain type to 2D domains.

3.

Verify elements toggle is set to all elements.

4.

Verify that only the partition 2D domains option is active.

5.

Click create.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

Click the Morphing menu and pick Morph. Enter the alter dimensions subpanel if not already there.

7.

Change the morphing method to radius.

8.

Change the center calculation to by normals.

9.

Keep all the other settings.

10. For domains (under edge and 2D) select the 2D domain and the two edge domains as shown in Figure 2.

Figure 2: Domains to select for altering the gauge radius

When the circular edge domain is selected, the radius box populates with the current radius value. 11. In the radius field, type 12. 12. Click morph.

Summary The gauge thickness of the spring wire is changed from 7.5 to 12.0.

Proprietary Information of Altair Engineering

p.357

Altair HyperMesh 2019 Tutorials

p.358

HM-3580: Morphing About an Axis Using Domains Model Files This exercise uses the spring.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Changing the Radius of the Spring Coil In this exercise, you will increase the radius of the spring coil.

Figure 1: Before and after morphing

Step 1: Load and review the model. Open the HyperMesh file, spring.hm.

Step 2: Change the coil radius. 1.

Click the Morphing menu and pick Create > Domains.

2.

Switch domain type to 2D domains.

3.

Verify that the elements toggle is set to all elements.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

Verify that only the partition 2D domains option is active.

5.

Click create.

6.

Click the Morphing menu and pick Morph. Enter the alter dimensions subpanel if not already there.

7.

Change the morphing method to radius.

8.

Change the center calculation to by axis.

9.

Change the axis to the z-axis.

Figure 2: Domains and base node to select for altering the coil radius

10. For domains (under edge and 2D) select the 2-D domain and the two edge domains. 11. For the base node for the z-axis select the node as shown in Figure 2. 12. Keep the default settings for the remaining options. 13. Activate add to current. 14. In the radius field, type 20. 15. Click morph.

Summary Twenty units are added to the coil radius.

Proprietary Information of Altair Engineering

p.359

Altair HyperMesh 2019 Tutorials

HM-3590: Morph Adhesive Layers Objective Use morphing to change the thickness of the middle layers of a four-layered solid, while maintaining the thickness of the outer layers.

Model Files This exercise uses the Morph_Adhesive_Layers.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Tools Domains will be created using 3D domains > by component. Thickness will be altered using alter dimensions.

Proprietary Information of Altair Engineering

p.360

Altair HyperMesh 2019 Tutorials

Step 1: Open the file. 1.

Open the file, Morph_Adhesive_Layers.hm.

Step 2: Create domains and handles. 1.

Click the Morphing menu and pick Create > Domains.

2.

Switch the domain type to 3D domains.

3.

Toggle the element selector to all elements.

4.

Activate the divide by comps and partition 2D domains options. The panel should appear as in the following image:

5.

Click create to create the domains.

6.

Click return to exit the Domains panel.

Step 3: Display only the morph faces of interest. 1.

Using the Model Browser, hide all the components except ^morphface.

2.

Mask all ^morphface elements except those on the outer layer and the layer between the Outer comp and the Adhesive_Outer to leave all the elements shown in the following image. HINT:

Select a couple of elements on the face you want to keep. Select elements >> by face, and then select elements >> reverse. This will reverse the selection to the elements you do not want and will allow you to mask those elements with the mask button.

Proprietary Information of Altair Engineering

p.361

Altair HyperMesh 2019 Tutorials

3.

To reduce the number of domains and handles shown on the screen, click the Mask tab.

4.

Click the + next to Morphing to expand it.

5.

Click the + in the Show column for Local Domains/Handles to display the domains and handles for only the displayed elements.

6.

Hide the ^morphface component in the Model Browser.

p.362

Step 4: Increase the thickness of the outer adhesive layer by 5 units. 1.

Click the Morphing menu and pick Morph to open the Morph panel.

2.

Open the alter dimensions subpanel.

3.

Change the dimension type to radius.

4.

Activate the add to current checkbox.

5.

For domains, select the curved edge domains as well as the 2-D domains representing the curved surfaces as seen in the following image.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

Set the center calculation to by axis.

7.

For the axis, use the z-axis.

8.

For B select the temp node that represents the center of the cylinder.

9.

In radius= box, change value to 5 units.

10. Click morph. 11. Go to the save shape subpanel. 12. For name= enter sh1. 13. Switch to as node perturbations. 14. Click save. 15. Click undo all to revert back to the original model configuration. 16. Show all components except the ^morphface component. 17. Go to the apply shapes subpanel. 18. For shapes select sh1. 19. Click select. 20. Click animate. This takes you to the Deformed Shape panel. 21. Change the animation scale from model units to scale factor. 22. Set the scale factor to 1. 23. Click linear to start the animation. 24. Once you are done viewing your animation and verifying that it is as intended, you can return to the main panel area. With this step you have successfully completed morphing one of the middle layers of the four-layer model. Optional: Using the process shown above, increase the thickness of Adhesive_Inner component by 5 units.

Proprietary Information of Altair Engineering

p.363

Altair HyperMesh 2019 Tutorials

HM-3600: Morph Tube to Different Configurations Objective Use morphing to create multiple configurations of a model.

Model Files This exercise uses the tube.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Tools Domains, morph

Figure 1: Tube to morph

Step 1: Open the file. 1.

Open the file, tube.hm.

Step 2: Create domains and handles. 1.

From the menu bar, click Morphing > Create > Domains.

2.

Go to the create subpanel.

3.

Switch the domain type to 3D domains.

4.

Toggle the element selector to all elements.

5.

Activate the partition 2D domains option.

Proprietary Information of Altair Engineering

p.364

Altair HyperMesh 2019 Tutorials

6.

p.365

Click create.

Step 3: Partition the outer domain. 1.

Make sure you are still in the Domains > create subpanel.

2.

In the Model Browser, hide the component solid.

3.

Using the Mask panel ( ^morphfaces. HINT:

), display only the outer elements of the component

Select a couple of elements on the face you want to keep. Select elements >> by face, and then select elements >> reverse. This will reverse the selection to the elements you do not want and will allow you to mask those elements with the mask button.

4.

Click return to return to the Domains panel.

5.

To reduce the number of domains and handles shown on the screen, click the Mask tab.

6.

Click the + next to Morphing to expand it.

7.

Click the + in the Show column for the Local Domains/Handles to display the domains and handles for only the displayed elements.

8.

Change your view to a left view.

9.

Change the domain type to 2D domains.

10. Change the elements selector from all elements to elems. 11. Select the elements as displayed in the following picture.

Figure 2: Elements to partition

12. Click create to create the new domain.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

13. Click return to exit the panel.

Step 4: Increase the outer diameter of the middle section of the tube. 1.

Click Morphing > Morph to open the Morph panel.

2.

Go to the alter dimensions subpanel.

3.

Set the dimension type to radius.

4.

Set the center calculation to by edges.

5.

Switch the mesh to wireframe.

6.

Select the two edge domains and the 2D domain as shown in the following figure.

Figure 3: Select the following Edge and 2D domains.

7.

Set the radius= value to 27.

8.

Click morph to morph the part.

9.

Remain in this panel for the next section.

Figure 4: New profile of the part

Proprietary Information of Altair Engineering

p.366

Altair HyperMesh 2019 Tutorials

Step 5: Offset the inner diameter of the tube. 1.

Click unmask all

2.

Use the Mask panel to display only the tube inner elements of the component ^morphfaces. HINT:

to display all the elements.

Select a couple of elements on the face you want to keep. Select elements by face followed by elements reverse. This will reverse the selection to the elements you do not want and will allow you to mask out those elements.

3.

Click return to return to the Domains panel.

4.

To reduce the number of domains and handles shown on the screen, click the Mask tab.

5.

Click the + next to Morphing to expand it.

6.

Click the + in the Show column for the Local Domains/Handles to display the domains and handles for only the displayed elements.

7.

Click Morphing > Morph to open the Morph panel.

8.

Go to the alter dimensions subpanel, set the dimension type to radius.

9.

Select domains >> displayed. This selects the two inner edge domains as well as the 2D domain for the tube inner.

Figure 6: edge domains on the inner radius

10. Change the center calculation: to by axis. 11. For the axis, switch to the y-axis. 12. For base point, select the temp node at the center of the tube arc. 13. For radius= enter 3. 14. Check add to current. 15. Click morph to morph the inner diameter of the tube.

Figure 7: Tube with offset inner

Proprietary Information of Altair Engineering

p.367

Altair HyperMesh 2019 Tutorials

Summary Using morphing operations, dimension changes have been successfully performed on a tubular mesh.

Proprietary Information of Altair Engineering

p.368

Altair HyperMesh 2019 Tutorials

p.369

HM-3610: Shaping a Dome Using Cyclic Symmetry Model Files This exercise uses the bottle.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Using Cyclical Symmetry to Assist in the Morphing of a Bottle In this exercise you will create a dome shape at the bottom of the bottle using morph volumes.

Figure 1: Before and after morphing

Step 1: Load and review the model. Open the HyperMesh file bottle.hm

Step 2: Create morph volumes. 1.

From the menu bar, select Morphing > Create > Morph Volumes.

2.

Switch create morphvol to create matrix.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

Set: •

x density = 3

•

y density = 8

•

z density = 5

•

buffer % = 5

4.

Select elems >> displayed.

5.

Toggle global system to local system.

6.

For syst, select the system located at the top of the bottle.

7.

Use the default values for the remaining settings.

8.

Click create to create the morph volumes. Note:

9.

p.370

Morph volumes are created, encompassing the bottle, with red colored handles created at the corners of each morph volume.

Click return to exit the panel.

Step 3: Create symmetry. 1.

From the menu bar, select Morphing > Create >Symmetries.

2.

Under domains, activate morph volumes & mapping check box. Symmetries can either be linked to domains or to morph volumes. Here you are associating the symmetries to the morph volumes.

3.

Change 1 plane to cyclical.

4.

Change 180 degrees to set freq.

5.

Set # of cycles to 8.

6.

For syst select the cylindrical coordinate system located at the top of the bottle.

7.

Click create. Note that a cyclical symmetry is created.

8.

Click return to exit the panel.

Step 4: Create the dome. 1.

From the menu bar select Morphing > Create > Morph Volumes, and then select the update edges subpanel.

2.

Toggle update nodes to update ends.

3.

Change the view to the bottom view by selecting the XY Bottom Plane View .

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.371

4.

Verify that the options by edges and free are selected (see image below).

5.

Using the image below as reference, select the line to the left of the tangency at the top of the center circle.

Figure 2: Updating tangencies, selecting line

6.

After selecting the line, select the tangency (shown below).

Figure 3: Updating tangencies, select tangency

Notice that after selecting the tangency, the two arrows are replaced with a single arrow.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

7.

Repeat steps 5 and 6 on the three other tangencies shown in the image below:

Figure 4: Updating tangencies, additional tangencies to update

8.

When finished, click return to exit the panel.

9.

From the menu bar select Morphing > Morph and then select the move handles subpanel:

10. Select the handles at the bottom of the bottle, as shown in Figure 5.

Figure 3: Handles to translate

11. Switch the morphing method from interactive to translate. 12. Switch to along xyz 13. Set z val = 10 14. Click morph. Since you have symmetries defined, translating a single handle on the inner ring at the bottom, ensures that a similar behavior is imparted on all the handles symmetrically associated to it.

Proprietary Information of Altair Engineering

p.372

Altair HyperMesh 2019 Tutorials

p.373

15. To reduce the number of domains and handles shown on the screen, click the Mask tab. If this isn’t displayed, select View > Browsers > HyperMesh > Mask. 16. Click the - in the Hide column to turn off the display of all morphing entities. 17. Rotate the model to view the changes made.

Figure 6: Morphed model

Summary Using morph volumes with appropriate tangencies, and by creating symmetries you are able to create a dome-shaped feature at the bottom of the bottle.

Remarks There are four different methods to define the continuity between the morph volumes. •

Free makes morph volume edges independent of other edges.

•

Fixed connectivity allows you to prescribe the angle at the end of an edge.

•

Master-slave maintains tangency between two morph volume edges while keeping the master edge independent of the slave edge. (When the master edge moves, the

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

slave edge follows, but when the slave edge moves, the master edge does not have to follow.) •

Continuous maintains tangency between two morph volume edges while allowing both edges to affect each other.

The default setting in morph volume is always set to tangent which is continuous edge connectivity. This definition can always be changed in the update edges subpanel, based upon the morphing needs.

Proprietary Information of Altair Engineering

p.374

Altair HyperMesh 2019 Tutorials

p.375

HM-3620: Shaping a Bead Using Cyclic Symmetry Model Files This exercise uses the bottle.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Creating a Circular Bead on the Bottle In this exercise you will first create a bead using the default continuous edge connectivity. You will then update the edges to free and see how it affects the bead creation.

Figure 1: Adding beads to the bottle

Step 1: Load and review the model. Open the HyperMesh file bottle.hm

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.376

Step 2: Create morph volumes. 1.

From the menu bar, select Morphing > Create > Morph Volumes.

2.

Switch create morphvol to create matrix.

3.

Set: •

x density = 3

•

y density = 8

•

z density = 5

•

buffer % = 5

4.

Select elems >> displayed.

5.

Toggle global system to local system.

6.

For syst, select the system located at the top of the bottle.

7.

Use the default values for the remaining settings.

8.

Click create to create the morph volumes. Note:

9.

Morph volumes are created encompassing the bottle, with red colored handles created at the corners of each morph volume.

Click return to exit the panel.

Step 3: Create symmetry. 1.

From the menu bar select Morphing > Create >Symmetries.

2.

Under domain, activate morph volumes & mapping. Symmetries can either be linked to domains or to morph volumes. In this case, you are associating the symmetries to the morph volumes.

3.

Change 1 plane to cyclical.

4.

Change 180 degrees to set freq.

5.

Set # of cycles to 8.

6.

For syst select the cylindrical coordinate system located at the top of the bottle.

7.

Click create. Note:

8.

A cyclical symmetry is created.

Click return to exit the panel.

Step 4: Split the morph volumes. 1.

On the toolbar, click XZ Left Plane View

2.

From the menu bar, select Morphing > Create > Morph Volumes, then select the split/combine subpanel.

Proprietary Information of Altair Engineering

.

Altair HyperMesh 2019 Tutorials

3.

Set the toggles to split mvols and by edges.

4.

Set single split to 0.8.

5.

Select an edge of Morph Volume 1 (Figure 2).

6.

Click split.

7.

Set single split to 0.2.

8.

Select an edge of Morph Volume 2 (Figure 2).

9.

Click split.

10. Click return to exit the panel.

Figure 2: Splitting morph volumes

Step 5: Morph the part. 1.

From the menu bar select Morphing > Morph, then select the move handles subpanel.

2.

Switch the morphing method from interactive to translate.

3.

Switch the translate option to along xyz.

4.

Set x-val = -5.0.

5.

For system =, select the cylindrical coordinate system located at the top of the bottle.

6.

Select a handle as shown in figure 3.

Proprietary Information of Altair Engineering

p.377

Altair HyperMesh 2019 Tutorials

7.

p.378

Click morph.

Figure 3: Selecting a handle for morphing

As the bead is created, the upper and lower portions of the bottle deform too (figure 4). This is not the intention, as you want to create a bead without affecting the other parts of the bottle.

Figure 4: Morphing using continuous morph volumes

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

8.

Click undo to undo the morphing operation.

Step 6: Update the morph volume edges. To stop this bulging effect of the upper and the lower portions of the bottle, you will use the free edge connectivity between these morph volumes. 1.

From the menu bar select Morphing > Create > Morph Volumes, and then select the update edges subpanel.

2.

Toggle update nodes to update ends.

3.

Switch edge tangency to free.

4.

Update the edges, working your way around the bottle (see figures 5 and 6 below).

Figure 5: Selecting edges to update the tangencies

Figure 6: Changing the tangencies from continuous to free

5.

Click return to exit the panel.

Step 7: Morph the part. 1.

From the menu bar select Morphing > Morph, then select the move handles subpanel.

Proprietary Information of Altair Engineering

p.379

Altair HyperMesh 2019 Tutorials

2.

Verify that the morphing method is translate.

3.

Switch the translate option to along xyz.

4.

Set x-val = -5.0.

5.

For system =, select the cylindrical coordinate system located at the top of the bottle.

6.

Select the handle as shown previously in figure 3.

7.

Click morph.

Figure 7: Bead created with free edge connectivity

Summary Using morph volumes with appropriate tangencies and symmetries you were able to create a bead on the given bottle.

Proprietary Information of Altair Engineering

p.380

Altair HyperMesh 2019 Tutorials

HM-3625: Morph a Symmetric Part onto a New Geometry Objective Update the mesh to a new geometry quickly using symmetry.

Model Files This exercise uses the fe_only.hm and new_design.igs files, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Tools 3-D domains, symmetry, interactive morphing.

Figure 1: Mesh to morph

Proprietary Information of Altair Engineering

p.381

Altair HyperMesh 2019 Tutorials

Step 1: Load the model. 1.

From the menu bar, select File > Open > Model and load the file fe_only.hm.

2.

From the menu bar, select File > Import > Geometry and load the file new_design.igs.

Step 2: Create domains and handles. 1.

From the menu bar, select Morphing > Create > Domains.

2.

Switch the domain type from global domains to 3D domains.

3.

Toggle the element selector to all elements.

4.

Activate the partition 2D domains option.

5.

Click create to create the domains.

6.

Select return to exit the panel.

Step 3: Create symmetries. 1.

From the menu bar, select Morphing > Create > Symmetries to enter the Symmetry panel.

2.

Switch the symmetry type to cyclical.

3.

Switch the symmetry angle from 180 degrees to set freq.

4.

Set the # of cycles to 18.

5.

Click syst.

6.

Select the center point of the gear.

7.

Click domains >> all.

8.

Click create.

9.

Click return.

Step 4: Morph the mesh to the new geometry. 1.

From the menu bar, select Morphing > Morph , then select the move handles subpanel.

2.

Zoom in to one of the cogs of the gear as in the following image:

Figure 2: Mesh, domains handles and the new geometry

Proprietary Information of Altair Engineering

p.382

Altair HyperMesh 2019 Tutorials

3.

Switch the morphing method to move to point.

4.

With from: handle active, select the node depicted in the following image.

5.

With to: point active, select the point on the geometry you want to move the handle to, as depicted in the following image:

Figure 3: Morphing handle to point

As the handles are moved, you will see that the mesh starts conforming to the new geometry.

Figure 4: Mesh mapped onto the new geometry

6.

In the same manner, move the following handles:

Figure 5: Handles to map

Proprietary Information of Altair Engineering

p.383

Altair HyperMesh 2019 Tutorials

7.

Return to the main menu.

Figure 6: Updated (morphed) mesh

Summary Notice how each cog on the gear is updated. Taking advantage of the symmetry in this part, you are able to morph it much quicker.

Proprietary Information of Altair Engineering

p.384

Altair HyperMesh 2019 Tutorials

HM-3630: Morphing with Shapes Model Files This exercise uses the yoke.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Morphing a Yoke via Morph Volumes and Shapes In this exercise you will increase the diameter of one of the prongs of a yoke using morph volumes. You will reflect the shape on to the other prong and finally position the combined shapes from one yoke to the other.

Figure 1: Yoke model

Proprietary Information of Altair Engineering

p.385

Altair HyperMesh 2019 Tutorials

Step 1: Load and review the model. 1.

Open the HyperMesh file yoke.hm.

2.

In the Model Browser, right-click component yoke_2, then select Hide; make sure component yoke_1 is in Show mode.

Step 2: Convert hexas to morph volume. 1.

From the menu bar, select Morphing > Create > Morph Volumes, then select the convert subpanel.

2.

Select elems >> by collector.

3.

Select hexas. Make sure that register all inner nodes is checked.

4.

Click select.

5.

Click convert.

Figure 2: Converting hexas volumes to morph volumes

Note:

All the seven hexa elements are converted into morph volumes.

Step 3: Increase the prong diameter. 1.

In the Model Browser, right-click Tag and select Show to display all the tags.

2.

From the menu bar, select Morphing > Morph, then select the move handles subpanel.

3.

Set the mode selector to move to node.

4.

Click options and make sure morphing>mvols: is set to active (toggle if it is set to inactive).

5.

Click return.

6.

For handle, click Handle 1, and for node, click tag 1’.

Proprietary Information of Altair Engineering

p.386

Altair HyperMesh 2019 Tutorials

7.

Repeat this process for the other 35 handles.

Figure 3: Using tags to change the morph volumes

Step 4: Save the morphed shape. 1.

From the menu bar, select Morphing > Create > Shapes.

2.

Go to the save as shape subpanel.

3.

For name=, enter Prong1.

4.

Toggle as handle perturbations to as node perturbations.

5.

Click create and select Yes to the message which appears.

6.

Click undo all to bring the model to its original position before morphing.

Step 5: Create coordinate system. You need to reference a coordinate system in order to create symmetry. 1.

In the Model Browser, right-click and select Hide for Shape and Morphing Volume. Right click on yoke_1 and select Show.

2.

From the menu bar, select Geometry > Create > Systems > Axis Direction to open the Systems panel, create by axis direction subpanel.

3.

Click origin and select the node labeled "origin."

4.

For X-axis, select the node labeled "X."

5.

For XY plane, select the node labeled "Y."

6.

Click create.

Proprietary Information of Altair Engineering

p.387

Altair HyperMesh 2019 Tutorials

7.

Click return.

Step 6: Create symmetry. 1.

From the menu bar, select Morphing > Create > Symmetries.

2.

For name =, enter symm1.

3.

Under domains, click the check-box for morph volumes. (make sure it is active).

4.

Set 1 plane and keep the rest of the default settings.

5.

Click syst and select the newly created coordinate system.

6.

Click create.

7.

Click return.

Step 7: Reflect shape. 1.

From the menu bar, select Morphing > Create > Shapes.

2.

Change the subpanel to apply shapes.

3.

Under shapes, change apply shapes to reflect shapes.

4.

Change apply only to apply & create.

5.

Keep the default auto-envelope.

6.

Click shapes and select the newly created shape from the previous section.

7.

Under reflect using: click symmetries and select the newly created symmetry.

8.

Click reflect.

Proprietary Information of Altair Engineering

p.388

Altair HyperMesh 2019 Tutorials

Note:

p.389

A reflected shape has been created and applied on the other prong.

The name of the shape, created by reflecting, has the same name as the original shape with a suffix “1.”

Step 8: Position the shapes onto the other yoke. In this step, you will position the shapes of the two prongs of the yoke onto the opposite yoke. 1.

In the Model Browser, right-click Title and select Show.

2.

In the Model Browser right-click yoke_2 and click Show.

3.

In the apply shapes subpanel, under shapes, change reflect shapes to position shapes.

4.

Change the selector from scale to no scale.

5.

Click shapes and select the two shapes present in the model.

6.

Under from: select the three nodes named from_N1, from_N2 and from_N3 for N1, N2 and N3.

7.

Under to: select the three nodes named to_N1, to_N2 and to_N3 for N1, N2 and N3.

8.

Click position.

9.

Click return.

Note:

The two or more shapes have been created and applied to the other yoke. The name of the first new shape (on the other yoke) will have a suffix “2” because it is the second copy of the first shape and the second shape will have a suffix of “11” as it is the first copy of the reflected shape.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.390

HM-3640: Interpolating Loads Using Shapes Model Files This exercise uses the s_bend_tube.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Using Shapes to Interpolate Loads Shapes are one of the most versatile types of the morphing entities. Loads can be converted into shapes and vice versa. When you position shapes, they act on a volume equivalent to the initial volume, but at the new location. In this regard, shapes can be used to interpolate loads on a mesh given the loading at the boundaries of a volume. In this exercise you are given a temperature distribution at points defined by a cube (hexa element). You will use shapes to interpolate the temperatures to the tube lying inside the cube.

Figure 1: Model

Step 1: Load and review the model. Open the HyperMesh file s_bend_tube.hm

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 2: Convert temperatures to shapes. 1.

From the menu bar, select Morphing > Create > Shapes, then select the Convert subpanel.

2.

Switch the conversion type to temperature to shapes.

3.

For loadcols, select temperature.

4.

Click select.

5.

Click convert.

Figure 2: Temperature converted in shape vectors

Note:

The temperature loads have been converted into shape vectors.

The shape vectors are proportional to the temperature loads on the corners of the cube and the distances from those corners. The name of the converted shape is the same as the temperature load collector.

Proprietary Information of Altair Engineering

p.391

Altair HyperMesh 2019 Tutorials

Step 3: Translate the shape. 1.

Click the apply shapes subpanel.

Figure 3: The base and the node for translating the shape

2.

Change the operation to translate shapes.

3.

Change apply only to create new.

4.

For envelope, use auto-envelope.

5.

For shapes, select temperature.

6.

Click select.

7.

For from: base, select the node shown in Figure 3.

8.

For to: nodes, select the node shown in Figure 3.

9.

Click translate. The shape has been transferred to the tube. You selected the same base and to node, effectively selecting a translate distance of 0. A new shape is created with the suffix 1 (temperature1).

Step 4: Convert shape vectors to temperature loads. 1.

Click the convert subpanel.

2.

Switch the conversion type to shapes to temperatures.

3.

For shapes, select temperature1.

Proprietary Information of Altair Engineering

p.392

Altair HyperMesh 2019 Tutorials

4.

Click select.

5.

Click convert. The shape has been converted into temperature load.

Step 5: Check the result. 1.

In the Model Browser, right-click and select Hide for Shape.

2.

In the Model Browser, right-click component cube and select Hide.

3.

In the Model Browser, right-click LoadCollector and select Hide.

4.

From the BCs menu, select Contour Loads. Make sure you expand the Contour Loads utility appropriately to visualize all the buttons.

5.

From the list of loads, select temperature1.

6.

Click Accept. This takes you to the Contour panel.

7.

Select simulation = temperature1.

8.

Select data type = Temperature.

9.

Click contour.

Figure 4: The contoured temperature results

Proprietary Information of Altair Engineering

p.393

Altair HyperMesh 2019 Tutorials

Summary Using shapes you have been able to interpolate temperatures from the corners of a volume on to an object located in that volume.

Proprietary Information of Altair Engineering

p.394

Altair HyperMesh 2019 Tutorials

HM-3650: Creating Shapes Using Record Model Files This exercise uses the floor.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Recording Shapes The Record panel gives you the flexibility of making changes to the mesh using panels outside the HyperMorph module and saving them as shapes. In this exercise you will change a bead using the Node Edit > align node subpanel and record the shape function. You will then reflect the shape to the other side of the mesh to complete the mesh update.

Figure 1: Location to record the nodal movements on and reflect

Step 1: Load and review the model. Open the HyperMesh file floor.hm.

Proprietary Information of Altair Engineering

p.395

Altair HyperMesh 2019 Tutorials

p.396

Step 2: Start recording nodal movements. 1.

From the menu bar select Morphing > Free Hand, then select the record subpanel.

2.

Click start.

3.

Click return.

Step 3: Change the bead profile. 1.

From the menu bar, select Geometry > Edit >Nodes > Align to enter the align node subpanel.

2.

Select the nodes shown below for the 1st end and 2nd end.

Figure 2: first set of nodes to align

3.

Select the nodes between the selected nodes to align the nodes to the 1st end: and 2nd end: nodes.

4.

Repeat the same process to align the next row of nodes (figure 3).

Figure 3: Second set of nodes to align

5.

Select the nodes between the selected nodes to align the nodes to the 1st end and 2nd end nodes.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

Repeat the same process to align the next row of nodes (figure 4).

Figure 4: Third set of nodes to align

7.

Click return to exit the panel.

Step 4: Stop the recording. 1.

From the menu bar select Morphing > Free Hand, then select the record subpanel.

2.

Click finish. This stops the record process.

Step 5: Save the morphed shape. 1.

Go to the save shape subpanel.

2.

Set name= Morph1.

3.

Toggle save option to as node perturbations.

4.

Click save.

5.

Click undo all to bring the model to its original position before morphing.

Proprietary Information of Altair Engineering

p.397

Altair HyperMesh 2019 Tutorials

Step 6: Create coordinate system. 1.

From the menu bar select Geometry > Create > Systems > Axis Direction.

2.

For origin select the node with tag origin. •

For x-axis select the node with tag x-axis.

•

For xy-plane select the node with xy-plane.

3.

Click create.

4.

Click return to exit the panel.

Step 7: Create symmetry. 1.

From the menu bar select Morphing > Create > Symmetries.

2.

Set name = symm1.

3.

For symmetry type use 1 plane.

4.

For align with use x-axis.

5.

Select the syst created in step 6.

6.

Click create. Note that 1 plane symmetry is created with a square symbol.

7.

Click return to exit the panel.

Proprietary Information of Altair Engineering

p.398

Altair HyperMesh 2019 Tutorials

Step 8: Reflect shape. 1.

From the menu bar select Morphing > Create > Shapes, then select the apply shapes subpanel.

2.

Under shape change the option to reflect shapes.

3.

Under reflect shapes change the option to apply & create.

4.

For shape, select Morph1.

5.

For symmetries, select symm1.

6.

Click reflect.

Summary The shape (Morph1) is reflected to the other side. Also, the reflected shape has the same name with the suffix 1. The changes that you made on one side are thus transferred to the other side.

Proprietary Information of Altair Engineering

p.399

Altair HyperMesh 2019 Tutorials

HM-3660: Maintaining Area Using Constraints Model Files This exercise uses the windshield.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Using Morph Constraints to Keep the Area of a Windshield Constant while Changing its Shape In this exercise will change the shape of the windshield while keeping its area constant.

Figure 1: Windshield mesh

Step 1: Load and review the model. Open the HyperMesh file windshield.hm.

Step 2: Create a shape to define the degree of freedom for the mesh. 1.

From the menu bar select Morphing > Free Hand and select the move nodes subpanel.

2.

Switch the method to translate.

3.

Key in

4.

•

x = 0;

•

Y = -5 (negative 5);

•

Z=0

Under moving nodes: click nodes >> by sets and select move_node.

Proprietary Information of Altair Engineering

p.400

Altair HyperMesh 2019 Tutorials

5.

Click select.

6.

Under fixed nodes: click nodes >> by sets and select fix_node.

7.

Click select.

8.

Under affected elements: click elems >> displayed.

9.

Click morph.

10. Go to the save shape subpanel. 11. For name =, enter Shape1. 12. Toggle the save option to as node perturbations. 13. Click save. 14. Click undo all to bring the model to its original position before morphing. This initial shape defines the direction in which the nodes have the freedom to move, as the shape of the windshield is changing, thus enabling us to keep the area at a constant.

Step 3: Create a constraint. 1.

From the menu bar select Morphing > Create > Morph Constraints.

2.

Set name = const1.

3.

Change the constraint type to area.

4.

For shapes, select Shape1.

5.

Select elems >> displayed.

6.

Switch the area option to equal to.

7.

Click calculate to calculate the area of the mesh: Note:

The value shows in the area box is: 1.085e+06.

This is the actual surface area of the windshield which will be maintained. 8.

Click create.

Note: 9.

The constraint is created. The symbol for the constraint is a matching-mesh.

Right-click Shape and select Hide in the Model Browser.

10. Right-click MorphingConstraint and select Hide in the Model Browser.

Proprietary Information of Altair Engineering

p.401

Altair HyperMesh 2019 Tutorials

p.402

Step 4: Create morph volume. 1.

From the menu bar select Morphing > Create > Morph Volumes.

2.

Switch the method to create morphvol.

3.

Toggle entity type to enclose elems.

4.

Select elems >> displayed.

5.

Toggle coordinate system to global system.

6.

Click create. The morph volume is created.

Step 5: Morph the part. 1.

From the menu bar select Morphing > Morph and select the move handles subpanel.

2.

Change the morph type to move to node.

3.

For from: handle, select handle1 (Figure 2).

4.

For from: node, select node1 (Figure 2).

5.

Repeat the process for the other handles and nodes.

Figure 2: From handles and from nodes

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 6: Save the morphed shape. 1.

Click the save shape radio button.

2.

Set name = Shape2.

3.

Toggle the save option to as node perturbations.

4.

Click save.

Step 7: Check the result. 1.

Right-click MorphingVolume in the Model Browser and select Hide.

2.

Go to View > Toolbars, make active Checks toolbar , select the Mass/Area Calc (

) icon.

3.

For comps, select windshield.

4.

Click select.

5.

Click calculate. The final area of the windshield is 1.085e+06, which is the same as the initial area. So, even though the profile of the windshield has changed, its area has not. As the height of the windshield reduced, it expanded in the direction provided by Shape1.

Summary Using morph constraints, you able to change the shape of the windshield, while keeping its area constant.

Proprietary Information of Altair Engineering

p.403

Altair HyperMesh 2019 Tutorials

HM-3670: Positioning a Dummy Using Limiting Constraints Model Files This exercise uses the dummy.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Using Limiting Constraints and Freehand Morphing to Position a Dummy and Morph the Seat In this exercise, you will learn to position the H-point of the dummy on a seat cushion. This helps to reduce design and remeshing of the seat based on the pre-stress analysis. To do this exercise you will be using a limiting constraint and freehand morphing.

Figure 1 Model with Seat cushion and dummy

Step 1: Load and review the model. Open the HyperMesh file dummy.hm

Step 2: Create constraints. 1.

From the menu bar select Morphing > Create > Morph Constraints.

2.

Set name= const1.

3.

Set type of constraint to on elements.

4.

Set the option under nodes to bounded.

Proprietary Information of Altair Engineering

p.404

Altair HyperMesh 2019 Tutorials

5.

Set project along: to N1,N2 along negative z (choose from side of cushion).

6.

Set distance= 2. This will ensure that there is a distance of 2 units between the dummy and the seat after the morphing is complete.

7.

Use nodes >> by collector and select cushion.

8.

Click select.

9.

Use elems >> by collector and select dummy.

10. Click select. 11. Click create. Constraints with a diamond shape are created.

Figure 2 Morphing Constraints on Seat cushion and dummy

Step 3: Morph the part. 1.

Right-click MorphingConstraint in the Model Browser and select Hide.

2.

From the menu bar, select Morphing > Free Hand and select the move nodes subpanel.

3.

Switch moving method to translate.

4.

For moving nodes, use nodes >> by collector and select cushion.

5.

Click select.

Proprietary Information of Altair Engineering

p.405

Altair HyperMesh 2019 Tutorials

6.

For fixed nodes, use nodes >> by collector and select dummy.

7.

Click select.

8.

For affected elements, use elems >> by collector and select cushion.

9.

Click select.

10. For the translate magnitude, set •

x=0

•

y=0

•

z = 80

11. Click morph. The top surface of the cushion has conformed to the shape of the dummy. The distance between the dummy and the seat-cushion is 2 mm.

Summary Using limiting constraints, you are able to move a mesh such that it moves an adjoining mesh along with it, thus preventing penetration between the two of them.

Proprietary Information of Altair Engineering

p.406

Altair HyperMesh 2019 Tutorials

HM-3680: Preserving a Shape Using Cluster Constraints Model Files This exercise uses the truck.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Using Cluster Constraints to Preserve the Wheel Shape while Lengthening the Body of a Truck When circular features are stretched, they become elliptical in shape. In some cases as in the wheels of a truck, this effect is not desirable. In such cases, using cluster constraints will allow you to translate the features, along with the morph, while maintaining its circular shape. In the exercise you will be changing the length of the cab while preserving the shape of the wheel. To facilitate the morphing process you will be employing constraint and symmetry.

Figure 1: Truck model

Step 1: Load and review the model. Open the HyperMesh file truck.hm.

Step 2: Create a coordinate system. 1.

Using the menu bar select Geometry > Create > Systems > Axis Direction.

2.

For origin select the node with tag origin.

3.

For x-axis, select node with tag x-axis.

4.

For xy-plane, select node with xy-plane.

5.

Click create to create the coordinate system.

Proprietary Information of Altair Engineering

p.407

Altair HyperMesh 2019 Tutorials

6.

On the toolbar, select XZ Right Plane View (

7.

Click return to exit the panel.

p.408

)

Step 3: Create and split the morph volume. 1.

From the menu bar select Morphing > Create > Morph Volumes.

2.

Switch the creation method to create morphvol.

3.

Set entity type to enclose elements.

4.

Select elems >> all.

5.

Set system to global system.

6.

Set buffer % = 5. The morph volume is created.

7.

Click create to create the morph volume.

8.

Click the split/combine subpanel.

9.

Toggle the operation to split mvols.

10. Toggle to split the morph volume by edges. 11. Toggle the type of split to single split. 12. Set single split = 0.44. 13. Select the morph volume in the graphics window.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.409

14. Click split to split the morph volume. The original morph volume is now split into two morph volumes. 15. Click return to exit the panel.

Step 4: Create a Symmetry. 1.

From the menu bar select Morphing > Create > Symmetries:

2.

For name =, enter symm1.

3.

Under domain, check the box for morph volumes. Symmetry can be linked to either domains or morph volumes. In this exercise since you are dealing with morph volumes you will use the check to link the symmetry to the morph volume.

4.

Switch the symmetry type to 1 plane.

5.

For syst, select the coordinate system created in step 4.2.

6.

Click create to create the symmetry. A 1 plane symmetry with a square symbol has been created.

7.

Click return to exit the panel.

Step 5: Morph the part. 1.

From the menu bar select Morphing > Morph, then click the move handles subpanel.

2.

Switch the morphing mode to translate.

3.

Switch the along option to along xyz.

4.

Set the following values: •

X val = 500

•

Y val = 0

•

Z val = 0

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

5.

Select two handles as shown in figure 3.

6.

Click morph to morph the front half of the truck.

Figure 2.1 Front half of the truck to morph

Figure 2.2 Front half of the truck morphed

The front end is stretched 500 units. Since the front wheels are also the part of the morph volumes they became elliptical after morphing. This is not desirable. You will undo this morphing, constrain the wheels and re-do it.

Figure 3: undesired morphing of the front wheel

Proprietary Information of Altair Engineering

p.410

Altair HyperMesh 2019 Tutorials

7.

Undo all morphs.

Step 6: Create a cluster constraint. As seen in the previous image, the front wheels, after morphing, become elliptical. To fix this issue, you will be employing a particular type of constraint, called a cluster constraint, which helps to keep the original shape of a portion of the model while morphing. 1.

From the menu bar select Morphing > Create > Morph Constraints.

2.

Set name = const2.

3.

Switch the constraint type to cluster.

4.

Select nodes >> by collector .

5.

Select comps >> by id.

6.

Use id = 1-8 and then hit ENTER on the keyboard.

7.

Click select to select the components.

8.

Click create to create the cluster constraint. The cluster constraints are created on the nodes of the selected components.

Figure 4

9.

Click return to exit the panel.

10. In the Model Browser, right-click MorphingConstraint and click Hide to turn off the constraints.

Proprietary Information of Altair Engineering

p.411

Altair HyperMesh 2019 Tutorials

Step 7: Morph the part. Repeat the procedure in Step 5 to morph the front of the truck by 500 units. The front end is stretched 500 mm. The front wheels are moved in the morphing process while maintaining their circular shape.

Summary Using cluster constraints and morph volumes you are able to stretch the cab of the pickup without distorting the wheels.

Proprietary Information of Altair Engineering

p.412

Altair HyperMesh 2019 Tutorials

p.413

HM-3690: Remeshing Domains After Morphing Model Files This exercise uses the arm2D.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise: Remeshing Domains After Morphing Depending on the morphing being performed, there is a possibility that the mesh can get distorted. For such cases, HyperMorph provides a remeshing capability. The advantage of this remeshing is that the newly created elements are automatically a part of the original domain. This provides continuity to the morphing process along with proper element quality.

Figure 1: Model

Step 1: Load and review the model. Open the HyperMesh file arm2D.hm.

Step 2: Set the morph options. 1.

From the menu bar select Morphing > Assign > Morph Options.

2.

Select the auto qa subpanel.

3.

Switch auto quality check to 2D jacobian.

4.

Set limit = to 0.7.

Step 3: Create domains and handles. 1.

From the menu bar select Morphing > Create > Domains.

2.

Switch the creation type to 2D domains.

3.

Switch from all elems to elems.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

Use elems >> by sets and select set_1.

5.

Click select.

6.

Click create to create the domain.

7.

Use elems >> by sets and select set_2.

8.

Click select.

9.

Click create to create the domain. Note:

Two 2D domains are created.

Step 4: Translate the washer. 1.

From the menu bar select Morphing > Morph, then select move handles.

2.

Switch the mode to translate.

3.

Switch the along option to along vector.

4.

Select N1 and N2 as shown in figure 2.

Figure 2: Selecting N1 and N2 for the translate vector

5.

Set dist = 0.25.

Proprietary Information of Altair Engineering

p.414

Altair HyperMesh 2019 Tutorials

6.

Select the two handles on the washer.

7.

Click morph to morph the washer.

p.415

The elements outside the washer get compressed as the washer moves. Also, as the elements fail (jacobian < 0.7) they are highlighted (figure 3).

Figure 3: Elements after morphing and quality check on Jacobian 2D

Step 5: Remesh the domain. 1.

From the menu bar select Morphing > Create > Domains and then select the update subpanel.

2.

Switch the update option to remesh 2D/3D.

3.

Switch new mesh type: to quads.

4.

Select both 2-D domains on the model.

5.

Click calc avg to get the average element size.

6.

Click remesh to remesh the domain.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.416

Figure 4: Updated mesh and quality check

The mesh is updated.

Summary Using this technique, you can update the mesh in regions that might have undergone excessive elemental deformation during morphing. Since the domains and handles are maintained, it allows you to conduct further morphing if need be.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Analysis Setup

Proprietary Information of Altair Engineering

p.417

7

Altair HyperMesh 2019 Tutorials

p.418

HM-4000: Setting up Loading Conditions In this tutorial, you will learn how to: •

Create constraints (OPTISTRUCT SPC) on the channel’s geometry lines

•

Create a force (OPTISTRUCT FORCE) on the bracket to simulate a pressing load on it

•

Define a load step (OPTISTRUCT SUBCASE)

•

Export the model to an OptiStruct input file

•

Submit the OptiStruct input file to OptiStruct

•

Review the resulting HTML report file

The purpose of using a finite element (FE) pre-processor is to create a model, which can be run by a solver. A finite element solver can solve for responses of parts to loading conditions on them. The loads can be in the form of boundary constraints, forces, pressures, temperatures, and so on. In this tutorial, you will gain an understanding of the basic concepts for creating a solver input file by using a template. More specifically, you will learn how to define loading conditions on a model, specify solver specific controls, and submit an input file to a solver from HyperMesh.

Model Files This exercise uses the channel_brkt_assem_loading.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory. The model contains the bracket and channel assembly in the following image.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.419

Exercise: Setting up Loading Conditions

Step 1: Load the OptiStruct user profile. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select OptiStruct.

3.

Click OK.

Step 2: Retrieve and view the HyperMesh model file, channel_brkt_assem_loading.hm. 1.

Open a model file by clicking File > Open > Model from the menu bar, or clicking on the Standard toolbar.

2.

In the Open Model dialog, open the channel_brkt_assem_loading.hm file. A model appears in the graphics area.

Step 3: Create two load collectors named pressing_load and constraints. 1.

In the Model browser, right-click and select Create > Load Collector from the context menu. HyperMesh creates and opens a load collector in the Entity Editor.

2.

In the Entity Editor: •

For Name, enter pressing_load.

•

Click the Color icon, and select a color for the load collector.

•

Set Card Image to .

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

p.420

Repeat steps 3.1 and 3.2 to create second load collector labeled constraints.

Step 4: Apply constraints (OPTISTRUCT SPC) to the channel’s line geometry. 1.

In the Model browser, View folder, right-click on View2 and select Show from the context menu. Note:

By selecting this view, HyperMesh sets the component's and load collector's displays back to what they were when the view was saved. The load collectors that you created in step 3 are now turned off because they did not exist when the view was saved. You will need to turn these back on to see the display of the BCs when you create them in the next steps.

2.

In the Load Collector folder, click on the display of their geometry.

3.

In the Component folder, click geometry.

4.

Open the Constraints panel by clicking BCs > Create > Constraints from the menu bar.

5.

Go to the create subpanel.

6.

Set the entity selector to lines.

Proprietary Information of Altair Engineering

next to pressing_load and constraints to turn next to channel to turn on the display of its

Altair HyperMesh 2019 Tutorials

7.

Select the six lines on the perimeter of the channel’s bottom surface as indicated in the following image.

8.

Verify that all six dofs (degrees of freedom) are selected. Note:

9.

p.421

For an OptiStruct linear static analysis, dof 1, 2, and 3 represent translations in the global x-, y-, and z-directions, respectively. Dof 4, 5, and 6 represent rotations about the global x-, y- and z-axis, respectively.

Click load types = and select SPC.

10. Click create. Hypermesh creates constraints on the lines.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

11. In the size = field, enter 5. HyperMesh reduces the display size of the constraints. 12. Select the label constraints checkbox. HyperMesh displays a label for each constraint. Note:

The labels identify what dofs are assigned to the constraints.

13. Exit the main menu by clicking return.

Step 5: Map the constraints (OPTISTRUCT SPC) on the geometry lines to the channel nodes associated to the lines. 1.

Open the loads on geometry panel by clicking BCs > Loads on Geometry from the menu bar.

2.

Click loadcols.

3.

Select the load collector, constraints.

4.

Click select.

5.

Click map loads. HyperMesh creates a constraint at each node associated to the geometry lines.

6.

Click return.

7.

In the Model browser, Component folder, turn off the display of geometry for all component collectors.

Proprietary Information of Altair Engineering

p.422

Altair HyperMesh 2019 Tutorials

Step 6: Prepare to create forces (OPTISTRUCT FORCE) on the bracket for the pressing load case. 1.

In the Model browser, View folder, right-click on View3 and select Show from the context menu.

2.

In the Load Collector folder, right-click on pressing_load and select Make Current from the context menu. Note:

3.

The pressing_load load collector is now the current load collector, and any loads created will be placed in this collector.

Right-click on pressing_load and select Show from the context menu.

Step 7: Create two forces (OPTISTRUCT FORCE) on the bracket for the pressing load case. 1.

Open the forces panel by clicking BCs > Create > Forces from the menu bar.

2.

Go to the create subpanel.

3.

Set the entity selector to nodes.

4.

Select the two nodes indicated in the following image.

5.

In the magnitude = field, enter 5.

6.

Set the orientation selector to y-axis.

7.

Click load types = and select FORCE.

8.

Click create. HyperMesh creates two forces.

9.

In the magnitude % = field, enter 200.0. HyperMesh increases the display size of the forces.

Proprietary Information of Altair Engineering

p.423

Altair HyperMesh 2019 Tutorials

10. Select the label loads checkbox. Each force displays the label FORCE = 5.00e+00.

The two forces created for the pressing load case

11. Click return.

Step 8: Define the load step for the pressing load case. 1.

Create a Load Step by right-clicking in the Model browser and selecting Create > Load Step from the context menu. HyperMesh creates and opens a load step in the Entity Editor.

2.

In the Entity Editor: •

For Name, enter pressing_step.

•

Set Analysis type to Linear Static.

Proprietary Information of Altair Engineering

p.424

Altair HyperMesh 2019 Tutorials

•

For SPC, click Unspecified >> Loadcol.

•

In the Select Loadcol dialog, select constraints and then click OK.

•

For LOAD, click Unspecified >> Loadcol.

•

In the Select Loadcol dialog, select pressing_load and then click OK.

p.425

Step 9: Display and mask the load step (the load collectors defined in the load step). 1.

In the Model browser, Load Step folder, right-click on pressing_step and select Hide from the context menu. HyperMesh hides the pressing_load and constraints load collector

2.

Right-click on pressing_step again and select Show from the context menu.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.426

HM-4010: Formatting Model for Analysis In this tutorial, you will learn how to: •

Create a solver input file by using a template

•

Review entities in HyperMesh to see how they will appear in the solver input file

•

Define materials and properties

•

Select solver element types for HyperMesh element configurations

The purpose of using a finite element (FE) pre-processor is to create a model that can be run by a solver. HyperMesh interfaces with many FE solvers and all of them have unique input file formats. HyperMesh has a unique template(s) for each solver it supports. A template contains solver specific formatting instructions, which HyperMesh uses to create an input file for that solver.

Model Files This exercise uses the channel_brkt_assem_analysis.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory. The model contains the bracket and channel assembly in the following image.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.427

Exercise: OptiStruct Linear Statics Setup for a Shell Assembly

Step 1: Load the OptiStruct user profile. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select OptiStruct.

3.

Click OK.

Step 2: Retrieve and view the file, channel_brkt_assem_analysis.hm. 1.

Open a model file by clicking File > Open > Model from the menu bar, or clicking on the Standard toolbar.

2.

In the Open Model dialog, open the channel_brkt_assem_analysis.hm file. A model appears in the graphics area.

Step 3: Review a bracket element to identify what type of OptiStruct element it is and to see how it will be formatted in the OptiStruct input file. 1.

Open the Card Edit panel by clicking

2.

Set the entity selector to elems.

3.

In the graphics area, select an element on the bracket component. Note:

4.

on the Collectors toolbar.

The bracket component is blue.

Click edit. The Card Image opens, and indicates that the selected element is an OptiStruct CQUAD4 or CTRIA3, depending on whether you selected a quad or tria element. Note:

EID is the element’s ID, PID is the ID of the element’s property, and G(X) is the grid (node) ID that makes up the element. Options specific to the CQUAD4 or CTRIA3 appear in the menu panel area.

5.

Close the Card Image by clicking return.

6.

Exit the Card Edit panel by clicking return.

Step 4: Review and edit the existing steel material’s card image by accessing the card editor from the Model browser. This material is defined for the channel. 1.

In the Model browser, Material folder, click steel. The Entity Editor opens and displays the material's corresponding data. Note:

The card image indicates the material is of OptiStruct type MAT1.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

In the Entity Editor, NU (Poisson's Ratio) field, change the value from 0.3 to 0.28.

Step 5: Define a material collector named aluminum for the bracket. This material is defined for the channel. 1.

In the Model browser, right-click and select Create > Material from the context menu. HyperMesh creates and opens a material in the Entity Editor.

Proprietary Information of Altair Engineering

p.428

Altair HyperMesh 2019 Tutorials

2.

For Name, enter aluminum.

3.

Set Card Image to MAT1.

4.

For E (Young's Modulus), enter 7.0e4.

5.

For NU (Poisson's Ratio), enter 0.33.

Step 6: Define a property collector (PSHELL card image) that will be assigned to the channel component collector. 1.

In the Model browser, right-click and select Create > Property from the context menu. HyperMesh creates and opens a property in the Entity Editor.

2.

For Name, enter channel.

3.

Set Card Image to PSHELL.

4.

For Material, click Unspecified >> Material.

Proprietary Information of Altair Engineering

p.429

Altair HyperMesh 2019 Tutorials

5.

In the Select Material dialog, select steel and then click OK. HyperMesh assigns the material.

6.

For T (thickness), enter 3.0.

p.430

Step 7: Assign the channel property to the channel component. 1.

In the Model browser, Component folder, click channel. The Entity Editor opens and displays the component's corresponding data.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

For Property, click Unspecified >> Property.

3.

In the Select Property dialog, select channel and then click OK. HyperMesh assigns the property channel to the component channel.

Step 8: Update the bracket property to have a PSHELL card image, a thickness of 2.0, and the aluminum material. 1.

In the Model browser, Property folder, click bracket. The Entity Editor opens and displays the properties' corresponding data.

2.

Set Card Image to PSHELL.

3.

For Material, click Unspecified >> Material.

4.

In the Select Material dialog, select aluminum and then click OK. HyperMesh assigns the material aluminum to the property bracket.

Proprietary Information of Altair Engineering

p.431

Altair HyperMesh 2019 Tutorials

5.

p.432

For T (thickness), enter 2.0.

Step 9: Calculate the section properties for the bar elements (OptiStruct CBEAM) by using HyperBeam. 1.

Open the HyperBeam panel by clicking Properties > HyperBeam from the menu bar.

2.

Go to the standard section subpanel.

3.

Set the standard section library to HYPERBEAM.

4.

Set the standard section type to solid circle.

5.

Click create. HyperMesh invokes the HyperBeam module. Note:

The solid, green circle represents the cross section. Under the local coordinate system you should see the number, 10.0000, which is the circle’s radius.

HyperBeam module with the standard solid circle section

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

Under Parameter Definition, click the Value field next to Radius (r) and change the value from 10 to 3. HyperMesh updates the values in the Data pane to reflect the circle's new diameter.

7.

In the Model browser, right-click on circle_section.1 and select Rename from the context menu.

8.

In the editable field, rename the section 6mm_Beam_Sect.

9.

Close the HyperBeam module and return to your HyperMesh session by clicking File > Exit from the menu bar.

10. Return to the main menu by clicking return.

Step 10: Create a property collector named bars_prop for the bar elements (OptiStruct). 1.

In the Model browser, right-click and select Create > Property from the context menu. HyperMesh creates and opens a property in the Entity Editor.

2.

For Name, enter bars_prop.

3.

Set Card Image to PBEAM.

4.

For Material, click Unspecified >> Material.

5.

In the Select Material dialog, select steel and then click OK. HyperMesh assigns the material steel to the property bars_prop.

6.

For Beam Section, click Unspecified >> Beamsection.

Proprietary Information of Altair Engineering

p.433

Altair HyperMesh 2019 Tutorials

7.

In the Select Beam Section dialog, select 6mm_Beam_Sect and then click OK. HyperMesh assigns the beam section, and populates the parameter fields in the PBEAM card with the data in the 6mm_Beam_Sect beam section.

Step 11: Update the CBEAM elements in the bolts component to use the PBEAM Property. 1.

In the Model browser, Component folder, click bolts. The Entity Editor opens and displays the component's corresponding data.

2.

For Property, click Unspecified >> Property.

Proprietary Information of Altair Engineering

p.434

Altair HyperMesh 2019 Tutorials

3.

In the Select Property dialog, select bars_prop and then click OK. HyperMesh assigns the property bars_prop to the component bolts.

Step 12: Define a H3D file to be output from OptiStruct by using the control cards panel. 1.

Open the Control Cards panel by clicking Setup > Create > Control Cards from the menu bar.

2.

In the Card Image, select the control card FORMAT. Note:

3.

In the card image, the FORMAT line is set to H3D. This specifies OptiStruct to output results to a Hyper3D (H3D) file, which can be viewed in the HyperView Player. A HTML report file will be output and the H3D file will be embedded in it.

In the number_of_formats = field, enter 2. A second FORMAT line appears in the card image.

Proprietary Information of Altair Engineering

p.435

Altair HyperMesh 2019 Tutorials

4.

In the second FORMAT line, click H3D and then select HM. Note:

5.

This option specifies OptiStruct to output the results to a HyperMesh binary results file, allowing the results to be post-processed within HyperMesh.

Exit to the Control Cards panel by clicking return. Note:

6.

p.436

The FORMAT button is now green, which indicates that the card will be exported to the OptiStruct input file.

Return to the main menu by clicking return.

Step 13: Export the model to an OptiStruct input file. 1.

From the menu bar, click File > Export > Solver Deck.

2.

In the File field, click

3.

In the Select OptiStruct file dialog, navigate to your working directory and save the file as channel_brkt_assem_loading.fem.

4.

Click Export. HyperMesh exports the model as an OptiStruct .fem input file for the solver specified by the current user profile.

.

Step 14: Review the contents of the file channel_brkt_assem_loading.fem. 1.

In any text editor (Notepad, Wordpad, Vi, etc.), open the file channel_brkt_assem_loading.fem.

2.

Near the top of the file, note the following: •

The line FORMAT HM, which you specified in HyperMesh

•

The load step (OptiStruct SUBCASE) named pressing_step which you defined in HyperMesh

•

Under the load step, the load collector ids (OptiStruct load and constraint set identification numbers)

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

Search for "FORCE."

4.

Note the load set identification number for each force (OptiStruct FORCE). It is either 1 or 2 as shown below. These numbers correspond to the numbers under the load steps in the file.

5.

Search for "SPC" (HyperMesh constraint).

6.

Note the constraint set identification number for each constraint (OptiStruct SPC). It is 2 as shown below, which lists a few of the constraints. This number corresponds to the number under the load steps in the file.

7.

Search for the load collector name "pressing_load."

8.

Note the load collectors, pressing_load and constraints. Also, note their collector ID and color ID. When the model is imported into HyperMesh, the loads are organized into these load collectors and have these IDs and colors.

9.

Close the file channel_brkt_assem_loading.fem.

Step 15 (Optional): Save your work. With the exercise completed, you can save the model as a HyperMesh file, if desired.

Proprietary Information of Altair Engineering

p.437

Altair HyperMesh 2019 Tutorials

HM-4020: Obtaining and Assigning Beam Cross-Section Properties using HyperBeam In this tutorial you will learn how to: •

Obtain beam section properties for various types of beam cross-sections using HyperBeam, a module within HyperMesh

•

Populate the fields of property collectors with beam properties

•

Assign a property collector to a beam element you create

In FEA, beams are typically modeled as 1D elements. In this tutorial you will become familiar with the modeling of beam sections for 1D elements (beam, bar, and rod) in HyperMesh. The focus is on obtaining and assigning beam-section properties, not on creating beam elements themselves.

Model Files This exercise uses the hyperbeam.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Model geometry

The model geometry represents different types of cross-sections used in this tutorial: standard, shell, and solid. The model consists of a solid cylinder attached to a hollow trapezoidal structure, which is further joined to an irregularly shaped solid component (see previous image).

Proprietary Information of Altair Engineering

p.438

Altair HyperMesh 2019 Tutorials

Exercise: Obtaining and Assigning Beam Cross-Section Properties using HyperBeam

Step 1: Load the OptiStruct user profile. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select OptiStruct.

3.

Click OK.

Step 2: Retrieve and view the file, hyperbeam.hm. 1.

Open a model file by clicking File > Open > Model from the menu bar, or clicking on the Standard toolbar.

2.

In the Open Model dialog, open the hyperbeam.hm file. A model appears in the graphics area. Note:

This model's geometry represents different types of cross-sections: standard, shell, and solid. In the following step you will create a standard circular section to represent the cross-section of the cylinder, a shell section with lines to represent the cross-section of the hollow trapezoidal feature, and a solid section with lines to represent the cross-section of the solid irregular feature. This model is organized into four collectors: one contains all of the surfaces, two contain the lines for the shell-section and the solid-section, respectively, and the last component stores beam elements.

Step 3: Model a standard circular section using HyperBeam. In this step, use the standard section subpanel in the HyperBeam panel to quickly model a solid circular section. In order to define a circular cross-section, HyperBeam requires the diameter of the crosssection as input. Measure the diameter of the section before invoking HyperBeam using the Distance panel from the Geom page. 1.

Use the nodes panel to create three nodes on the circle defining the base of the solid cylinder. •

From the menu bar, click Geometry > Create > Nodes > Extract on Line.

•

Using the lines selector, select the circular line defining the base of the cylinder.

•

In the number of nodes field, enter 3.

•

Click create. HyperMesh generates three nodes on the line, two of which are located at the same location (since the circular line is a line that closes upon itself).

•

Click return.

Note:

With the two independent locations left, you can measure the diameter.

Proprietary Information of Altair Engineering

p.439

Altair HyperMesh 2019 Tutorials

Nodes on circle to measure diameter

2.

3.

Use the Distance panel to measure the distance between the two nodes diametrically opposed. •

From the menu bar, click Geometry > Check > Nodes > Distance.

•

Go to the two nodes subpanel.

•

Use the N1 and N2 selectors to select the two nodes, which are diametrically opposed, on the circular line that defines the base of the cylinder. The distance= field reads 110 units, which indicates the distance between the two nodes and the diameter of the circle.

•

Click return.

Use the HyperBeam panel to create a solid circle standard section. •

From the menu bar, click Properties > HyperBeam.

•

Go to the the standard section subpanel.

•

Set the standard section library to HYPERBEAM.

•

Set the standard section type to solid circle.

•

Click create. The HyperBeam module opens with a solid circle cross-section displayed in the center panel. The left pane (HyperBeam view) lists the crosssections defined in the model, and the right pane (Results window) displays the results for the various beam properties computed for the dimensions displayed.

Proprietary Information of Altair Engineering

p.440

Altair HyperMesh 2019 Tutorials

HyperBeam window (standard section)

4.

Modify the diameter of the cross-section. •

Under Parameter Definition, click the Value field next to Radius (r).

•

In the editable field, enter 55 and then press ENTER. The value of the diameter updates, along with the quantities computed for the cross-section in the Results window. These properties are calculated based on the dimensions that were input. For example, HyperBeam calculates the area of this cross-section, its moments of inertia, and its torsional constant.

Note: 5.

6.

Alternatively, drag the graphical handles, which represent the diameter of the cross-section, until the diameter changes to the desired value.

Assign the name “Solid Circle” to this cross-section in the HyperBeam view. •

In the HyperBeam view, right-click on the name of the cross-section under the auto1 folder and select Rename from the context menu.

•

In the editable field, enter Solid Circle and press ENTER.

Return to HyperMesh by clicking File > Exit from the menu bar. The information that was computed is automatically stored in a beamsect collector with the name you specified for the section. This beamsect collector will later be used to populate the fields of a property card.

Proprietary Information of Altair Engineering

p.441

Altair HyperMesh 2019 Tutorials

Note:

Since geometry information was available, this cross-section could have been defined as a solid section using the solid section subpanel. A standard section was used instead because it did not require selection, although it required a diameter measurement.

You may save your HyperMesh model to your working directory at this point. In this step, a beam cross-section for standard sections was created using HyperBeam. You also learned how to specify the dimensions for the standard section, and how to save this section for subsequent use.

Step 4: Model a shell section. In this step, use the shell section subpanel of the HyperBeam panel to model a beam section for the trapezoidal feature of the geometry. Use the lines in the pre-defined component shell_section to define the section. These lines are located at the mid-plane of the trapezoidal geometry. In addition to these lines, HyperBeam also requires the thickness of the feature as input to calculate the shell section properties.

Shell section lines

Use the various panels, such as the Distance panel, to find the thickness of this feature. The thickness of the feature is equal to 2 units. 1.

Create a shell section using the lines in the shell_section component. •

From the menu bar, click Properties > HyperBeam.

•

Go to the shell section subpanel.

•

Set the entity selector to lines.

•

Click lines >> by collector.

•

Select the collector, shell_section.

•

Click select.

•

Set cross section plane to fit to entities.

•

Set section based node to plane base. HyperMesh activates the base node selector.

Proprietary Information of Altair Engineering

p.442

Altair HyperMesh 2019 Tutorials

•

While left-clicking, move the mouse on top of one of the mid-plane lines as shown in the image above. Click anywhere on the highlighted line to define the base node.

•

Set part gen to auto.

•

Click create. The HyperBeam module opens.

Note:

p.443

The cross section plane option allows the software to define the plane for calculating beam cross-sectional properties based on the entity (lines/element) selection. A user-controlled plane can also be defined by changing the crosssection plane using the toggle. When using the fit to entities option, you can select a reference node for the plane if you want properties about a point other than the section centroid. This is done using the section base node option. This node defines the origin of the coordinate system that serves as the reference when computing the various beam cross-section properties. All the properties are calculated both about the centroid and about the node you select.

Shell section

The coordinates of the centroid are calculated with respect to the user-defined coordinate system appearing at the node location specified earlier. The coordinates of the shear center are calculated both from the centroid and from the origin of the section. Local Ys and Zs are the coordinates of the shear center with respect to the origin of the section, while principal Vs and Ws are the coordinates of the shear center from the centroid of the section.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

p.444

Modify the thickness of the cross-section and assign it a value of 2 units. •

In the Model browser, right-click on shell_section.1 and select Edit from the context menu. The Edit Shell Section dialog opens.

•

In the Part thickness field, enter 2. HyperMesh updates the values for the beam properties computed in the Results window.

•

Click Update.

•

Click Exit to close the dialog.

3.

Rename the section, “Trapezoidal Section.”

4.

Exit the HyperBeam module by clicking File > Exit from the menu bar. In this step, a beam cross-section representing a shell section was created using HyperBeam, and the thickness for the shell section was assigned. The shell section is defined with only one thickness as it is defined as one part. For shell sections comprised of multiple parts, each part is assigned an independent thickness. You may save your model to your working directory.

Step 5: Create a solid section using surfaces. In this step, model the irregular solid feature of the geometry as a solid section using the solid section subpanel of the HyperBeam panel. The input for a solid section can be 2D elements, surfaces, or a set of lines that form a closed area. Use the surfaces in the solid_section collector to define the solid section. 1.

Create a solid section using the surfaces in the solid_section component.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.445

•

In the HyperBeam panel, go to the solid section subpanel.

•

Set the entity selector to use surfs.

•

Select the highlighted surface in the following image.

•

Set section base node to base node.

•

Click base node.

•

While left-clicking, hover over a line or the surface until the surface highlights. Click anywhere on the highlighted entity to select a base node.

Defining the solid section

•

Set analysis type to first order. This option tells HyperBeam to use first order (linear) elements to calculate the properties of the section.

•

Click create. The HyperBeam module opens, meshes the area enclosed by the selected curves with quadrilateral elements, and calculates the properties using these elements.

Solid section

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

Rename the section "Solid Section" and save your data.

3.

Exit HyperBeam and save your data.

p.446

Step 6: Assign beam properties to a property collector and a beam element. In HyperMesh, you can assign the beam properties computed in HyperBeam and stored in a beamsect collector to your solver beam property card. To achieve this, create a property collector with the solver beam property card of interest, and assign the beamsect collector to the property collector. When creating an actual beam element, assign the property collector to the element itself. 1.

Create a property collector with a PBEAM card and assign the Solid Circle beamsect collector to it. •

Create a property collector by right-clicking in the Model browser and selecting Create > Property from the context menu. HyperMesh displays the property in the Entity Editor.

•

Name the property standard_section.

•

Set the Card Image to PBEAM.

•

Assign the Material as steel.

•

Assign the Beam Section as Solid Circle.

The properties calculated using HyperBeam are automatically assigned to the PBEAM card. Observe that the values of the parameters (A, I1a, I2a, I12a, J, etc.) are extracted from the properties of the selected section. 2.

Use the Bars panel to create a beam element with the standard_section property assigned, and a direction vector set to the global x-axis. •

From the menu bar, click Mesh > Create > 1D

•

Elements > Bars

•

Click property = and select standard_section.

•

Click the lower-left switch and select vectors as the option to define the orientation of the beam.

•

Set the orientation selector to x-axis.

•

Activate node A.

•

While left-clicking, hover over the line that runs though the cylinder until it is highlighted. Select two nodes at the ends of the line for node A and node B.

Creating a beam element

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.447

The beam element is created and placed into the beam component. Note:

When creating beam elements, the z-axis is defined by the two nodes selected as node A and node B. The direction of the cross-section (x- or y-axis) is defined either by using components, vectors, or a direction node. Due to the nature of this solid circle, how you define the x- or y-axis is unimportant.

Changes made to a beamsect collector (for example, through editing of a cross-section) are also automatically applied to any property collector referencing this beamsect collector.

Step 7 (Optional): Save your work. Summary In this tutorial, you experimented with the tools and techniques for modeling beam crosssection and obtaining their properties using HyperBeam. You learned how to edit crosssections and assign their properties to property collectors, which can then be assigned to 1D elements. For more details on how to create 1-D elements, review the tutorial, Creating 1-D Elements. Additional techniques for creating 1-D elements from connector entities are discussed in the tutorial, Creating Connectors.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

HM-4030: Defining Composites In this tutorial, you will learn how to assign element material orientation using the following: •

System ID

•

Vector

•

Angle

Model Files This exercise uses the composites.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Step 1: Load the OptiStruct user profile. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select OptiStruct.

3.

Click OK.

Step 2: Retrieve and view the file, composites.hm. 1.

Open a model file by clicking File > Open > Model from the menu bar, or clicking on the Standard toolbar.

2.

In the Open Model dialog, open the composites.hm file. A model appears in the graphics area.

Proprietary Information of Altair Engineering

p.448

Altair HyperMesh 2019 Tutorials

Step 3: Update all of the elements to the correct element types for OptiStruct. 1.

Open the Element Type panel by clicking Mesh > Assign > Element Type from the menu bar.

2.

Click elems >> all. HyperMesh selects all of the element types (1D, 2D, and 3D).

3.

Click update.

4.

Return to the main menu by clicking return.

Step 4: Assign element material coordinate direction using system ID. 1.

Open the Composites panel by clicking composites from the 2D page.

2.

Go to the material orientation subpanel.

3.

Set the entity selector to elems.

4.

Click elems >> all.

5.

Set the Material orientation method to by system ID.

6.

Activate the system selector.

7.

Select the rectangular system on top of ball as indicated in the following image. Note:

The system ID = 1.

8.

Click color and select a display color for the review vectors or lines.

9.

In the size = field, enter 2.0. Note:

This value specifies, in model units, how large the review vectors are when displayed.

Proprietary Information of Altair Engineering

p.449

Altair HyperMesh 2019 Tutorials

p.450

10. Click assign.

11. Open the Card Edit panel by clicking

on the Collectors toolbar.

12. Set the entity selector to elems. 13. Select any element in the model. 14. Click edit. 15. In the Card Previewer dialog, review the card. Note:

This function assigns the ID of the coordinate system to the selected elements. This can be verified by reviewing the MCID field of the CQUAD4 card populated with System ID 1 for the currently loaded OptiStruct user profile. How each analysis code interprets this information varies. For OptiStruct, refer to the CQUAD4 and PCOMP(G) bulk data cards in the Bulk Data Section of the OptiStruct Reference Manual. For visualization purposes HyperMesh also projects the x-axis of the selected coordinate system onto the face of the shell elements to define the x-axis of the material coordinate system. If you later modify the system, the element material coordinate directions change implicitly.

16. Exit the Card Previewer by clicking return. 17. Exit the Card Edit panel and return to the Composites panel by clicking return.

Step 5: Assign element material coordinate direction using a system axis. In this step you should be in the Composites panel, material orientation subpanel. 1.

Set the entity selector to elems.

2.

Click elems >> all.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

Set the Material orientation method to by system axis.

4.

Activate the system selector.

5.

Select the rectangular system on top of ball as indicated in the following image. Note:

The system ID = 1.

6.

Under the system selector, set the switch to local 2-axis.

7.

In the size= field, enter 2.0. Note:

p.451

This value specifies, in model units, how large the review vectors are when displayed.

8.

Click color and select a display color for the review vectors or lines.

9.

Click project.

10. Open the Card Edit panel. 11. Set the entity selector to elems. 12. Select any element in the model. 13. Click edit. 14. In the Card Previewer dialog, review the card. Note:

This function assigns a material angle to the selected elements, which for OptiStruct is defined as the angle between the vector direction connecting node1 and node2 of the shell element (that is, the element coordinate system x-axis) and the projection of the selected local axis onto the surface of the shell element. This can be verified by reviewing the THETA field of the CQUAD4 card populated with an angle (in degrees) for the currently loaded OptiStruct user profile. Each element in this case will have a unique THETA value as defined by the projection. How each analysis code interprets this information varies. For OptiStruct, refer to the CQUAD4 and PCOMP(G) bulk data cards in the Bulk Data Section of the OptiStruct Reference Manual. For visualization purposes HyperMesh also projects the local axis of the selected coordinate system onto the face of the shell elements to define the x-axis of the material coordinate system.

15. Exit the Card Previewer. 16. Exit the Card Edit panel and return to the Composites panel.

Step 6: Assign element material coordinate direction using a vector. In this step you should be in the Composites panel, material orientation subpanel. 1.

Set the entity selector to elems.

2.

Click elems >> all.

3.

Set the Material orientation method to by vector.

4.

Set the orientation selector to vector.

5.

Activate the vector selector.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

p.452

Select the radial r vector from the spherical coordinate system on the bottom of the ball. Note:

The r-axis will flash once when you click on it.

7.

Click B.

8.

Select the origin of the local spherical system as the base.

9.

In the size = field, enter 2.0. Note:

This value specifies, in model units, how large the review vectors are when displayed.

10. Click color and select a display color for the review vectors or lines. 11. Click project. 12. Open the Card Edit panel. 13. Set the entity selector to elems. 14. Select any element in the model. 15. Click edit. 16. In the Card Previewer dialog, review the card. Note:

This function assigns a material angle to the selected elements, which for OptiStruct is defined as the angle between the vector direction connecting node1 and node2 of the shell element (that is, the element coordinate system x-axis) and the projection of the selected vector onto the surface of the shell element. This can be verified by reviewing the THETA field of the CQUAD4 card populated with an angle (in degrees) for the currently loaded OptiStruct user profile. Each element in this case will have a unique THETA value as defined by the projection. How each analysis code interprets this information varies. For OptiStruct, refer to the CQUAD4 and PCOMP(G) bulk data cards in the Bulk Data Section of the OptiStruct Reference Manual. For visualization purposes HyperMesh also projects the selected vector onto the face of the shell elements to define the x-axis of the material coordinate system.

17. Exit the Card Previewer. 18. Exit the Card Edit panel and return to the Composites panel.

Step 7: Assign element material coordinate direction using an angle. In this step you should be in the Composites panel, material orientation subpanel. 1.

Set the entity selector to elems.

2.

Click elems >> all.

3.

Set the Material orientation method to by angle.

4.

In the angle = field, enter 45.00.

5.

In the size = field, enter 2.0. Note:

This value specifies, in model units, how large the review vectors are when displayed.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

Click color and select a display color for the review vectors or lines.

7.

Click set.

8.

Open the Card Edit panel.

9.

Set the entity selector to elems.

10. Select any element in the model. 11. Click edit. 12. In the Card Previewer dialog, review the card. Note:

This function assigns a material angle of 45 degrees to the selected elements, which for OptiStruct is defined as the angle 45 degrees from the vector direction connecting node1 and node2 of the shell element (that is, the element coordinate system x-axis) using right hand rule. In order to use right hand rule, the normal direction of the element must be known and can be determined from the Tools page, Normals panel. This can be verified by reviewing the THETA field of the CQUAD4 card populated with a 45-degree angle for the currently loaded OptiStruct user profile. Each element in this case will have a THETA of 45 degrees. How each analysis code interprets this information varies. For OptiStruct, refer to the CQUAD4 and PCOMP(G) bulk data cards in the Bulk Data Section of the OptiStruct Reference Manual. For visualization purposes HyperMesh defines a vector using OptiStruct convention on the face of the shell elements to define the x-axis of the material coordinate system. This option should be used only in situations where great care has been taken to assure that the node1-node2 direction of the shell elements are initially aligned properly.

13. Exit the Card Previewer. 14. Exit the Card Edit panel and return to the Composites panel.

Step 8: Review ply directions. In this step you should be in the Composites panel. 1.

Go to ply directions subpanel.

2.

Use the switch to select zone based model.

3.

Set the entity selector to elems.

4.

Click elems >> by collector.

5.

Select the collector, yellow_sample. Note:

The yellow_sample collector has a PCOMP card image assigned to it with the following laminate definitions (45/60/90). The PCOMP definition assigned to the yellow_sample collector can be reviewed in the card editor.

6.

Click select.

7.

In the ply = field, enter 1. Note:

This defines the ply number to review.

8.

Open the Card Edit panel.

9.

Set the entity selector to props.

Proprietary Information of Altair Engineering

p.453

Altair HyperMesh 2019 Tutorials

10. Click props. 11. Select yellow_sample. 12. Click select. 13. Click edit. 14. In the Card Previewer dialog, review the card. Note:

The first ply defined on the PCOMP card is the most negative z-axis ply as determined from the element normal. All ply angles on the PCOMP card are relative to the material coordinate direction set in the above exercises using right hand rule. In order to use right hand rule, the normal direction of the element must also be known and can be determined from the Tools page, Normals panel. For OptiStruct, refer to the PCOMP(G) bulk data cards in the Bulk Data Section of the OptiStruct Reference Manual.

15. Exit the Card Previewer. 16. Exit the Card Edit panel and return to the Composites panel. 17. In the size = field, enter 2.0. Note:

This value specifies, in model units, how large the review vectors are when displayed.

18. Click color and select a display color for the review vectors or lines. 19. Click review. 20. Review additional ply angles, reselect elements, and enter a ply ID by clicking review. Note:

Elements that do not have ply angles assigned will not be displayed. Ply directions are set through card images in the solver template; an example is PCOMP card for OptiStruct.

Proprietary Information of Altair Engineering

p.454

Altair HyperMesh 2019 Tutorials

HM-4040: Working with Loads on Geometry In this tutorial, you will learn how to: •

Create loads and boundary conditions on geometry

•

Map the loads from geometry to elements

•

Export to a solver deck

•

Modify the mesh and remap the loads to the new mesh

Model Files This exercise uses the c-channel0.hm file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

C-channel model in shaded mode

Exercise: Working with Loads on Geometry Step 1: Retrieve the model file, c-channel0.hm. In this tutorial, you will experiment with the export of the loads applied to geometry entities. Therefore, you will need to have a template loaded. In this step, load the OptiStruct user profile and retrieve the c-channel model. By loading the OptiStruct user profile, the template will be automatically loaded. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select OptiStruct.

3.

Click OK.

4.

Open a model file by clicking File > Open > Model from the menu bar, or clicking on the Standard toolbar.

Proprietary Information of Altair Engineering

p.455

Altair HyperMesh 2019 Tutorials

5.

p.456

In the Open Model dialog, open the c-channel0.hm file. A model appears in the graphics area. Note:

The model's geometry is of a C-channel with two reinforcement ribs. The various surfaces are organized into several component collectors.

Step 2: Create three load collectors for constraints, forces, and pressure loads. In this step, create load collectors to organize constraints, forces, and pressure loads in. 1.

In the Model browser, right-click and select Create > Load Collector from the context menu. HyperMesh creates and opens a load collector in the Entity Editor.

2.

In the Entity Editor:

3.

•

For Name, enter constraints.

•

Click the Color icon, and select a new color for the load collector.

•

Set Card Image to .

Repeat steps 2.1 and 2.2 to create two more load collectors named pressure and forces. Note:

Different boundary conditions can now be created.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Defining loads and boundary conditions on geometry. In the following steps you will apply constraints, pressures, and forces to geometric entities in the model. You will first constrain the bottom portion of the c-channel using line data, then you will create pressure loads on the top surfaces. Lastly, you will apply forces to the eight corners of the surfaces defining the top of the c-channel.

Constraints on lines, pressures on surfaces, and forces on fixed points

Step 3: Fully constrain the bottom eight lines of the c-channel using the Constraints panel. 1.

In the Model browser, Load Collector folder, right-click on constraints and select Make Current from the context menu.

2.

Open the Constraints panel by clicking BCs > Create > Constraints from the menu bar.

3.

Go to the create subpanel.

4.

Set the entity selector to lines.

5.

Select the eight lines defining the bottom portion of the c-channel as indicated in the following image.

Lines to constrain

Proprietary Information of Altair Engineering

p.457

Altair HyperMesh 2019 Tutorials

6.

In the size= field, enter 1. Note:

This is the size of the icons that will be used to represent the constraints in the graphics area.

7.

Clear the label constraints checkbox.

8.

Select the dof1, dof2, dof3, dof4, dof5, and dof6 checkboxes. Note:

9.

The selected Dofs will be constrained. Dofs 1, 2, and 3 are x, y, and z translation degrees of freedom. Dofs 4, 5, and 6 are x, y, and z rotational degrees of freedom.

Click load types = and select SPC.

10. Click create. HyperMesh applies constraints to the selected lines. Constraints are represented by triangular icons in the graphics area.

11. Optional: Display the degrees of freedom labels by selecting the label constraints checkbox.

Proprietary Information of Altair Engineering

p.458

Altair HyperMesh 2019 Tutorials

12. Exit the panel by clicking return.

Step 4: Apply a pressure of 25 units normal to the top three surfaces using the Pressures panel. 1.

In the Model browser, Load Collector folder, right-click on pressure and select Make Current from the context menu.

2.

Open the Pressures panel by clicking BCs > Create > Pressures from the menu bar.

3.

Go to the create subpanel.

4.

Set the first switch to entities.

5.

Set the entity selector to surfs.

6.

Select the three surfaces defining the top of the c-channel as indicated in the following image.

Surfaces to apply pressure to

7.

In the magnitude = field, enter –25 for the pressure. Note:

Specifying a negative magnitude ensures that the pressure load pushes down on the surfaces. By default, pressure load are created normal to the surfaces.

Proprietary Information of Altair Engineering

p.459

Altair HyperMesh 2019 Tutorials

8.

Toggle the display of the pressures from magnitude % = to uniform size =. Note:

9.

p.460

Pressure loads are represented by arrows in the graphics area. You can input the size of the arrow as a value or as a percentage of the actual pressure load applied. In this exercise, you will specify its length as a certain number.

In the uniform size = field, enter 1. Note:

This is the display size of the pressure arrows in the graphics area.

10. Clear the label loads checkbox. Note:

In this exercise, you will not display the actual value of the pressure load in the graphics area.

11. Click load types = and select PLOAD. 12. Click create. HyperMesh applies pressure loads to the selected surfaces. Pressure loads are represented with an arrow and a label in the graphics area. Note:

Labels can be template based (PLOAD here) or follow the HyperMesh terminology (P) as specified in the modeling subpanel of the Options panel.

13. Exit the panel by clicking return.

Step 5: Create forces at the eight corners of the three top surfaces. 1.

In the Model browser, Load Collector folder, right-click on forces and select Make Current from the context menu.

2.

Open the Forces panel by clicking BCs > Create > Forces from the menu bar.

3.

Go to the create subpanel.

4.

Set the entity selector to points.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

5.

Select the eight fixed points defining the corners of the c-channel’s top surfaces as indicated in the following image.

Fixed points to apply forces to

6.

Set the coordinate system toggle to global system.

7.

Toggle the vector definition from magnitude % = to uniform size =.

8.

In the uniform size = field, enter 1.

9.

Clear the label loads checkbox.

10. In the magnitude = field, enter –15. Note:

The minus sign is used to specify a direction opposite to the one you will select in the next step.

11. Under magnitude =, set the orientation selector to z-axis. 12. Click load types = and select FORCE. 13. Click create. HyperMesh creates a point force for each fixed point you selected, with the given magnitude in the z-direction.

Loads on geometry

Proprietary Information of Altair Engineering

p.461

Altair HyperMesh 2019 Tutorials

p.462

14. Exit the panel by clicking return. Tip:

If you organized some loads in the wrong load collector, use the Organize panel to move the loads into the right collector.

In the previous steps you created various types of loads on various geometric entities: lines, surfaces, and fixed points. The ultimate goal is to apply these loading conditions to finite elements. In the following steps you will create the elements to apply the loading conditions to.

Step 6: Generate elements on the surfaces. In this step, use the Automesh panel to create a quad dominant (mixed) mesh. The elements generated will be organized into their surface's component collector, which will avoid the need to set current component collectors. 1.

Open the Automesh panel by pressing F12.

2.

Set the entity selector to surfs.

3.

Click surfs >> displayed.

4.

In the element size = field, enter 0.25.

5.

Set the mesh type to mixed.

6.

Toggle from elems to current comp to elems to surf comp. Note:

7.

Set the meshing mode to automatic. Note:

8.

This option ensures that the elements created will be organized into the surface’s component collector. In this mode, HyperMesh automatically generates a mesh on the surfaces based on the element size and the type of elements selected. No further user input is required or can be supplied.

Click mesh. HyperMesh creates a shell mesh on the surfaces.

Meshed c-channel

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

9.

p.463

Exit the panel by clicking return.

In this step, you created a shell mesh on the surfaces. In the following step you will map the loads that were applied to geometric entities to these finite elements.

Step 7: Map the loads from geometry to elements. A load collector, just like component collectors, can store both loads on geometry and loads on finite elements. These two types of loads are separate and independent, and can therefore be manipulated independently. At this time, your load collectors contain loads only in their geom side. By mapping these loads on geometry to finite elements and using your existing loadcols, you will also populate their elems side. In this step, use the Load on Geom panel to map the loads from the geometric entities (to which the geometric loads are applied) to the mesh associated with these geometric entities for the constraints and pressure load collectors. 1.

Open the Loads on Geometry panel by clicking BCs > Loads on Geometry from the menu bar.

2.

Click loadcols.

3.

Select the load collector, constraints.

4.

Click select.

5.

Click map loads. HyperMesh maps the constraints previously applied to the lines to the nodes of the mesh associated to these lines. Note:

These constraints are placed in the same load collector as the ones applied to the geometry, only in the elems portion.

Constraints mapped to the elements

6.

Repeat steps 7.1 through 7.5 to map the pressure loadcol to the mesh. HyperMesh maps the pressure loads previously applied to the surfaces to the nodes of the mesh associated to these surfaces Note:

These pressure loads are placed in the same load collector as the ones applied to the geometry.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.464

Step 8: Export the model to a solver deck. When you export a model using an export template, only the loads on the mesh are exported. The loads on the mesh may have been applied directly to the mesh, mapped from geometry to the mesh, or both. You can use the Export tab to export loads to an ASCII solver-specific file (according to the loaded export template). The loads are exported as mesh loads. Use the Custom template to determine which loads are exported. If all is selected, then all of the loads on the geometry that have not been mapped (if any) are mapped to the loads on the mesh, and all of the loads on the mesh are exported. If displayed is selected, then all of the displayed loads on the mesh (if any) are exported. All of the loads on the mesh associated with the displayed loads on the geometry (if any) are exported as well. If any of the loads on geometry are displayed and have not been mapped, they will automatically be mapped to the loads on the mesh and exported as well. In this step, use the Model browser to ensure that only the already mapped loading conditions are exported. One load collector stores both the loads on the geometry and the loads on the mesh. The mesh (or multiple meshes) is associated with the geometric entities to which the loads on the geometry have been applied. Each load type is stored in a dedicated section of the same load collector. Use the Display panel to separate or simultaneously visualize the loads on the mesh and the loads on the geometry. Turn off the display of the loads applied to the geometric entities to only display the loads applied to the mesh. 1.

In the Model browser, Load Collector folder, click off the display of their geometry.

next to all of the loads to turn

Load collector's geometry display turned off

2.

From the menu bar, click File > Export > Solver Deck.

3.

In the File field, click

4.

In the Select OptiStruct file dialog, navigate to your working directory and save the file.

5.

View advanced export options by clicking

6.

From the Export drop-down list, select Displayed.

7.

Click Export. HyperMesh exports the model as an OptiStruct .fem input file.

.

Proprietary Information of Altair Engineering

next to Export options.

Altair HyperMesh 2019 Tutorials

Note:

p.465

Because you turned off the geometry display of the load collectors in your model, HyperMesh only exports the loads mapped previously. You may open the exported deck in any text editor to verify that no OptiStruct FORCE card has been exported in the deck.

In this section you experimented with exporting loads applied to geometric entities and elements in the Export tab. You learned that with different combinations of the all/displayed options and loads displayed in the Model browser, you can control what information gets exported.

Step 9: Modify the mesh and remap the loads to the new mesh. When loads are applied to geometry, you can re-applying them to different meshes as many times as you want. This functionality is particularly useful when you want to remesh a model without having to delete complicated loads or boundary conditions. After remeshing, you can easily remap loads or boundary conditions that have been applied to geometric entities to the new mesh, while loads applied to elements are automatically deleted when the elements themselves are deleted. Note: If you delete geometric entities to which loads are applied to, the loads will be deleted. The deletion of geometric entities will not affect any loads applied to the mesh. In this step, you will remesh the surfaces. 1.

Go to the Automesh panel.

2.

Click surfs >> displayed.

3.

In the element size = field, enter 0.5.

4.

Leave all other options used earlier unchanged.

5.

Click mesh. The automesher deletes the existing elements, and creates a completely new set based on the new element size. Note:

6.

HyperMesh removes the loads that were applied to the initial mesh since the elements are no longer there.

Click return.

New mesh

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 10: Map all the loads on geometry to the new mesh using the Load on Geom panel. In this step you will remap the loads applied to the geometry to the new mesh. 1.

Open the Loads on Geometry panel by clicking BCs > Loads on Geometry from the menu bar.

2.

Click loadcols.

3.

Select the following load collectors: constraints, pressure, and forces.

4.

Click select.

5.

Click map loads. HyperMesh applies the loading conditions initially defined for the geometric entities to the new mesh, and places the various loading conditions into the same load collector as the corresponding ones applied to the geometry. Note:

You did not have to display these loads to map them.

In this step, you experimented with the remapping of loads applied to geometric entities to a new mesh. Loads applied to geometric entities can be mapped several times to the different finite element entities attached to these geometric entities. For example, this functionality is useful in a situation where a mesh had to be changed, and it saved you from having to recreate loads on the elements.

Step 11 (Optional): Save your work. With all of the exercises complete, you can save the model if desired.

Summary In this tutorial, you used several boundary condition creation panels to generate constraints and various loading conditions on geometric entities. You then experimented with the mapping of these loads on the geometry to finite elements. You also familiarized yourself with the rules that govern the export of loads on geometric entities. No consideration to the creation of specific card images that need to accompany the various loading conditions was given. For more information on how to generate the various loading conditions for different solvers, refer to the Modeling / Solver Specific section of the HyperMesh tutorials.

Proprietary Information of Altair Engineering

p.466

Altair HyperMesh 2019 Tutorials

HM-4060: Working with Include Files In this tutorial, you will learn how to: •

Import include files

•

Review and manipulate includes

•

Create includes and reorganize the database

•

Locate entities in includes

•

Import new data into includes

•

Export options

While HyperMesh supports include formulations for several other solvers, you will use LSDYNA 970 input decks for the purpose of this tutorial. Many FEA solvers allow you to organize your input deck into separate files, and provide a mechanism to read all files linked to a single input deck. This capability is commonly known as "includes." HyperMesh provides several options for importing such models, one of which preserves the include structure upon import. The Include view in the Model browser is available to manipulate these includes. The Include view lets you create, review, edit, organize, and update the contents of any HyperMesh model into various include files. Every entity in HyperMesh then belongs to either the master model or one of its include files.

Model Files This exercise uses the master.k file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Step 1: Load the LS-DYNA user profile and import the model. In this step you will load the LS-DYNA user profile, import the LS-DYNA decks (master file and include files) defining the model, and preserve the organization of the data into the various include files. 1.

Start HyperMesh Desktop.

2.

In the User Profile dialog, select LsDyna, Keyword970. Note:

3.

Selecting a solver user profile sets the FE input reader to this solver and loads the solver’s FE output template. It also loads a macro menu with numerous tools specific to this interface. The graphical user interface is also tailored to this solver with panel names and options renamed or removed to match its terminology as much as possible.

Click OK.

Proprietary Information of Altair Engineering

p.467

Altair HyperMesh 2019 Tutorials

4.

p.468

From the menu bar, click File > Import > Solver Deck. Note:

The Import - Solver Deck tab contains the following advanced options for importing include files:

•

Merge: merges all of the data in the individual includes into a master model, and then imports the master model into HyperMesh as a single model. HyperMesh has no knowledge regarding individual include files with this option.

•

Skip: reads INCLUDE statements as control cards and ignores the data within the include files. None of the contents of the include files are processed.

•

Preserve: preserves the INCLUDE statements, and processes the contents of the include files. The contents of the include files are "marked" to remember which include file they belong to. When the deck is exported from HyperMesh, if desired, all of the entities that are marked as belonging to include files get written back to that include file. The entire file structure (the master file and all of its include files) are rewritten from the HyperMesh database.

5.

In the File field, open the master.k file.

6.

Next to Import options, click

7.

From the Include files drop-down list, select Preserve.

8.

Click Import. HyperMesh imports the master.k deck, and the wheels.key, frame.key and engine.key include files, which are also present in the same directory. The truck model defined with a master deck and several include files were imported into HyperMesh while preserving the organization of the data between the various files.

.

Truck model

Step 2: Review the model organization using the Include view in the Model browser. You can access the Include view ( ) in the Model browser. In this view you can create, review, edit, organize, and update the contents of a model into various include files. From the right-click context menu you can access additional Include view functions. For a complete description of the options available, refer to Model Browser's include view.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.469

In this section, you will launch the Include view, review the structure of the model and its organization into the various includes, and experiment with some of the display and configuration options available. 1.

In the Model browser, click database structure. Note:

. HyperMesh displays a tree-like organization of the

The Master Model is at the top level of the include browser. Data, which does not have any references to an include file, is stored in the master model. Each include file is represented by along with its file name. Each include can be expanded to reveal its contents. The contents of each include is grouped into folders containing each type, next to which appears the total number of entities of that type. Each of the folders can be expanded to review the individual entities in that folder. The browser can be configured to show only specific entities of interest.

2.

Expand the include, engine.key.

3.

Review its content, which consists of components, materials, and properties.

4.

Expand the Component folder, which consists of six component collectors.

Components content of the engine.key include

5.

Review the contents of the other includes as well as the contents of the folders belonging to the Master Model. The wheels.key include contains, for example, components, control volumes, groups, materials, properties, and sets. Note:

While most entities are presented in this tree, elements and nodes are not listed, as this would not be practical for larger models.

6.

In the Model browser, right-click and select Collapse All from the context menu. All of the folders collapse.

7.

Right-click on Master Model and experiment with the Show and Hide display options in the context menu.

8.

Visually review the components that each include contains by isolating the include you wish to review using the Isolate only option in the context menu.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Displaying only the frame.key include

9.

Turn on the display of the entire model.

In this section, you launched the Include view and reviewed the structure of the model and its organization into the various includes. You also customized the Include view and used some of the display options to modify the display of the model in the graphics area.

Step 3: Review the various options available in the Include view. You can configure the columns within the Include View so that only the columns you are interested in are displayed. In this step you will learn how to configure the Include View in the Model browser. 1.

In the Model browser, right-click and select Collapse All from the context menu. Note:

2.

There are columns for Export, Include Path, and Include Type.

Expand the frame.key folder. Note:

The Export, Include Path and Include Type columns are only relevant for the include files and not for the individual entities within the file.

Proprietary Information of Altair Engineering

p.470

Altair HyperMesh 2019 Tutorials

3.

In the Model browser, right-click and select Configure Browser from the context menu.

4.

In the Browser Configuration dialog, select the Columns tab. Note:

p.471

From the Columns tab you can can define which columns are displayed in the Model browser when you are in the Include View.

5.

Clear the Include Type checkbox.

6.

Click OK. The Include Type column is no longer visible in the browser.

Step 4: Create new includes, reorganize the model, and locate entities in includes. Whether you import includes or are simply starting from a ‘flat’ HyperMesh model, you can create new includes in your database using the Include View, and organize entities into them using the Organize panel. You can also select entities (using the standard SHIFT and CTRL keys) from the Include view and drag them between two includes or between the master model and an include. To determine which include a specific entity belongs to, you can use the Organize panel’s locate function. In this section, create a new include for the doors and organize the corresponding collectors into it using the Organize panel. Finally, determine which include a certain material belongs to using the locate function. 1.

In the Model browser, Include View, right-click on Master Model and select Create > Include File from the context menu. HyperMesh adds a new include under the master model with an editable name, and displays it in bold, which signifies that it is the current include. Note:

You can add includes under the master model or under includes themselves.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

In the editable field, enter the name doors.key for the new include. Note:

You can rename or make current a new include using the right-click context menu.

3.

Open the Organize panel by clicking organize from the Tool page.

4.

Go to the includes subpanel.

5.

Set the entity selector to comps.

6.

Click dest = and select doors.key as the destination for the components.

7.

Click comps.

8.

Select the components: SHELL: DOOR-LEFT, SHELL: DOOR-RIGHT, and SHELL: DOOR-WINDOWG-LEFT.

9.

Click select.

10. Click move. HyperMesh moves the selected components into the doors.key include. Note:

An expand/collapse icon is added next to the doors.key include, which indicates that data has been placed under it.

11. Expand the doors.key include, Component folder to review the components that you moved. 12. Hide all of the includes except doors.key. HyperMesh displays the elements organized in this include in the graphics area.

Door and window elements in doors.key.

Proprietary Information of Altair Engineering

p.472

Altair HyperMesh 2019 Tutorials

p.473

13. Change the display back to Display All. 14. In the Organize panel, includes subpanel, set the entity selector to mats. 15. Click locate. HyperMesh displays a list of all the materials available in this model. 16. Select the material, MATL1_38. HyperMesh updates the dest= field to show which include (or master) file this particular material belongs to. In this case, it belongs to the wheels.key include.

17. Exit the panel by clicking return. In this section, you created a new include in the Include view, and moved some components from the master model, as well as their corresponding elements, into it. Finally, you used the locate function to quickly identify which include a material belonged to.

Step 5: Import new data into an include and export the model. By default, the Master Model is always the current file (displayed in bold in the Include view) and any new entities you create or import into HyperMesh will be automatically placed in it. You can use the Make Current option from the Include view context menu to make any include the current include. When you create a new include, this include will automatically become the current include. You can use the Include File Options function in the Include view context menu to define export options for individual include files. Using this option, you can define whether the include file should get exported, when the export function is used, and where the file should be exported. The Export - Solver Deck tab contains the following advanced options for exporting models that contain include files: •

Merge: merges all of the data in individual include files into a single master model during export. The exported file does not contain references to any include files.

•

Preserve: exports all the data in individual include files separately to their corresponding files. The references to these includes in the master model file are also maintained.

In this section, you will create a new include in the master model labeled barrier.dyn, and then import a barrier model into it. You will then review the include file options for each one of the includes in the model and modify them as needed. Lastly, you will export the model, while also preserving the includes. 1.

In the Include view, right-click on Master Model and select Create > Include File from the context menu.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

p.474

In the editable field, enter the name barrier.dyn for the new include. Note: The new include is displayed in bold, which indicates that it is now the current include and any new data created or imported into HyperMesh will be placed in it.

3.

From the menu bar, click File > Import > Solver Deck. The Import tab opens.

4.

In the File field, open the barrier.dyn file.

5.

Click Import. Hypermesh imports the barrier.

Truck and barrier

6.

In the Include view, expand Barrier.dyn and review its contents. Note:

7.

barrier.dyn is displayed in bold, and both barrier.dyn and doors.key are non-italicized, while engine.key, frame.key, and wheels.key are all italicized. This is a visual representation of the export option that is set for each of these three includes.

Right-click on engine.key and select Include File Options from the context menu. The Include File Options dialog opens, and displays the following: •

File path- type in or browse for the directory in which the include is to be exported.

•

Do not export - When this check box is selected, HyperMesh will not export include when you export the model. When this check box is clear, HyperMesh exports the include when you export the model. This check box is automatically selected when you read includes into HyperMesh that have their permission set to read only, as well as includes that are referenced by the master include using absolute paths. The frame.key, wheels.key and engine.key includes are all referenced by the master.k include, that you imported initially using relative paths (edit the master.k file to verify this), but their permissions were set to read only. In order to export these includes, clear the Do not export check box.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

8.

For the engine.key, frame.key and wheels.key includes, clear the Do not export check box and then click Set.

9.

Right-click on an include and select Export All Includes from the context menu. The Export all includes dialog opens.

10. In the File name field, enter the location and name of the master model and click OK. HyperMesh exports all of the include files as individual files. Note:

This option is equivalent to exporting the master model from the Export Solver Deck tab ( ) with the preserve includes check box selected. When you want to export a single file, use the export subpanel and set export option to merge includes.

11. Go to the directory you selected in the previous step and verify that all of the includes have been exported with the names set in the Include view.

Step 6 (Optional): Save your work The tutorial is complete. Save your work as a HyperMesh file. In this tutorial you used the include browser to manage the use of includes in your truck model. Several options for import, display, organization, and export were used.

Proprietary Information of Altair Engineering

p.475

Altair HyperMesh 2019 Tutorials

p.476

HM-4070: OptiView In this tutorial, you will: •

Import an optimization model

•

Create a new set of optimization entities

•

Organize these into optimization problems

•

Run both problems

•

View results

Model Files This exercise uses the cclip.fem file, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise

Step 1: Launch HyperMesh and set the user profile to OptiStruct. Step 2: Import the cclip.fem file. from the Standard toolbar.

1.

Select Import Solver Deck

2.

Select OptiStruct for the File type.

3.

Browse to \tutorial\hm\ and select cclip.fem.

4.

Click Import to open the file.

Step 3: Create Problem 1 and organize optimization entities. 1.

In the Model browser, click

(Optimization View).

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

Review the Optimization Repository. The Optimization Repository gives an overview of all optimization related entities in the database. Info types and children entities help give a clear snapshot without having to review individual entities.

Figure 1

3.

Right-click the Optimization Problems folder and click Create > Optimization Problem. HyperMesh creates an optimization problem and opens it in the Entity Editor.

4.

In the Entity Editor, name this problem Topology.

5.

Drag and drop all the entities from the repository into the newly created problem. Note:

You can drag and drop entities from the repository into problems or problems into problems. Any combination of selected entities can be dragged and dropped.

Step 4: Define a new set of optimization entities. 1.

In the Model browser, right-click and select Create > Free Size Desvar from the context menu. The Free Size Optimization panel opens, from which you can define a free size design variable. Tip: Give the free size design variable a meaningful name so you can easily drag and drop.

2.

Use the props selector to select the shells property.

3.

You can create new response/constraint pairs, or anything else you want to change from problem to problem. For this tutorial, we will just compare Topology to Free Size.

Step 5: Create Problem 2 and organize optimization entities. 1.

In the Model browser, right-click and select Create > Optimization Problem from the context menu.

2.

In the Entity Editor, name this problem Free Size.

3.

Drag and drop all the entities defined in the repository to the newly created problem. Note: Two design variables will be defined for the Free Size problem.

Proprietary Information of Altair Engineering

p.477

Altair HyperMesh 2019 Tutorials

4.

p.478

In the Free Size folder, right-click on the shell design variable and select Remove from Problem from the context menu. Note:

This will not delete the problem from the repository.

Step 6: Set problems to export and run. 1.

In the Model browser, right-click on the Topology problem and select Set Export from the context menu. Note:

Once problems are defined, only one can be exported at a time. The problem set to export is in bold, and furthermore, the Entity State browser shows these rules.

2.

Open the OptiStruct panel.

3.

Set the export options to custom.

4.

Save the input file as cclip_topology.fem.

5.

Click OptiStruct to run the analysis. Note:

The Optimization View allows one .hm for all optimization problems, and it is up to the user to wisely name each input file.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Customization

Proprietary Information of Altair Engineering

p.479

8

Altair HyperMesh 2019 Tutorials

p.480

HM-8010: Add a Button to the User Page on the Utility Menu In this tutorial you will create a new button on the User page of the Utility menu.

Tools The User page is available on the Utility menu. To access the User page: 1.

From the menu bar, click View > Browsers > HyperMesh > Utility.

2.

At the bottom of the Utility menu, click the User button

Command files and Tcl/Tk scripts can be added to the userpage.mac file. When HyperMesh starts, it first looks for the userpage.mac file in the directory from which it launches, and then in the installation directory. UNIX users also have the option of putting the userpage.mac file in their home directory. The userpage.mac file controls the display and available operations on the User page of the HyperMesh Utility menu. In order to invoke a command file or Tcl/Tk script from the User page, a button must be defined inside the userpage.mac file. The *createbutton command is used to define the button and its characteristics. The syntax for this command is: *createbutton(page, name, row, column, width, COLOR, helpString, macroName [ , arg1 … ]) where: page

The page number on which the button is to appear. For the User page, this value is 5.

name

The text to display on the button, enclosed in quotes: " ".

row

The row in which to place the button. The number of visible rows depends on your monitor’s graphics resolution. A positive value indicates an absolute row number. A 0 indicates the next highest available row. A negative value indicates the number of rows to skip. Rows begin at the bottom of the menu.

column

The column where the button starts (0-10). Columns begin to the right of the menu.

width

The width of the button (max = 10).

COLOR

The color of the button. The available button colors are: RED, BLUE, GREEN, CYAN, MAGENTA, YELLOW, GRAY, and BUTTON (background). The color name must appear in capital letters.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

helpString

The string to be displayed in the menu bar when the middle mouse button is pressed and the button is clicked, enclosed in quotes: " ".

macroName

The command to run when the button is pressed, enclosed in quotes: " ".

arg1…

A list of optional arguments passed to the script.

p.481

Exercise In this exercise, you will create a button on the User page that will launch the lighting.tcl dialog from the HyperMesh installation.

Step 1: Create the userpage.mac file. Using a text editor, create a blank userpage.mac file in the appropriate directory. When HyperMesh starts, it first looks for the userpage.mac file in the directory from which it launches and then in the installation directory. On Windows, the default launch directory is in the My Documents folder. UNIX users also have the option of putting the userpage.mac file in their home directory. It is not recommended to modify the userpage.mac file in the installation directory.

Step 2: Add the command to create the button. 1.

Add the following text to the userpage.mac file:

*createbutton(5,"Lighting",10,5,5,YELLOW,"Launch the lighting.tcl script","EvalTcl","lighting.tcl") The EvalTcl macro is defined in the globalpage.mac file in the HyperMesh installation. It takes a Tcl script as its argument and executes the script. Notice that the full path is not used to reference the lighting.tcl script. A full path can be specified if the file is not located in one of the predefined paths that HyperMesh searches to find scripts. Users can add additional search paths using the TCL_INCLUDE environment variable. Relative paths can also be used from these search paths. 2.

Save the modified userpage.mac file.

Step 3: Load the updated userpage.mac file. 1.

Restart HyperMesh from the working directory or reload the current macro menu .mac file. This allows the current session to use the modified userpage.mac file. To reload the current macro menu .mac file while HyperMesh is open, from the menu bar select Preferences > Menu Config and click on retrieve next to macro file. Make sure to load the proper .mac file from the hm/scripts/ directory based on the current user profile, or load the default hm.mac in the hm/bin/ directory if no user profile is loaded.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

p.482

Click the User button on the Utility Menu. You will see Lighting, the button defined in Step 2. Compare this button to its definition. It is yellow in color, begins in column 5 of row 10, and extends half way across the Utility Menu.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

HM-8020: Create a Utility Menu Macro From a Command File In this tutorial you will: •

Determine the commands to save the current HyperMesh model

•

Create a Utility Menu macro to execute the command

•

Create a new button on the User page of the Utility Menu to run the macro

Tools In order to execute command file commands or Tcl scripts from a button on any of the HyperMesh Utility Menu pages, a Utility Menu macro must first be defined. A Utility Menu macro contains valid command file or templex commands that execute the appropriate operations, and is defined using the *beginmacro and *endmacro commands. Macros may accept data passed to them using the arguments $1, $2, etc. Each argument specifies where the values should be substituted. These macros are defined within the .mac files, including the userpage.mac file. The following skeleton code shows the format of a Utility Menu macro: *beginmacro(macroname) command statements go here *endmacro() Utility Menu macros consist of HyperMesh Tcl modify commands.

Exercise Create a Utility Menu macro from a command file that saves the model and add a button on the User page that will launch the macro: 1.

Define the task.

2.

Delete the existing command.cmf file. This file is located in either the start-in directory or the current working directory.

3.

Perform the operations in HyperMesh that the script should run.

4.

Extract the commands from the command.cmf file.

5.

Add the commands to the userpage.mac file.

6.

Modify as necessary and add macro wrapper commands *beginmacro and *endmacro.

7.

Add macro button using *createbutton that calls the new macro defined in Step 6.

8.

Reload the current .mac file into HyperMesh to load the modified userpage.mac.

9.

Test the macro.

Proprietary Information of Altair Engineering

p.483

Altair HyperMesh 2019 Tutorials

p.484

Step 1: Define the task. The first step in creating a macro is to define the process you want to automate and recognize the individual tasks to reach the desired conclusion. Here, you want to create a one-button macro to automate saving the current HyperMesh model to a file named temp.hm. The actions necessary to complete this task are: •

From the menu bar, select File > Save as > Model….

•

Use the file browser to locate a directory and enter the name for the filename.

•

Click Save.

Step 2: Delete the existing command.cmf file. The current command.cmf file is located in the current working directory. When first opening HyperMesh, the file is created in the directory HyperMesh is launched from. As soon as you begin working in HyperMesh all executed commands are written to the command.cmf file. If the file already exists, the commands are appended to the file. Deleting the file allows HyperMesh to create a new file and allows the user to easily find the relevant commands.

Step 3: Perform the operations in HyperMesh. Execute the full process within HyperMesh. Every command issued in HyperMesh appears in the order executed and is reflected in the command.cmf file. 1.

From the menu bar, select File > Save as > Model….

2.

Using the file browser, locate a directory to save the temporary file with the name temp.hm. Remember this is just a temporary file and will be overwritten each time the macro is executed.

3.

Click Save.

Step 4: Extract the commands from the command.cmf file. 1.

Open the command.cmf file using any text editor.

2.

Locate the *writefile command at or near the end of the command.cmf file. This is the command that writes the model file.

3.

Select and copy this line.

Step 5: Add the commands to the userpage.mac file. 1.

Open the userpage.mac file using any text editor.

2.

Paste the *writefile command copied from the command.cmf file inside the userpage.mac file.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.485

Step 6: Modify as necessary and add Utility Menu macro wrapper commands. 1.

Remove the path in the *writefile command so that it looks like: *writefile("temp.hm",0)

2.

Enclose the commands from Step 5 between the wrapper commands *beginmacro and *endmacro. In the *beginmacro command, name the macro macroSave. *beginmacro(macroSave) *writefile("temp.hm",0) *endmacro() The macro name macroSave will be used to connect the button with the macro via the macroName field in the *createbutton command.

3.

Add the command *answer(yes) after the *writefile command. The command *answer(yes) automatically answers “yes” if prompted to overwrite the file in the event temp.hm already exists.

4.

Save the userpage.mac file.

Step 7: Add the macro button. Create a button on the User page to execute the macro. 1.

Create a new button in the userpage.mac file. *createbutton(5,"Save File",20,0,10,GREEN,"Save file","macroSave") This creates a button on page 5 (User page), names it, places it in the 20th row, starts it at column 0, sets the width at 10 columns, applies to it the color green, provides a help string and references the macro macroSave defined in Step 6.

2.

Save the userpage.mac file.

Step 8: Reload the current .mac file into HyperMesh to load the modified userpage.mac. To reload the current macro menu .mac file while HyperMesh is open, select Preferences > Menu Config from the menu bar and click on retrieve next to macro file. Make sure to load the proper .mac file from the hm\scripts\ directory based on the current user profile, or load the default hm.mac in the hm\bin\ directory if no user profile is loaded.

Step 9: Test the macro. 1.

Click the User button on the Utility Menu. The new button labeled Save File should be on the User page.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

2.

Click this button to automatically save your file. The file is saved to the directory specified in the *writefile command. In this case no directory is specified so HyperMesh saves the file to the start-up or current working directory. It will always save with the name specified in the macro (in this case, temp.hm).

Proprietary Information of Altair Engineering

p.486

Altair HyperMesh 2019 Tutorials

HM-8030: Create a Utility Menu Macro to Create Constraints on a Plane In this tutorial you will: •

Determine the commands to create constraints on a plane

•

Create a Utility Menu macro to execute the commands

•

Create a new button on the User page of the Utility Menu to run the macro

Tools In order to execute command file commands or Tcl scripts from a button on any of the HyperMesh Utility Menu pages, a Utility Menu macro must first be defined. A Utility Menu macro contains valid command file or templex commands that execute the appropriate operations, and is defined using the *beginmacro and *endmacro commands. Macros may accept data passed to them using the arguments $1, $2, etc. Each argument specifies where the values should be substituted. These macros are defined within the .mac files, including the userpage.mac file. The following skeleton code shows the format of a Utility Menu macro: *beginmacro(macroname) command statements go here *endmacro() Utility Menu macros consist of HyperMesh Tcl modify commands. Load collectors can be created and edited using the Model Browser. Simply right-click in the Model Browser and select Create > Load Collector to create one. To edit the name, color, or card image of a load collector, right click on the load collector name in the Model Browser and select Edit The Constraints panel can be accessed from the menu bar by selecting BCs > Create > Constraints The Constraints panel allows you to create and update constraints.

Exercise In this exercise you will create a Utility Menu macro from a command file that creates constraints on a plane and add a button on the User page that will launch the macro: 1.

Define the task.

2.

Delete the existing command.cmf file. This file is located in either the start-in directory or the current working directory.

3.

Perform the operations in HyperMesh that the script should run.

Proprietary Information of Altair Engineering

p.487

Altair HyperMesh 2019 Tutorials

4.

Extract the commands from the command.cmf file.

5.

Add them to the userpage.mac file.

6.

Modify as necessary and add macro wrapper commands *beginmacro and *endmacro.

7.

Add macro button using *createbutton that calls the new macro defined in Step 6.

8.

Reload the current .mac file into HyperMesh to load the modified userpage.mac.

9.

Test the macro.

p.488

Step 1: Define the task. The first step in creating a macro is to define the process you want to automate and recognize the individual tasks to reach the desired conclusion. Here, you want to create a one-button macro to automatically create constraints on certain nodes. The actions necessary to complete this task are: •

Create a load collector for the constraints.

•

Enter the Constraints panel.

•

Apply constraints to the nodes on the end of the beam lying in the YZ plane.

Step 2: Delete the existing command.cmf file. The current command.cmf file is located in the current working directory. When first opening HyperMesh, the file is created in the directory HyperMesh is launched from. As soon as you begin working in HyperMesh all executed commands are written to the command.cmf file. If the file already exists, the commands are appended to the file. Deleting the file allows HyperMesh to create a new file and allows the user to easily find the relevant commands.

Step 3: Perform the operations in HyperMesh. Execute the full process within HyperMesh. Every command issued in HyperMesh appears in the order executed and is reflected in the command.cmf file. 1.

From the menu bar, select File > Open > Model and load the file, c_channel-tcl.hm.

2.

Right click in the Model Browser and select Create > Load Collector.

3.

In the Name field enter the name constraints.

4.

Click create.

5.

Open the Constraints panel.

6.

Active the create subpanel.

7.

Click nodes and select the on plane option. The plane that will be selected is the YZ plane. This is accomplished by selecting the xaxis vector, which is normal to the YZ plane. The base node option is then highlighted, allowing a node on one end of the beam to be selected as the base node for the plane. All nodes on that plane are highlighted when select is clicked.

8.

Click create.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 4: Extract the commands from the command.cmf file. 1.

Open the command.cmf file using any text editor.

2.

Select and copy all lines in the file. Observe the *createmark command and the list of entity ID numbers. A mark is a storage buffer in HyperMesh. For some actions performed on entities, the entity ID is first entered into the designated mark. There are two marks available to the user (1 and 2) for each entity type (elements, nodes, lines, surfaces, points, etc…). At the execution of the command using the mark, the changes apply to all entities identified in the mark.

Step 5: Add the commands to the userpage.mac file. 1.

Open the userpage.mac file using any text editor.

2.

Paste the commands copied from the command.cmf file inside the userpage.mac file.

Step 6: Modify as necessary and add Utility menu macro wrapper commands. 1.

Enclose the commands in Step 5 between the wrapper commands *beginmacro and *endmacro. In the *beginmacro command, name the macro macroEdge_Const as shown, following. Remove any lines copied from the command.cmf file that are not shown in the following. *beginmacro(macroEdge_Const) *collectorcreate(loadcols,"constraints","",11) *createmark(nodes,1) 3358-3360 3296 3297 3142 etc … *loadcreateonentity_curve(nodes,1,3,1,0,0,0,0,0,0,0,0,0,0,0) *endmacro() The macro name macroEdge_Const will be used to connect the button with the macro via the macroName field in the *createbutton command.

2.

Change the *createmark(nodes,1) command to *createmark(nodes,1) "on plane" 0 0 0 1 0 0 0.5 1 0 "on plane" is one of many selection methods available. This method allows the selection of only entities that lie within a tolerance (in this case, 0.5) of the plane defined at the point (0,0,0) with normal vector (1,0,0). In this exercise, this is the YZ plane. See the Entity Selector online help topic for further details. The final macro should look like: *beginmacro(macroEdge_Const) *collectorcreate(loadcols,"constraints","",11)

Proprietary Information of Altair Engineering

p.489

Altair HyperMesh 2019 Tutorials

p.490

*createmark(nodes,1) "on plane" 0 0 0 1 0 0 0.5 1 0 *loadcreateonentity(nodes,1,3,1,0,0,0,0,0,0) *endmacro() 3.

Save the userpage.mac file.

Step 7: Add the macro button. Create a button on the User page to execute the macro. 1.

Create a new button in the userpage.mac file. *createbutton(5,"Edge Const",18,0,10,GREEN,"Add constraints to outer edge of elements","macroEdge_Const") This creates a button on page 5 (User page), names it, places it in the 20th row, starts it at column 0, makes it 10 columns wide, gives it the color green, provides a help string and references the macro macroSave defined in Step 6.

2.

Save the userpage.mac file.

Step 8: Reload the current .mac file into HyperMesh to load the modified userpage.mac. To reload the current macro menu .mac file while HyperMesh is open, select Preferences > Menu Config from the menu bar and click on retrieve next to macro file. Make sure to load the proper .mac file from the hm\scripts\ directory based on the current user profile, or load the default hm.mac in hm\bin\ if no user profile is loaded.

Step 9: Test the macro. 1.

Click the User button on the Utility Menu. The new button labeled Edge Const should be on the User page.

2.

Click this button to run the macro that automatically creates constraints on the outer row of nodes. Some commands used in this exercise are very model-specific. For example, creating a load collector named “constraints” may cause an error if the collector already exists. Also, selecting nodes using the by plane option and specifying the YZ plane may not be applicable to a lot of situations. Several options exist to make the *createmark commands general enough to work with any model. For example, to select all the currently displayed elements in the model use the command *createmark(elements,1) "by displayed". Another option is to replace the *createmark command with *createmarkpanel. When executed, this command presents the user with a selection panel for the entity

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

specified. For this macro, the *createmarkpanel command could be used to allow the user to select the appropriate nodes. Additionally, this Utility Menu macro could be converted to a Tcl script that allows for additional logic and error checking controls. This way, the user could also be prompted to enter a name for the load collector using hm_getstring. An error check could then be performed to determine if that load collector already exists, and appropriate action would then be taken.

Proprietary Information of Altair Engineering

p.491

Altair HyperMesh 2019 Tutorials

HM-8040: Create a Utility Menu Macro from a Tcl Script In this tutorial you will: •

Determine the commands to save the current HyperMesh model

•

Create a Utility Menu macro to execute the commands

•

Create a new button on the User page of the Utility Menu to run the macro

Tools In order to execute command file commands or Tcl scripts from a button on any of the HyperMesh Utility Menu pages, a Utility Menu macro must first be defined. A Utility Menu macro contains valid command file or templex commands that execute the appropriate operations, and is defined using the *beginmacro and *endmacro commands. Macros may accept data passed to them using the arguments $1, $2, etc. Each argument specifies where the values should be substituted. These macros are defined within the .mac files, including the userpage.mac file. The following skeleton code shows the format of a Utility Menu macro: *beginmacro(macroname) command statements go here *endmacro() Utility Menu macros consist of HyperMesh Tcl modify commands.

Exercise In this exercise you will create a Tcl script from the command file commands, create a Utility Menu macro that runs the Tcl script and add a button on the User page that will launch the macro: 1.

Define the task.

2.

Delete the existing command.cmf file. This file is located in either the start-in directory or the current working directory.

3.

Perform the operations in HyperMesh that the script should run.

4.

Extract the commands from the command.cmf file.

5.

Create a Tcl script by converting the commands to Tcl format and modifying as necessary.

6.

Create a new Utility Menu macro that runs a Tcl script.

7.

Add macro button using *createbutton that calls the macro created in Step 6 with the appropriate Tcl script filename.

8.

Reload the current .mac file into HyperMesh to load the modified userpage.mac.

9.

Test the macro.

Proprietary Information of Altair Engineering

p.492

Altair HyperMesh 2019 Tutorials

p.493

Step 1: Define the task. The first step in creating a macro is to define the process you want to automate and recognize the individual tasks to reach the desired conclusion. Here, you want to create a one-button macro to automate saving the current HyperMesh model to a file named temp.hm. The actions necessary to complete this task are: •

From the menu bar, select File > Save as > Model.

•

Use the file browser to locate a directory and enter the name for the filename.

•

Click Save.

Step 2: Delete the existing command.cmf file. The current command.cmf file is located in the current working directory. When first opening HyperMesh, the file is created in the directory HyperMesh is launched from. As soon as you begin working in HyperMesh all executed commands are written to the command.cmf file. If the file already exists, the commands are appended to the file. Deleting the file allows HyperMesh to create a new file and allows the user to easily find the relevant commands.

Step 3: Perform the operations in HyperMesh. Execute the full process within HyperMesh. Every command issued in HyperMesh appears in the order executed and is reflected in the command.cmf file. 1.

From the menu bar, select Files > Save as > Model.

2.

Using the file browser, locate a directory to save the temporary file with the name temp.hm. Remember this is just a temporary file and will be overwritten each time the macro is executed.

3.

Click Save.

Step 4: Extract the commands from the command.cmf file. 1.

Open the command.cmf file using any text editor.

2.

Locate the *writefile command at or near the end of the command.cmf file. This is the command that writes the model file.

3.

Select and copy this line.

Step 5: Create a Tcl script names savefile.tcl, convert the commands to Tcl format and modify as necessary. 1.

Create a new file named savefile.tcl using any text editor.

2.

Paste the *writefile command copied from the command.cmf file inside the savefile.tcl file.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

Remove all () and , and replace them with spaces. Also remove the “ “. The command should look like: *writefile temp.hm 0

4.

Add the command *answer yes after the *writefile command. The command *answer yes automatically answers “yes” if prompted to overwrite the file in the event temp.hm already exists. Notice that there are no parentheses.

5.

Save the savefile.tcl script in the current working directory.

Step 6: Create a Utility Menu macro that runs a Tcl script. 1.

Create a new Utility Menu macro that calls the *evaltclscript command to run a Tcl script, using the macro wrapper commands *beginmacro and *endmacro. In the *beginmacro command, name the macro EvalTcl. *beginmacro("EvalTcl") *evaltclscript($1,0) *endmacro() The macro name EvalTcl will be used to connect the button with the macro via the macroName field in the *createbutton command.

2.

Save the userpage.mac file.

Step 7: Add the macro button. Create a button on the User page to execute the macro. 1.

Create a new button in the userpage.mac file. *createbutton(5,"SaveFile TCL",15,0,10,GREEN,"Save file using TCL macro", "EvalTcl","savefile.tcl") This creates a button on page 5 (User page), names it, places it in the 20th row, starts it at column 0, sets its width at 10 columns, applies to it the color green, provides a help string and references the macro EvalTcl defined in Step 6. Notice that the full path is not used to reference the savefile.tcl script. A full path can be specified if the file is not located in one of the predefined paths that HyperMesh searches to find scripts. Users can add additional search paths using the TCL_INCLUDE environment variable. Relative paths can also be used from these search paths.

2.

Save the userpage.mac file.

Proprietary Information of Altair Engineering

p.494

Altair HyperMesh 2019 Tutorials

p.495

Step 8: Reload the current .mac file into HyperMesh to load the modified userpage.mac. To reload the current macro menu .mac file while HyperMesh is open, select Preferences > Menu Config from the menu bar and click on retrieve next to macro file. Make sure to load the proper .mac file from the hm\scripts\ directory based on the current user profile, or load the default hm.mac in hm\bin\ if no user profile is loaded.

Step 9: Test the macro. 1.

Click the User button on the Utility Menu. The new button labeled Save File TCL should be on the User page.

2.

Click this button to automatically save your file. The file is saved to the directory specified in the *writefile command. In this case no directory is specified so HyperMesh saves the file to the start-up or current working directory. It will always save with the name specified in the macro, in this case temp.hm.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

HM-8050: Create Forces on Nodes and Add a Button on the User Page In this tutorial you will: •

Determine the commands to create forces on nodes

•

Create a Utility menu macro to execute the commands

•

Create a new button on the User page of the Utility Menu to run the macro

Tools In order to execute command file commands or Tcl scripts from a button on any of the HyperMesh Utility Menu pages, a Utility Menu macro must first be defined. A Utility Menu macro contains valid command file or templex commands that execute the appropriate operations, and is defined using the *beginmacro and *endmacro commands. Macros may accept data passed to them using the arguments $1, $2, etc. Each argument specifies where the values should be substituted. These macros are defined within the .mac files, including the userpage.mac file. The following skeleton code shows the format of a Utility menu macro: *beginmacro(macroname) command statements go here *endmacro() Utility menu macros consist of HyperMesh Tcl modify commands. Load collectors can be created and edited using the Model Browser. Simply right click in the Model Browser and select Create > Load Collector to create one. To edit the name, color, or card image of a load collector, right click on the load collector name in the Model Browser and select Edit The Forces panel can be accessed from the menu bar by selecting BCs > Create > Forces. The Forces panel allows you to create and update forces.

Exercise In this exercise you will create a Tcl script from the command file commands, create a Utility Menu macro that runs the Tcl script and add a button on the User page that will launch the macro: 1.

Define the task.

2.

Delete the existing command.cmf file. This file is located in either the start-in directory or the current working directory.

3.

Perform the operations in HyperMesh that the script should run.

Proprietary Information of Altair Engineering

p.496

Altair HyperMesh 2019 Tutorials

4.

Extract the commands from the command.cmf file.

5.

Create a Tcl script by converting the commands to Tcl format and modifying as necessary.

6.

Create a Utility Menu macro that runs a Tcl script.

7.

Add macro button using *createbutton that calls the macro created in Step 6 with the appropriate Tcl script filename.

8.

Reload the current .mac file into HyperMesh to load the modified userpage.mac.

9.

Test the macro.

p.497

Step 1: Define the task. The first step in creating a macro is to define the process you want to automate and recognize the individual tasks to reach the desired conclusion. Here, you want to create a one-button macro to automatically create forces on certain nodes. The actions necessary to complete this task are: •

Create a load collector for the forces

•

Enter the Forces panel

•

Apply forces to the nodes of interest

Step 2: Delete the existing command.cmf file. The current command.cmf file is located in the current working directory. When first opening HyperMesh, the file is created in the directory HyperMesh is launched from. As soon as you begin working in HyperMesh all executed commands are written to the command.cmf file. If the file already exists, the commands are appended to the file. Deleting the file allows HyperMesh to create a new file and allows the user to easily find the relevant commands.

Step 3: Perform the operations in HyperMesh. Execute the full process within HyperMesh. Every command issued in HyperMesh appears in the order executed and is reflected in the command.cmf file. 1.

From the menu bar, select File > Open > Model and then load the file, c_channeltcl.hm.

2.

Right click in the Model Browser and select Create > Load Collector.

3.

In the Name field enter the name forces.

4.

Click Create.

5.

Open the Forces panel.

6.

Activate the create subpanel.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

7.

9.

Click nodes and select one node in the model. •

For the direction of the force choose the z-axis option.

•

For magnitude=, enter 23.

•

Toggle from magnitude % option to uniform size option for load size and set the value to 15.

Click create.

Step 4: Extract the commands from the command.cmf file. 1.

Open the command.cmf file using any text editor or use the Open Command File option in the Scripting Toolbar.

2.

Select and copy the following three lines in the file: *loadsize(1,15,0,1) *createmark(nodes,1) 3237 *loadcreateonentity_curve(nodes,1,1,1,0,0,23,0,0,23,0,0,0,0,0) Observe the *createmark command and the list of entity id numbers. A mark is a storage buffer in HyperMesh. For some actions performed on entities, the entity ID is first entered into the designated mark. There are two marks available to the user (1 and 2) for each entity type (elements, nodes, lines, surfaces, points, etc.). At the execution of the command using the mark, the changes apply to all entities identified in the mark.

Step 5: Create a Tcl script named create_force.tcl, convert the commands to Tcl format and modify as necessary. 1.

Create a new file named create_force.tcl using any text editor.

2.

Paste the copied commands from the command.cmf file inside the create_force.tcl file.

3.

Remove all () and , and replace them with spaces. The commands should look something like: *loadsize 1 15 0 1 *createmark nodes 1 3237 *loadcreateonentity_curve nodes 1 1 1 0 0 23 0 0 23 0 0 0 0 0 Simply running the above commands will work without a problem, but note that the *createmark command is hard coded to the single node picked when generating the command file. Also notice that the magnitude is hard coded as well. This is not very useful for a generic utility.

Proprietary Information of Altair Engineering

p.498

Altair HyperMesh 2019 Tutorials

4.

p.499

Replace the *createmark command with the *createmarkpanel command. The command *createmarkpanel presents the user with a selection panel for the entity specified. The commands should now look like this: *loadsize 1 15 0 1 *createmarkpanel nodes 1 "Select nodes for load creation" *loadcreateonentity_curve nodes 1 1 1 0 0 23 0 0 23 0 0 0 0 0

5.

If you want to let the user specify the magnitude, prompt the user for a value using hm_getfloat. Then replace the hard coded magnitude in the *loadcreateonentity_curve command with the user defined value. The commands should now look like this: *loadsize 1 15 0 1 *createmarkpanel nodes 1 "Select nodes for load creation" set mag_val [hm_getfloat "Magnitude=" "Enter force magnitude:"] *loadcreateonentity_curve nodes 1 1 1 0 0 $mag_val 0 0 $mag_val 0 0 0 0 0

6.

Save the create_force.tcl script.

Step 6: Create a Utility menu macro that runs a Tcl script. 1.

Create a new Utility Menu macro that calls the *evaltclscript command to run a Tcl script, using the macro wrapper commands *beginmacro and *endmacro. In the *beginmacro command, name the macro EvalTcl. *beginmacro("EvalTcl") *evaltclscript($1,0) *endmacro() The macro name EvalTcl will be used to connect the button with the macro via the macroName field in the *createbutton command.

2.

Save the userpage.mac file.

Step 7: Add the macro button. Create a button on the User page to execute the macro. 1.

Create a new button in the userpage.mac file. *createbutton(5,"Create Force",16,0,10,GREEN,"Create z-direction force on selected nodes","EvalTcl","create_force.tcl") This creates a button on page 5 (User page), names it, places it in the 16th row, places its start at column 0, gives it a width of 10 columns, applies to it the color green, provides a help string and references the macro create_force.tcl defined in Step 6.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Notice that the full path is not used to reference the create_force.tcl script. A full path can be specified if the file is not located in one of the predefined paths that HyperMesh searches to find scripts. Users can add additional search paths using the TCL_INCLUDE environment variable. Relative paths can also be used from these search paths. 2.

Save the userpage.mac file.

Step 8: Reload the current .mac file into HyperMesh to load the modified userpage.mac. To reload the current macro menu .mac file while HyperMesh is open from the menu bar select Preferences > Menu Config and click on retrieve next to macro file. Make sure to load the proper .mac file from the hm\scripts\ directory based on the current user profile, or load the default hm.mac in hm\bin\ if no user profile is loaded.

Step 9: Test the macro. 1.

Click the User button on the Utility Menu. The new button labeled Create Force should be on the User page.

2.

Click this button to run the Tcl script that automatically creates forces in the z-direction of the selected nodes. The new forces are created on the specified nodes with the given magnitude and placed in the current load collector If no load collector exists, the forces are placed in a load collector called auto1. It is often necessary to debug Tcl scripts using the Command Window. This allows you to run the Tcl script and easily review error messages, as well as print out debug information. Additional details can be found in the Creating Tcl Scripts and Running Tcl Scripts sections.

Proprietary Information of Altair Engineering

p.500

Altair HyperMesh 2019 Tutorials

p.501

HM-8060: Calculate the Resultant Sum of Forces In this tutorial you will create a Tcl script that: •

Determines the components of a given set of force vectors

•

Calculates a vector resultant sum of the forces

•

Reports the resultant sum

Tools The Tcl commands if, foreach and expr will be used to add logic and mathematical functions to the script. The command hm_getentityvalue is used to extract information from HyperMesh entities, based on data names. Data names are generic references to the information that physically define an entity in the HyperMesh environment. An example of this is the x, y, and z coordinates that define a node location in three-dimensional space. The available data names for each entity can be found in the HyperMesh Reference Guide Data Names topic. Data names are accessed using the hm_getentityvalue command. This command uses the data names available for an entity to return the particular value of interest. The command will return a value that is either a string or a numeric value, depending on the command syntax and the value stored in that particular data name field. The basic syntax of the command is: hm_getentityvalue entity_type id data_name flag where entity_type is the requested entity type (elements, loads, nodes, etc.), id is the entity ID, the data_name is the data field name of interest, and flag is either 0 or 1 depending on whether the command should return a numeric value (0) or a string (1). To retrieve the x-component of a force with ID 12, the following command can be used: set force_x [hm_getentityvalue loads 12 "comp1" 0] Note: To assign the value from the command to a variable, the command is placed within square brackets.

Exercise Create a Tcl script to compute the resultant sum of a given selection of forces. This requires that the script read data from the force entities and manipulate the data to calculate the resultant. To calculate the resultant of the forces, retrieve the x, y, and z components of the forces and compute a vector sum. 1.

Define the process.

2.

Determine the data names to use to extract the force components.

3.

Create the Tcl script and add logic as necessary.

4.

Test the script.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Step 1: Define the process. The script should automate the following process: •

Prompt the user to select a number of forces to calculate the resultant.

•

Make sure the user has selected one or more loads.

•

Extract the components of each force.

•

Sum the components.

•

Report the result to the user.

Step 2: Determine the data names to use to extract the force components. The following table lists several relevant data names for force loads: comp1

x component of the vector

comp2

y component of the vector

comp3

z component of the vector

config

The number "1" for forces The number "2" for moments The number "8" for velocities The number "9" for accelerations

entitytype

the type of entity to which this load is applied (1=node, 3=component, 10=set)

node

when a load is applied to a node, this serves as a pointer to the node

inputsystemid

reference system ID

Steps 3-9: Create the Tcl script and add logic as necessary. A Tcl script to perform this function might be similar to the following:

Step 3: Open a text file and save the file as HM8060.tcl.

Proprietary Information of Altair Engineering

p.502

Altair HyperMesh 2019 Tutorials

p.503

Step 4: Select the desired loads and then add those loads to a list. The *createmarkpanel command is used to allow the user to graphically select the loads from the HyperMesh interface and add them to the mark. The command below adds the loads to mark 1. Once the loads have been added to mark 1, the load ids are assigned to a list called loads_list, using the TCL command set. Add the following 2 lines to the file HM8060.tcl: *createmarkpanel loads 1 "Select forces to compute resultant"; set loads_list [hm_getmark loads 1];

Step 5: Initialize the variables for the x, y, and z components. Use the TCL command set to initialize the variables for the x, y, and z components of force to 0. These variables will be used later in the script to compute the resultant force for each component. Add the following 3 lines to the TCL file HM8060.tcl: set x_comp_sum "0"; set y_comp_sum "0"; set z_comp_sum "0";

Step 6: Begin an if loop which checks to see if the variable loads_list has values. If it does, proceed with the macro. Before calculating the resultant of the forces selected, we should check to make sure that the variable loads_list has values in it. This is done by using an if loop. In the if loop below, we are checking that the variable loads_list is not empty. Add the following line to the TCL file to initialize the if loop: if {$loads_list != ""} {

Step 7: Use a foreach loop to iterate through each load in the list loads_list and extract the x, y, and z components using the hm_getentityvalue command and the appropriate data name. Using a foreach loop, each load in the list loads_list will be iterated through. Within the foreach loop, each load is referenced by load_id and then the component value is added to the previous loads component’s value. For example, let’s look at the x component. Using the set command, the variable x_comp_sum is defined as the previous value of x_comp_sum, plus the x component of the current load. The x component of the current load is retrieved by using the hm_getentityvalue command and the data name comp1 (all the available data names for loads are shown in the table above). This process is done for the y and z components as well. Add the following 4 lines to the TCL file: foreach load_id $loads_list { set x_comp_sum [expr $x_comp_sum + [hm_getentityvalue

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.504

loads $load_id "comp1" 0]]; set y_comp_sum [expr $y_comp_sum + [hm_getentityvalue loads $load_id "comp2" 0]]; set z_comp_sum [expr $z_comp_sum + [hm_getentityvalue loads $load_id "comp3" 0]]; }

Step 8: Report the Resultant Force to the user. Use the command hm_usermessage to report each of the components of the resultant force. Add the following line to the TCL file: hm_usermessage "Resultant force: $x_comp_sum, $y_comp_sum $z_comp_sum ";

Step 9: Complete the if loop and report an error message if no loads are found. To complete the if loop, add an else statement. Remember the if statement checked to see if the variable loads_list was not empty. This else statement returns an error message to the user to let them know that no loads were selected. } else { hm_errormessage "No loads selected"; }

Step 10: Test the script. 1.

From the menu bar, select View > Command Window to display the Command Window at the bottom of the screen.

2.

Click and drag to open the Command Window from the bottom edge of the screen.

3.

Open the file c_channel-tcl.hm.

4.

Use the source command to execute the script. For example: source HM8060.tcl It is often necessary to debug Tcl scripts using the Command Window. This allows you to run the Tcl script and easily review error messages, as well as print out debug information. Additional details can be found in the Creating Tcl Scripts and Running Tcl Scripts sections. There are several important assumptions used when creating this script. •

The user will always select force loads, as opposed to moments, pressures, etc.

•

The forces are applied to nodes, as opposed to comps or sets, and are valid to sum.

•

All of the forces are applied in the same coordinate system so that it is valid to sum the component values directly.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

If any of these assumptions are not true, the values returned by the script may be invalid. Additional conditional logic can be programmed to check for each of these situations and an error message can be returned or they can be handled appropriately. 5.

The result of the macro is shown in the status bar. Either a message with the resultant force is shown or else there is a note saying that no loads were selected.

Proprietary Information of Altair Engineering

p.505

Altair HyperMesh 2019 Tutorials

p.506

HM-8070: Create Spline Surfaces on Tria Elements In this tutorial you will create a Tcl script that creates spline surfaces from the nodes of selected tria elements.

Tools The Tcl commands if, foreach, and incr will be used to add logic to the script. The command hm_getentityvalue is used to extract information from HyperMesh entities, based on data names. Data names are generic references to the information that physically define an entity in the HyperMesh environment. An example of this is the x-, y-, and z-coordinates that define a node location in three-dimensional space. The available data names for each can be found in the HyperMesh Reference Guide Data Names topic. Data names are accessed using the hm_getentityvalue command. This command uses the data names available for an entity to return the particular value of interest. The command will return a value that is either a string or a numeric value, depending on the command syntax and the value stored in that particular data name field. The basic syntax of the command is: hm_getentityvalue entity_type id data_name flag where entity_type is the requested entity type (elements, loads, nodes, etc…), id is the entity ID, the data_name is the data field name of interest, and flag is either 0 or 1 depending on whether the command should return a numeric value (0) or a string (1). To retrieve the x-component of a force with ID 12, the following command can be used: set force_x [hm_getentityvalue loads 12 "comp1" 0] Note that to assign the value from the command to a variable, the command is placed within square brackets.

Exercise Create a Tcl script that creates spline surfaces from the nodes of selected tria elements. This requires that the script read data from the element entities. To create the spline surfaces, retrieve the 3-node IDs of the tria elements. 1.

Define the process.

2.

Determine the data names to use to extract the element type and node IDs.

3.

Create the Tcl script and add logic as necessary.

4.

Test the script.

Step 1: Define the process. The script should automate the following process: •

Prompt the user to select a number of tria elements to create spline surfaces from.

•

Make sure the user has selected one or more elements.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

•

If a selected element is not a tria, skip that element.

•

Extract the node IDs of each element.

•

Create the spline surface from the nodes.

•

Report on the number of spline surfaces created.

p.507

Step 2: Determine the data names to use to extract the element type and node IDs. The following table lists several relevant data names for tria elements: config

The number, “103”

node1

first node (node pointer)

node2

second node (node pointer)

node3

third node (node pointer)

Steps 3-14: Create the Tcl script and add logic as necessary. A Tcl script to perform this function might be similar to the following:

Step 3: Open a text file and save the file as HM8070.tcl. Step 4: Allow the user to select the desired elements and then add those loads to a list The *createmarkpanel command is used to allow the user to graphically select the elements from the HyperMesh interface and add them to the mark. The command below adds the elements to mark 1. Once the elements have been added to mark 1, the element ids are assigned to a list called elems_list, using the TCL command set. Add the following 2 lines to the file HM8070.tcl: *createmarkpanel elems 1 "Select tria elements to create surfaces"; set elems_list [hm_getmark elems 1];

Step 5: Begin an if loop which checks to see if the variable elems_list has values. If it does, proceed with the macro. Before continuing with the macro, we should check to make sure that the variable elems_list has values in it. This is done by using an if loop. In the if loop below, we are checking that the variable elems_list is not empty. Add the following line to the TCL file to initialize the if loop: if {$elems_list != ""} {

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.508

Step 6: Initialize a variable which counts the number of times the foreach loop is entered. The variable success_count is initialized and set to 0. This variable is used to count the number of times the foreach loop (defined in Step 7) is entered. We will use this variable at the end of the script. Add the following line to the TCL script: set success_count 0;

Step 7: Use a foreach loop to iterate through each element in the list elems_list and then set a variable config which stores the element configuration. This is extracted using the hm_getentityvalue command and the appropriate data name. Using a foreach loop, each element in the list elems_list will be iterated through. Within the foreach loop, each load is referenced by elem_id and then the variable config is defined. This variable is set to the result of the hm_getentityvalue which uses the element data name config to report the configuration of the element. A tria element will have an element configuration of 103 while a quad element will have a configuration of 104. Add the following 2 lines to the TCL file: foreach elem_id $elems_list { set config [hm_getentityvalue elems $elem_id "config" 0];

Step 8: Begin an if loop which checks to see if the variable config has a value of 103. If it does, proceed with the macro. Using an if loop, the variable config is checked to see if it doesn’t have a value of 103. A value of 103 means that the element configuration is a tria element. If the value is not equal to 103, the continue statement is used to move outside of the foreach loop. If the value is the config variable is 103, then the macro is continued. Add the following lines to the TCL script: if {$config != 103} { continue; }

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.509

Step 9: Set 3 variables which contain the node id of each of the nodes used to define the tria element. Three variables are defined (node1, node2, and node3) which represent the 3 nodes that define the tria element. These 3 nodes will be used to create the spline surface. Using the hm_getentityvalue command and the element data names node1, node2, and node3 along with the pointer id, the node id is retrieved and assigned to the appropriate variable. Add the following 3 lines to the TCL script: set node1 [hm_getentityvalue elems $elem_id "node1.id" 0]; set node2 [hm_getentityvalue elems $elem_id "node2.id" 0]; set node3 [hm_getentityvalue elems $elem_id "node3.id" 0];

Step 10: Set the appropriate mode to create the surface. Using the *surfacemode command, the surface mode can be set according to the following: 1 – mesh keep surface 2 – mesh delete surface 3 – mesh without surface 4 – surface only In this example, we only want to create a surface, so mode 4 is used. Add the following line to the TCL script: *surfacemode 4;

Step 11: Create a node mark which contains the 3 nodes defined in Step 9 and then use the *splinesurface command to create a spline surface using the nodes in the mark. Using the *createmark, mark 1 for nodes is created and it contains the 3 nodes defined in the variables node1, node2, and node3. *createmark nodes 1 $node1 $node2 $node3; *splinesurface nodes 1 0 1 1;

Step 12: Increase the variable success_count which is used to count the number of times the foreach loop is entered. Then, close the foreach loop.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.510

Using the incr command, the variable success_count is increased. Following this command, a } is used to close the foreach loop. Add the following 2 lines to the TCL script: incr success_count; }

Step 13: Clear the node and element marks, and then use the hm_usermessage command to report the number of spline surfaces created. Using the command *clearmark, mark 1 for the nodes and elements is cleared. Following these commands, the hm_usermessage command is used to report the number of spline surfaces created. The variable success_count is used to do this. Because this variable was increased each time the foreach loop was entered and the element configuration was 103, this variable kept a count of the number of spline surfaces that were created. Add the following 3 lines to the TCL script: *clearmark nodes 1; *clearmark elems 1; hm_usermessage "$success_count splines created."

Step 14: Add an else statement which compliments the if statement which checked to see if the elems_list variable was empty. If it is empty, the else statement is executed. The else statement compliments the if statement defined in Step 5 which checks to see if the elems_list variable is empty. If it is empty the else statement is executed. Inside the else statement, the hm_errormessage command is used to report to the user that no elements were selected. Following the hm_errormessage command, the if statement is closed using a }. Add the following 3 lines to the TCL script file: } else { hm_errormessage "No elements selected"; }

Step 15: Test the script. 1.

From the menu bar, select File > Open > Model and then load the file, splinetcl.hm.

2.

From the menu bar, select View > Command Window display the Command Window at the bottom of the screen.

3.

Click and drag to open the Command Window from the bottom edge of the screen.

4.

Use the source command to execute the script. For example: source HM8070.tcl

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.511

It is often necessary to debug Tcl scripts using the Command Window. This allows you to run the Tcl script and easily review error messages, as well as print out debug information. Additional details can be found in the Creating Tcl Scripts and Running Tcl Scripts sections. 5.

Select a few of the tria elements and observe the spline surfaces that are created.

There are several important things to notice. •

Only first order tria elements are considered. It is possible to add if/elseif logic to support other element configurations.

•

The data names for the nodes associated with an element are pointers. A pointer is used to directly access another data name. This means they “point” to the data names available for nodes. In order to retrieve any data from a pointer, the data name requested for the particular pointer must also be supplied. The additional data names are separated by a period or dot (.).

•

The *entityhighlighting and hm_commandfilestate commands are used to speed up the execution of the script. The *entityhighlighting command disables highlighting entities when the *createmark command is used. The hm_commandfilestate command controls if commands are written out to the command file. It is always important to “reset” these commands after a script is complete or before exiting due to an error.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.512

HM-8080: Calculate the Radius of an Arc In this tutorial you will create a Tcl script that determines the radius of an arc.

Tools The Tcl commands if and expr will be used to add logic and mathematical functions to the script. The command hm_getentityvalue is used to extract information from HyperMesh entities, based on data names. Data names are generic references to the information that physically define an entity in the HyperMesh environment. An example of this is the x, y, and z coordinates that define a node location in three-dimensional space. The available data names for each entity can be found in the HyperMesh Reference Guide Data Names topic. Data names are accessed using the hm_getentityvalue command. This command uses the data names available for an entity to return the particular value of interest. The command will return a value that is either a string or a numeric value, depending on the command syntax and the value stored in that particular data name field. The basic syntax of the command is: hm_getentityvalue entity_type id data_name flag where entity_type is the requested entity type (elements, loads, nodes, etc…), id is the entity ID, the data_name is the data field name of interest, and flag is either 0 or 1 depending on whether the command should return a numeric value (0) or a string (1). To retrieve the x-component of a force with ID 12, the following command can be used: set force_x [hm_getentityvalue loads 12 "comp1" 0] Note that to assign the value from the command to a variable, the command is placed within square brackets.

Exercise Create a Tcl script that determines the radius of a user selected arc. One point on the line and the center of the arc will need to be calculated. 1.

Define the process.

2.

Determine the data names to use to extract the node coordinates.

3.

Create the Tcl script and add logic as necessary.

4.

Test the script.

Step 1: Define the process. The script should automate the following process: •

Prompt the user to select a line.

•

Make sure the user has selected only one line.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.513

•

Determine the center of the arc by creating temporary nodes.

•

Calculate the distance between one end of the arc and the center node using node coordinate data names.

Step 2: Determine the data names to use to extract the node coordinates. The following table lists several relevant data names for nodes: globalx

x coordinate in the global system

globaly

y coordinate in the global system

globalz

z coordinate in the global system

Steps 3-12: Create the Tcl script and add logic as necessary. A Tcl script to perform this function might be similar to the following:

Step 3: Open a text file and save the file as HM8080.tcl. Step 4: Allow the user to select the desired line which defines a circle or an arc and then add that line to a variable The *createmarkpanel command is used to allow the user to graphically select the line which defines a circle or an arc from the HyperMesh interface and add it to the mark. The command below adds the line to mark 1. Once the line has been added to mark 1, the line id is assigned to a variable called line_list, using the TCL command set. Add the following 2 lines to the file HM8080.tcl: *createmarkpanel lines 1 "Select line to find radius"; set line_list [hm_getmark lines 1];

Step 5: Begin an if loop which checks to see if the variable line_list has values. If it does, proceed with the macro. Before continuing with the macro, we should check to make sure that the variable line_list has values in it. This is done by using an if loop. In the if loop below, we are checking to see if the variable line_list is empty. If the variable is empty, an error message is given to the user. Also, using the elseif statement in the if loop, we can check to see if more than one line is selected. If more than one line is selected, an error message is reported. If neither of those conditions are met, the macro proceeds under the else statement. Add the following line to the TCL file to define the if loop:

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.514

if {$line_list == ""} { hm_errormessage "No lines selected"; } elseif {[llength $line_list] != 1} { hm_errormessage "Only one line may be selected"; } else {

Step 6: Create 3 nodes on the line selected and then create a node at the circle center of the 3 nodes. Add those nodes to a variable. Use the *nodecreateonlines command to create 3 nodes on the line which is in mark 1. This is done with the first command below. Then, use the *createcenternode to create a node at the center of a circle formed by the three nodes that were just created in the *nodecreateonlines command. These three nodes are referenced by using -1. -2, and 3 which reference the last node created, the second to last node created, and the third to last node created. Then, the nodes are added to the nodes mark 1 using the *createmark command. Again, the nodes are referenced using -1, -2, -3, and -4 to add the last 4 nodes created to the mark. Finally, the nodes in mark 1 are added to the variable node_list. Add the following 4 lines to the TCL script: *nodecreateonlines lines 1 3 0 0; *createcenternode -1 -2 -3; *createmark nodes 1 -1 -2 -3 -4; set node_list [hm_getmark nodes 1];

Step 7: Use the lindex command to get the node id of the first node in the list node_list. Then get the x, y, and z coordinates for the node. Set a variable called id which contains the node id for the first node in the list node_list. The id for the first node is retrieved using the lindex command which takes the variable node_list and using the index 0, retrieves the first node id in the list. Then, using the variable id and the hm_getentityvalue command with the node data names x, y, and z, the x, y, and z coordinates for the node are set to the variables x1, y1, and z1. Add the following 4 lines to the TCL script: set set set set

id x1 y1 z1

[lindex $node_list [hm_getentityvalue [hm_getentityvalue [hm_getentityvalue

0]; nodes $id "x" 0]; nodes $id "y" 0]; nodes $id "z" 0];

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.515

Step 8: Use the lindex command to get the node id of the last node in the list node_list. Then get the x, y, and z coordinates for the node. Set a variable called id which contains the node id for the last node in the list node_list. The id for the first node is retrieved using the lindex command which takes the variable node_list and using the index 3, retrieves the first node id in the list. Then, using the variable id and the hm_getentityvalue command with the node data names x, y, and z, the x, y, and z coordinates for the node are set to the variables x2, y2, and z2. Add the following 4 lines to the TCL script: set set set set

id x2 y2 z2

[lindex $node_list [hm_getentityvalue [hm_getentityvalue [hm_getentityvalue

3 ]; nodes $id "x" 0]; nodes $id "y" 0]; nodes $id "z" 0];

Step 9: Define three variables which are the x, y, and z distance between the two nodes defined in the last two steps. Three variables are defined which are simply the x, y, and z distance between the two nodes defined in Steps 7 and 8. The component difference between each node is calculated using the coordinates defined in Steps 7 and 8 and the TCL command expr. Add the following 3 lines to the TCL script: set dx [expr $x1 - $x2]; set dy [expr $y1 - $y2]; set dz [expr $z1 - $z2];

Step 10: Define a variable called radius which uses the variables dx, dy, and dz to calculate the radius of the line which is a circle or an arc. Using the three variables which were defined in the previous step (dx, dy, and dz) the magnitude of the distance is calculated. This distance corresponds to the radius of the arc/circle which is defined by the line selected. To calculate the radius, the expr command is used. Add the following line to the TCL script: set radius [expr sqrt(($dx*$dx) + ($dy*$dy) + ($dz*$dz))];

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.516

Step 11: Clear the nodes in the temporary node mark. To clear all the nodes in the temporary node mark, use the *nodecleartempmark command. Add the following command to the TCL script: *nodecleartempmark;

Step 12: Report to the user the radius of the selected line. Using the hm_usermessage command, the value of the variable radius is reported to the user. Also, close the if loop which was started back in Step 5. Add the following two lines to the TCL script: hm_usermessage "Radius = $radius"; }

Step 13: Clear the lines and nodes mark. Using the hm_markclear command, the nodes mark and the lines mark are cleared. Add the following two lines to the TCL script: hm_markclear lines 1; hm_markclear nodes 1;

Step 14: Test the script. 1.

From the File menu, load the file, radius-tcl.hm.

2.

From the menu bar, select View>Command Window to display the Command Window at the bottom of the screen.

3.

Click and drag to open the Command Window from the bottom edge of the screen.

4.

Use the source command to execute the script. For example: source HM8080.tcl It is often necessary to debug Tcl scripts using the command window. This allows you to run the Tcl script and easily review error messages, as well as print out debug information. Additional details can be found in the Creating Tcl Scripts and Running Tcl Scripts sections.

5.

Select different lines to review the calculated radius.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

Important things to notice. • The *entityhighlighting and hm_commandfilestate commands are used to speed up the execution of the script. The *entityhighlighting command disables highlighting entities when the *createmark command is used. The hm_commandfilestate command controls if commands are written out to the command file. It is always important to “reset” these commands after a script is complete or before exiting due to an error.

Proprietary Information of Altair Engineering

p.517

Altair HyperMesh 2019 Tutorials

HM-8090: Create an OptiStruct PSHELL property In this tutorial you will create a Tcl script that: •

Prompts the user for a property name and thickness

•

Creates the property collector

•

Assigns the OptiStruct PSHELL card image to the property collector

•

Assigns the thickness value to the property

Tools The Tcl command if will be used to add logic to the script. The commands *dictionaryload and *attributeupdatedouble are used to assign information to the property collector. Solver-specific data created from the HyperMesh template system is stored in card images. Each piece of data that defines a card image has a text string (data name) and a numeric attribute ID. An example is the Young’s Modulus for a material. Templates exist for each solver supported by HyperMesh and are located in sub-folders under the \templates\feoutput directory. These templates define every solver-specific attribute including data names, attribute IDs, card image formats, and the format of the data upon export. The *defineattribute command is used to define attribute data names and IDs in a template file. In order to determine the commands required to create template-specific data, it is best to run through the process in HyperMesh and to review the commands that are written to the command.cmf file. Property collectors can be created and edited using the Model Browser. Simply right click in the Model Browser and select Create > Property to create one. To change the name, color, or card image of a property collector, right click on the property name in the Model Browser and select Edit

Exercise Create a Tcl script to create a property collector and assign a thickness. This requires that the script prompt the user for a name and a thickness value. 1.

Define the process.

2.

Delete the existing command.cmf file. This file is located in either the start-in directory or the current working directory.

3.

Perform the operations in HyperMesh that the script should run.

4.

Extract the commands from the command.cmf file.

5.

Create a Tcl script by converting the commands to Tcl format and modifying as necessary.

6.

Test the script.

Proprietary Information of Altair Engineering

p.518

Altair HyperMesh 2019 Tutorials

p.519

Step 1: Define the process. The script should automate the following process: •

Prompt the user to enter a name and a thickness value.

•

Make sure a property collector with the supplied name does not already exist.

•

Create the new property collector.

•

Assign the PSHELL card image to the property.

•

Assign the thickness to the PSHELL card.

Step 2: Delete the existing command.cmf file. The current command.cmf file is located in the current working directory. When first opening HyperMesh, the file is created in the directory HyperMesh is launched from. As soon as you begin working in HyperMesh, all executed commands are written to the command.cmf file. If the file already exists, the commands are appended to the file. Deleting the file allows HyperMesh to create a new file and allows the user to easily find the relevant commands.

Step 3: Perform the operations in HyperMesh. Execute the full process within HyperMesh. Every command issued in HyperMesh appears in the order executed and is reflected in the command.cmf file. 1.

If the OptiStruct user profile is not currently loaded, please load it at this time.

2.

Right click in the Model Browser and select Create > Property.

3.

Leave Type set to all and in the Name field, enter a name for the property.

4.

For card image=, select PSHELL.

5.

Check the option for Card edit property upon creation.

6.

Click Create.

7.

Activate the T field and enter a thickness value.

8.

Click return.

Step 4: Extract the commands from the command.cmf file. 1.

Open the command.cmf file using any text editor.

2.

Select and copy all lines in the file.

Step 5: Create a Tcl script by converting the commands to Tcl format and modify it as necessary. 1.

Create a new Tcl file using any text editor.

2.

Paste the copied commands from the command.cmf file inside the Tcl file.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

3.

p.520

Remove all () and , and replace them with spaces. Also place semi-colons (;) at the end of each line. The commands should look something like: *collectorcreateonly properties "my_prop" "" 11; *createmark properties 2 "my_prop"; *dictionaryload properties 2 "C:/Altair/hw12.0/templates/feoutput/optistruct/optistruct" "PSHELL"; *initializeattributes properties “my_prop”; *attributeupdatedouble properties 1 95 1 1 0 0.25;

These commands can now be run to duplicate the creation of the PSHELL property. However, simply running these commands as-is is not very flexible. The property ID, name and values are all hard coded. The template file location in the *dictionaryload command is also hard coded. Finally, there are a lot of extra commands that set unnecessary attributes. 4.

In the *attributeupdatedouble command, the ID of the property is hard coded. In order to make this flexible, you need to replace the hard coded ID with the ID of the new property collector: (Changes to the above commands are shown below in bold print). *collectorcreateonly properties "my_prop" "" 11; *createmark properties 2 -1 set prop_id [hm_getmark props 2]; *dictionaryload properties 2 "C:/Altair/hw12.0/templates/feoutput/optistruct/optistruct" "PSHELL"; *attributeupdatedouble properties $prop_id 95 1 1 0 0.25; Supplying an ID of -1 to the *createmark command can be used to select the most recently created entity.

5.

The template file path is also hard coded. You can make this flexible using the hm_info command: *collectorcreateonly properties "my_prop" "" 11; *createmark properties 2 "my_prop"; set prop_id [hm_getmark props 2]; *dictionaryload properties 2 "[hm_info -appinfo SPECIFIEDPATH TEMPLATES_DIR]/feoutput/optistruct/optistruct" "PSHELL"; *attributeupdatedouble properties $prop_id 95 1 1 0 0.25; The user also needs to be prompted to enter a property name and thickness value. You can then substitute those variables in the relevant commands: set prop_name [hm_getstring "Name="]; set prop_thick [hm_getfloat "Thickness="]; *collectorcreateonly properties "$prop_name" "" 11; *createmark properties 2 "$prop_name";

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

set prop_id [hm_getmark props 2]; *dictionaryload properties 2 "[hm_info -appinfo SPECIFIEDPATH TEMPLATES_DIR]/feoutput/optistruct/optistruct" "PSHELL"; *attributeupdatedouble properties $prop_id 95 1 1 0 $prop_thick; 6.

Finally, You need to add logic to test in order to make sure that the property name and thickness values are valid: set prop_name [hm_getstring "Name="]; if {$prop_name == ""} { hm_errormessage "No name specified."; return; } elseif {[hm_entityinfo exist properties $prop_name –byname] == 1} { hm_errormessage "Property already exists."; return; } set prop_thick [hm_getfloat "Thickness="]; if {$prop_thick == "" || $prop_thick Command Window to display the Command Window at the bottom of the screen.

2.

Click and drag to open the Command Window from the top or bottom edge of the screen.

3.

Use the source command to execute the script. For example: source filename.tcl

It is often necessary to debug Tcl scripts using the Command window. This allows you to run the Tcl script and easily review error messages, as well as print out debug information. Additional details can be found in the Creating Tcl Scripts and Running Tcl Scripts sections.

Proprietary Information of Altair Engineering

p.521

Altair HyperMesh 2019 Tutorials

Post-Processing

Proprietary Information of Altair Engineering

p.522

9

Altair HyperMesh 2019 Tutorials

p.523

HM-9000: Exporting Data for Fatigue Analysis This tutorial demonstrates how to write an input file for a given fatigue solver using the options available on the Fatigue panel.

Model Files This exercise uses the keyhole.hm and keyhole.res files, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Step 1: Retrieve the model file. For this tutorial, retrieve the file, keyhole.hm. This file contains a finite element (FE) model, for which an analysis has already been conducted, to obtain the stress/strain information for durability loads of interest. 1. From the menu bar, click File > Open > Model. 2. Open the keyhole.hm file.

Step 2: Load the results file. 1.

From the menu bar, click File > Load > Results.

2.

Open the keyhole.res file.

Step 3: Export data and write a fatigue solver input deck. 1.

Open the Fatigue panel by clicking fatigue from the Post page.

2.

Toggle FE Analysis Type to static/modal. Results contained in keyhole.res were obtained from linear statics analysis. Note:

3.

Select the transient dynamic option if a dynamic finite element analysis was used to obtain the stress/strain results for the model.

Toggle Output File Format to ascii. Note:

Select the binary option if the fatigue solver allows a binary input file. For more information on fatigue solvers and acceptable input file formats, see the Fatigue panel documentation.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

4.

Click browse… and locate the file folder you want store the file in, then enter a name for the output file. Note:

5.

p.524

This output file is the input file for the fatigue solver.

Click data group = and select any of the data groups that you want to write to the output file. Data groups are organized based on whether nodal or elemental results are available in the results file.

6.

Set select simulation to all. This specifies the data in the results file that is written to the output file. In this case, selecting all writes the stress/strain data for the selected nodes or elements for all loadcases represented in keyhole.res. Note:

You can write out stress/strain information for all of the time steps, or you can choose a range from a starting time step to an ending time step, or you can choose a selection of time steps manually from the available list.

The next sub-step is to select the entities for which the finite element analysis results file is written. Note:

The type of entity you select is based upon the data group you selected. Select nodes if the data group you selected refers to nodal results. Similarly, select elements if the data group you selected refers to elemental results. Select sets to choose a predefined entity set comprised of nodes or elements corresponding to a data group with nodal/elemental results, respectively. If the data group results and the entity type are not the same, HyperMesh displays the error message, "Results file doesn’t contain nodal values."

7.

Set the selector to elems.

8.

Click elems >> by window.

9.

Draw the window as shown in the following image.

10. Click interior. 11. Click select entities.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

12. Click write. An ASCII file is written to the selected directory. You can read this file into the appropriate fatigue solver to complete the fatigue analysis.

Proprietary Information of Altair Engineering

p.525

Altair HyperMesh 2019 Tutorials

HM-9010: Free Body Diagram In this tutorial, you will learn how to: Understand applications for and be able to extract resultant forces and moments from HyperMesh free body diagram (FBD) capabilities, including defining cross-sections for which resultant forces and moments are calculated Perform free body diagrams within HyperMesh to understand load paths and export free body loads to detailed models of interest as boundary conditions (BCs) within a submodeling scheme. This process is graphically shown for reference, following.

Global loads model of a generic wing.

Spar2 element set from the global loads model (middle Spar) with free body loads extracted.

Detailed model of Spar2 with free body loads applied as BCs from global loads model.

Proprietary Information of Altair Engineering

p.526

Altair HyperMesh 2019 Tutorials

p.527

Model Files This tutorial uses the icw_ex1.hm and icw_ex2.hm files, which can be found in the hm.zip file. Copy the file(s) from this directory to your working directory.

Exercise 1: Creating of Shear Moment Diagrams and Potato Plots from Global Loads Model using Resultant Force and Moment Functionality This exercise uses the model file, icw_ex2.hm.

Step 1: Create a coordinate system for spar2. 1.

Open HyperMesh Desktop.

2.

In the User Profiles dialog, set the user profile to OptiStruct.

3.

Open model file, icw_ex1.hm.

4.

Open the Sets browser by clicking Tools > Set Browser from the menu bar. Since you will be working with Spar2, you will need to display the elements which represent Spar2 in the graphics area. Element sets, in addition to components and assemblies, can be used as a model grouping and visualization tool. Elements sets can be created, deleted, made visible, and hidden using the Set browser.

5.

In the Sets browser, Elements folder, right-click on Spar2 and select Isolate from the context menu. The elements representing Spar2 display in the graphics area.

6.

Turn on element shading by clicking the Visualization toolbar.

7.

Open the Nodes panel by clicking Geometry > Create > Nodes > Interpolate Nodes from the menu bar.

8.

Using the node list selector, select the nodes on the top and bottom of the left side.

Proprietary Information of Altair Engineering

(Shaded Elements and Mesh Lines) on

Altair HyperMesh 2019 Tutorials

9.

Click create. HyperMesh creates a node on the left end of Spar2.

10. Repeat step 1.8 and 1.9 to create a node on the right side of Spar2. 11. Click return to exit the Nodes panel. 12. From the menu bar, click Geometry > Create > Systems > Axis Direction. 13. Go to the create by axis direction subpanel to create a system with origin at the left end and x-axis along the length of the spar. 14. Using the origin selector, select the left-middle node. 15. Using the x-axis selector, select the right-middle node for x-axis node. 16. Using the xy plane selector, select the left-top node for the xy-plane node.

17. Toggle to rectangular. 18. Click create.

19. Click return to exit the Systems panel.

Step 2: Create cross-section definitions for Spar2. 1.

Open the FBD Cross-Section Manager tab by clicking Post > Free Body > Cross-Section from the menu bar. Cross-section definitions are determined by the following criteria: •

An element set that contains the nodes that define the cross-section and determines which "side" the resultant force and moment vectors are to be calculated. Only elements connected to the nodes that define the cross-section,

Proprietary Information of Altair Engineering

p.528

Altair HyperMesh 2019 Tutorials

p.529

on one side or the other, need to be included in the element set. However, additional elements can be included for visualization purposes with no effect on the calculations.

2.

•

A node set that defines the cross-section geometry.

•

A summation node that can be any node in the model or that can be automatically set to the calculated centroid of the defined cross-section. Centroidal calculations are performed using nodal coordinates that make up the cross-section only, hence element thicknesses associated with the elements attached to the section are not considered. As such, there could be slight differences in the calculated centroid and the "true" centroid of the section if thicknesses vary throughout the section or the section is overly idealized.

•

(Optional) A result system that defines the coordinate system for which the resultant force and moment vectors are transformed into and output for the selected cross-section(s).

In the FDB Cross-section Manager tab, click the arrow next to Advanced options to display the Auto create cross-section form. Use this form to create cross-sections along the length of Spar2. Resultant force and moment extractions will be performed on these cross-sections to obtain the necessary data to generate shear moment diagrams and potato plots. There are two options to define cross-sections: a manual method and an advanced method. The advanced method automates the creation of "continuous" crosssections. The advanced method will be used in this tutorial. See the online help for details about the manual method.

3.

Click Elements twice.

4.

In the panel area, click elems > by sets.

5.

Select Spar2.

6.

Click select.

7.

Click proceed.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

8.

In the FBD Cross-section Manager tab, click Nodes twice.

9.

Select the left-top and left-bottom nodes which define the first cross-section for Spar2.

p.530

10. Click proceed. 11. In the Element set prefix field, enter Spar2_E. 12. In the Node set prefix, enter Spar2_N. Since the cross-section manager utility creates the necessary element and node sets, you must define a prefix string for both element and node sets. This string will be appended by an incremental number to give each created set a unique name. Optional input includes numbering offset which defines an initial number for which the appended set numbers will begin. 13. Verify that the Sets accumulate checkbox is selected. 14. Click Accept. A spreadsheet populates with the definitions of the cross-sections generated by the Auto create cross-sections utility.

15. Select the Display sections checkbox, and then select any section in the spreadsheet to review the selected cross-section. The graphics area will be updated with the element set, node set, sum node, and result system that define the selected cross-section. Optionally, if you select the Show model checkbox, the entire model will be visible in the graphics area with the selected cross-section highlighted in red and the remainder of the model transparent. 16. Select the first cross-section in the spreadsheet (Spar2_E1; Spar2_N1), hold SHIFT, and select the last cross-section (Spar2_E8; Spar2_N9) to select the cross-sections for updating their result system. 17. Update any single or multiple cross-sections by selecting the cross-sections from the spreadsheet using CTRL/SHIFT and then selecting Summation Node or Result System to update these definitions for all selected cross-sections.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.531

18. Click Result System twice. 19. Select the system located at the left-middle end of Spar2 (system 102 created in Step 1). 20. Click proceed. Note: You may have to display the Longeron2 system collector from the Model browser (Model tab) to display system 102. All cross-sections update to result system 102. Note that system 102 has the x-axis along the length of the spar, y-axis located at the neutral axis of the beam in the plane of the web, and z-axis perpendicular to the web of the beam. Also note that the sum node is set to the default centroid, which automatically calculates the centroid of each cross-section and at which the resulting resultant force and moment calculations will be performed. The result system is the system for which all resultant force and moment result vectors will be transformed into and output.

21. Close the FBD Cross-Section Manager utility.

Step 3: Extract resultant force and moment data for all crosssections of Spar2 for all load cases. 1.

Open the Resultant Force and Moment tab by clicking Post > Free Body > Resultant Force and Moment from the menu bar.

2.

In the .op2/xdb field, open the icw.op2. The selected .op2 file loads into the HyperMesh database for use with all FBD utilities until another .op2 file is selected. It also populates the Subcases list box with all subcases in the selected .op2 file that contain Grid Point Force (GPFORCE) data. See the FBD documentation in the HyperMesh User's Guide for more details.

3.

From the Loadsteps list, select all of the loadsteps using the filter buttons on the top of the list box or with CTRL/SHIFT.

4.

From the Cross-sections list, select all of the Spar2 cross-sections previously defined using the filter buttons on the top of the list box or with CTRL/SHIFT.

5.

Review the following table for a description of the Output options for the resultant force and moment utility. Function

Description

Coordinate System

Defines the coordinate system used for output of node locations (x,y,z) only. The coordinate system does not affect the transformation of the resultant force and

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.532

moment vector results, which is defined by the result system on each cross-section definition. Zero tolerance

Defines any number less than this number is set to zero for numerical issues.

Create load collectors

Creates load collectors containing the results of the resultant force and moment calculations so that the results can be visualized in the graphics area as force and moment vectors.

Show summary table

Brings up a window with formatted results similar to the .csv (comma separated) file. Use this output for quick checks of the data without having to open an alternative spreadsheet or text editor program.

Create .csv file

Creates a .csv file with the results of the resultant force and moment calculations, which can be opened directly within standard spreadsheet applications.

Create .fbd file

Creates an .fbd file with the results of the resultant force and moment calculations, which can be directly read into HyperGraph to create shear moment diagrams and potato plots.

6.

Click Coordinate system twice.

7.

Select coordinate system 102 which is located at left-middle end of Spar2.

8.

Click proceed. Note: You may have to display the Longeron2 system collector from the Model browser to display system 102.

9.

In the Zero tolerance field, enter 0.01.

10. Select the Create load collectors checkbox and optionally select a default color for the created load collectors. 11. Select the Show summary table checkbox. 12. Select the Create .csv file checkbox, and open an existing .csv file (append data) or enter a new file name; in this case, enter icw_res_force_moment.csv.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

13. Select the Create .fbd file checkbox, and open an existing .fbd file (append data) or enter a new file name; in this case, enter icw_res_force_moment.fbd. By default, files are put into the HyperMesh start directory unless you specify another directory or enter a file name. 14. Click Accept. Resultant force and moment calculations are executed on all of the selected cross-sections for all selected subcases. The Resultant Force and Moment Output Summary tab displays the resultant force and moment calculations (see the following image). For each cross-section, there is a separate data block grouped by loadstep. The data block contains crosssection nodal forces, moments, and the sum of those nodal forces and moments about the defined sum node, in this case the calculated centroid of the crosssection. Note that the sum of the moment components (Mx, My, Mz) for each node is not the direct sum, as the (rXF) terms for the force resultant vector about the sum node must also be added to each moment component appropriately. The sum of the forces components (Fx, Fy, Fz) for each node is, however, the simple sum.

15. Optional. Open the .csv (comma separated) file directly with Microsoft Excel by using Windows Explorer and double-clicking the file, icw_res_force_moment.csv. This file contains the same results as the summary table in the previous image, but is available for import into standard spreadsheet or text editor programs. 16. Optional. Open the .fbd file, icw_res_force_moment.fbd, in any standard text editor program. By default, files are put into the HyperMesh start directory unless you specify another directory or enter a file name. This file contains the same results as the summary table in the previous image, but in a compact format for use with HyperGraph in generating shear moment diagrams and potato plots of resultant force and moment data for various cross-sections. 17. Close the Resultant Force and Moment tab.

Proprietary Information of Altair Engineering

p.533

Altair HyperMesh 2019 Tutorials

Vector review of the Resultant Force and Moment results in the graphics area is covered in the next step.

Step 4: Use FBD Results Manager to review resultant force and moment vectors in graphics area. 1.

From the menu bar, select Post > Free Body Results Manager to open the FBD Results Manager tab.

2.

Click Element Set twice.

3.

Click set, and select Spar2_E2.

4.

Click proceed.

Proprietary Information of Altair Engineering

p.534

Altair HyperMesh 2019 Tutorials

5.

In the FDB Results Manager window, activate the Show model check box to display the entire model with the selected element set highlighted in red and all other elements transparent. This feature will help you easily locate the element set within the model.

6.

For Results type, select Resultant Force and Moment. This operation scans the database for available loadsteps with resultant force and moment results and populates the Loadsteps: list box.

7.

For Loadsteps, select SUBCASE1. This operation scans the database for available node sets with resultant force and moment results and populates the Node sets: list box.

8.

For Node sets, select Spar2_N3. This operation will scan the database for available force and moment vector results and will enable the check boxes for those force and moment vectors which are available.

9.

For Display options, select Fy (shear—the results coordinate system had y-axis in the plane of the web) and Mz (principal bending moment—the results coordinate system had z-axis perpendicular to the plane of the web). To determine the result coordinate system applied to a given cross-section of interest, use the FBD Cross-Section Manager to review the defined cross-section. This operation will show the element set, node set, results system, and sum node defined for the selected cross-section. Optionally, select other force components to review their magnitude and direction in the graphics area. Single or multiple force and moment vector results can be displayed in the graphics area to facilitate data mining and reporting.

10. (Optional) Select Update load collector color and select color to change the color of the selected load vectors. The new color setting applies only to the load components selected and is saved in the database. Therefore, this option can be used to recolor any single or multiple load vectors for any FBD result. 11. Click Accept to visualize the resultant force and moment vectors in the graphics area. 12. (Optional) Continue to review resultant force and moment vectors following Steps 4.2-4.14 for additional cross-sections. 13. Click Reset to clear the display and reset the form.

Proprietary Information of Altair Engineering

p.535

Altair HyperMesh 2019 Tutorials

p.536

14. Click Close to exit FBD Results Manager.

Step 5: Generate potato plots for Spar2 for selected crosssections. 1.

Click the Add Page

to create a new page.

2.

On the toolbar, use the pull-down menu to switch to the HyperGraph 2D client.

3.

From the menu bar, select Tools > Free Body Diagrams > Potato Plot to open the Potato Plot dialog.

4.

Click fbd file (

) to load the file, icw_res_force_moment.fbd.

The available cross-sections and loadstpes within the .fbd file are loaded into the form. 5.

From the Sections list, select cross-section Spar2_E1_Spar2_N1 as the crosssection for which to generate potato plots. Potato plots generate a single plot for each selected cross-section which contains data points for all selected loadsteps Potato plots effectively "take a slice" through shear moment diagrams at a given cross-section for all selected loadsteps. Since Spar2_E1_Spar2_N1 is the wing root section for Spar2, it will be the largest loaded section and hence can be utilized to determine the critical loadsteps for Spar2. Potato plots can facilitate critical loadstep determination by identifying maximum and minimum loads on given cross-section. In this case, you are going to be interested in identifying maximum and minimum shear and moment forces, Fy and Mz respectively. There are other methods for determining critical loadsteps and standard practices and methods should be examined and utilized.

6.

From the Loadsteps list, select all loadsteps using filter buttons next to the list box or using CTRL/SHIFT.

7.

On the Potato Plots tab, for X component select Fy (shear).

8.

For Y Component, select Mz (principal bending moment).

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

9.

p.537

Click Add plot. Note:

You can add additional potato plots by selecting alternative X and Y components and clicking Add Plot. You can also delete defined plots by selecting the plots from the spreadsheet area and clicking Delete Plots.

10. (Optional) On the Plot Titles tab, enter a Title and Subtitle. 11. On the Plot Options tab, for Reverse sign select cross-section Spar2_E1_Spar2_N1 in the top drop-down list. 12. Select Reverse selected section in the bottom drop-down list. The explanation for the reverse cross-section options is discussed in Step 6.11. 13. Activate the Label points: Loadstep check box. 14. Click Apply to generate the requested potato plots. Since one cross-section was selected, one plot will be generated (one for each crosssection). Potato plots are typically used to determine the loadsteps from which maximum/minimum behavior occurs. From the resulting potato plot of cross-section Spar2_E1_Spar2_N1 it can be determined that maximum/minimum loadsteps for shear and moment are SUBCASES 9, 11, 14, and 16. These critical loadsteps will be considered in future submodeling procedures as a subset of all the loadsteps used to design the spar. FBD forces will be extracted from these loadsteps in Exercise #2 and applied to a detailed model of Spar2 so that FBD analysis and design of the spar can be performed.

Step 6: Generate shear moment diagrams for Spar2 for selected subcases. 1.

Click the Add Page

to create a new page.

2.

From the menu bar, select Tools > Free Body Diagrams > Shear Moment Plot to open the Shear Moment Plot panel.

3.

Click fbd file (

) to load the file, icw_res_force_moment.fbd.

The available cross-sections and loadsteps within the .fbd file are loaded into the form. 4.

From the Sections list, select all sections related to Spar2 (Spar2_E1_Spar_N1 through Spar2_E8_Spar2_N9) using filter buttons next to the list box or using CTRL/SHIFT.

5.

From the Loadsteps list, select SUBCASE 9, SUBCASE 11, SUBCASE 14, and SUBCASE 16 the critical loadsteps determined in Step 6.5.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

6.

p.538

On the VMT Plots tab, for X component select X. The (X) X component is selected because the resultant force and moment extraction coordinate system was performed with coordinate system 102 which has the x-axis along the length of the Spar. Options for X component include X, Y, or Z coordinates as defined from the coordinate system selected to perform the resultant force and moment extraction (Step 3, part 6).

7.

On the VMT Plots tab, for Y component select Fy and Mz to plot the shear and principal bending moment for Spar2. To determine the result coordinate system applied to a given cross-section of interest, use FBD Cross-Section Manager to review the defined cross-section. This operation will show the element set, node set, results system, and sum node defined for the selected cross-section and can help in identifying which components of force or moment are required for the desired plot.

8.

(Optional) On the Plot Titles tab, type a Title and Subtitle.

9.

On the Plot Options tab, for Reverse sign select cross-section Spar2_E1_Spar2_N1 in the top drop-down list.

10. Select Reverse selected section in the bottom drop-down list. The option allows for methods to reverse the sign of the results from any single or multiple cross-sections. The option is useful since, for this particular plot, all crosssections were defined coming from the right. However the first section [Spar2_E1_Spar2_N1], since it has no elements to the left of this cross-section, can only be defined from the left. Cross-sections, defined by the nodes and elements within their respective sets, can be defined coming from the left or right depending on the elements chosen for any given nodal cross-section definition. Therefore any given cross-section can be defined from the left or from the right. The only difference in the results defined either way is that the results will be opposite in sign but equal in magnitude. Either way, for a shear moment diagram, it is important that all selected cross-sections be defined coming from the same direction so that the resulting plot is valid. 11. Verify that the Envelop results check box is deactivated. If you only want the maximum/minimum selected Y components to be plotted from all selected loadsteps for each cross-section, activate the envelop check box. For this tutorial, do not activate this check box. 12. For Layout, select the layout of plots desired. This option affects the number of resulting plots that will be generated. The options are: One plot per loadstep, One plot per Y Component, and One curve per plot. The total number of curves that are generated is always (Curves = number or loadsteps * number of Y components). In this example, since you selected four loadsteps and two Y components, there are a total of eight curves that will be extracted. The number of plots that these eight curves will be displayed on depends on the layout selection. With the option One Plot per loadstep, there are four plots since there are four loadsteps; each plot with both selected Y components, or in this case shear and moment on a single plot for each loadstep. The results of this layout option are shown in first picture, following. With the option, One Plot per Y component, there are two plots since there are two Y components, each plot with all four selected loadsteps, or in this case shear on one plot and moment on another plot for all four selected loadsteps. The results of this layout option are shown in the second picture, following. Try both options. 13. Click Apply to generate the shear moment plots.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

These plots can be used with traditional mechanics of materials calculations such as S = My/I and T = VQ/IT to calculate stresses for various cross-sections. The plots provide the M (bending or Mz) and V (shear or Fy) values to these equations which when coupled with cross-section properties which can be calculated using HyperBeam (from the main menu, select the1D page, then select HyperBeam), allows for the calculation of the cross-section stresses.

Proprietary Information of Altair Engineering

p.539

Altair HyperMesh 2019 Tutorials

p.540

Exercise 2: Extracting Free Body Diagrams from Global Loads Model and Transferring to Detailed Model as Boundary Conditions – Submodeling Techniques This exercise uses the model file, icw_ex2.hm.

Step 1: Extract free body diagrams for Spar2 using FBD Forces utility. 1.

If continuing from Exercise 1, proceed; otherwise open HyperMesh and load the model file, icw_ex2.hm.

2.

From the menu bar select Post > Free Body > Force to open the FBD Forces tab.

3.

If the icw.op2 file is currently loaded, proceed; otherwise, from the .op2 file: browser, select icw.op2. The selected .op2 file loads into the HyperMesh database for use with all FBD utilities until another .op2 file is selected. It also populates the Subcases list box with all subcases in the selected .op2 file that contain Grid Point Force (GPFORCE) data. See the FBD documentation in the HyperMesh User's Guide for more details.

4.

In the Loadsteps list, select SUBCASE 9, SUBCASE 11, SUBCASE 14, and SUBCASE 16, the critical subcases determined in Exercise 1, Step 5.

5.

In the Entity selection area, click Element Set twice.

6.

Click set, then select the Spar2 element set.

7.

Click proceed. Elements that represent Spar2 are now displayed in the graphics area. To turn on element shading, click Shaded Elements and Mesh Lines (

8.

Click Result System twice. The graphic area is updated with all systems in the model.

Proprietary Information of Altair Engineering

).

Altair HyperMesh 2019 Tutorials

9.

p.541

Select the system located at the left-middle end of Spar2 (system 102 created in Exercise 1, Step 1), and click proceed. Note: You may have to display the Longeron2 system collector from the Model Browser to display system 102. The result system is the system for which all free body force and moment result vectors will be transformed into and output.

10. Click Summation Node twice, select the left-bottom node, and then click proceed. This summation node is the node for which all free body force and moment vector results will be summed about to generate a single equivalent resultant force and moment vector. Note that for a free body (all loads), the summation about any point must be zero. Therefore, this feature is typically used to verify that the extraction produced a free body with zero summation. However, if a free body other than (all loads) is performed, the selection of the summation node can be used to determine the equivalent resultant force and moment vector for the extracted free body (applied load only or reaction loads only) which in general will not be zero and can be of interest.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.542

Review the following table for a description of the Output options for the FBD Forces utility. Output Function

Description

FBD type

Defines the types of grid point forces (GPFORCE) to consider in the free body extraction. GPFORCE data available at any given node includes, element, applied, SPC, and MPC forces. FBD types include; All loads (which considers all GPFORCE data), Applied loads only (which only considers applied forces only), and Reaction loads only (which considers SPC and MPC forces only).

Zero tolerance

Defines any number less than this number is set to zero for numerical issues.

Create load collectors

Creates load collectors containing the results of the FBD force calculations so that the results can be visualized in the graphics area as force and moment vectors.

Show summary table

This option brings up a window with formatted results similar to the .csv (comma separated)file. Use this output for quick checks of the data without having to open an alternative spreadsheet or text editor program.

Create .csv file

Creates a .csv file with the results of the resultant force and moment calculations, which can be opened directly within any standard spreadsheet applications.

11. For FBD type, select All Loads. 12. For Zero tolerance, type 0.01. 13. Activate Create load collectors and optionally select a default color for the created load collectors. 14. Activate Show summary table. 15. Activate Create .csv file, browse to the desired location, and type icw_fbd_force.csv. 16. Click Accept to execute the FBD forces calculations for all selected subcases. The FBD Forces Output Summary window displays the FBD forces calculations (see following image). There is a separate data block grouped by loadstep. The data block contains free body nodal forces, moments, and the sum of those nodal forces and moments about the defined sum node. Note that the sum of the moment components (Mx, My, Mz) for each node is not the direct sum as the (rXF) terms for the force resultant vector about the sum node must also be added to each moment component appropriately. The sum of the forces components (Fx, Fy, Fz) for each node is, however, the simple sum. In addition, the sum for a Free Body – All Loads result should be, and is, zero about any sum node selected. You can verify this with the SUM line at the bottom of each data block. For other FBD types, however, the sum about the sum node may or may not be zero, depending on the selections.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

17. (Optional) Open the icw_fbd_forces.csv file directly with Microsoft Excel by double-clicking the file in Windows Explorer. This file contains the same results as the summary table in the previous image, but is available for import into standard spreadsheet or text editor programs. 18. Click Close to exit the FBD Forces utility. Vector review of the FBD forces results in the graphics area is covered in the next step.

Step 2: Use FBD Results Manager to review FBD force vectors in graphics area. 1.

From the menu bar, select Post, then Free Body Results Manager to open the FBD Results Manager tab.

2.

Click Element Set twice.

3.

Click set, then check Spar2.

4.

Click select.

5.

Click proceed.

6.

(Optional) Activate the Show model check box to display the entire model with the selected element set highlighted in red and all other elements transparent. This feature will help you easily locate the element set within the model.

7.

For Results type, select FBD Forces – All Loads. This operation scans the database for available loadsteps with FBD Forces – All Loads results and populates the Loadsteps list box.

8.

For Loadsteps, select SUBCASE 9. This operation will scan the database for available force and moment vector results and will enable the check boxes for those force and moment vectors that are available.

Proprietary Information of Altair Engineering

p.543

Altair HyperMesh 2019 Tutorials

9.

For Display options, select Fy (shear—the results coordinate system had y-axis in the plane of the web). To determine the result coordinate system applied to a given cross-section of interest, use FBD Cross-Section Manager to review the defined cross-section. This operation will show the element set, node set, results system, and sum node defined for the selected cross-section. Optionally, select other force components to review their magnitude and direction in the graphics area. Single or multiple force and moment vector results can be displayed in the graphics area to facilitate data mining and reporting.

10. (Optional) Select Update load collector color and select color to change the color of the selected load vectors. The new color setting applies only to the load components selected and are saved in the database. Therefore, this option can be used to recolor any single or multiple load vectors for any FBD result. 11. Click Accept to make visible the FBD force vectors in the graphics area. 12. (Optional) Continue to review FBD Forces – All Load vector results following steps 2.6 – 2.13 for additional loadsteps and force/moment components. 13. Click Reset to clear the display and reset the form. 14. Click Close to exit the FBD Results Manager utility.

Step 3: Use FBD Export Manager to export FBD Forces to .fem file. 1.

From the menu bar, select Post, then Free Body Export Manager to open the FBD Export Manger tab.

2.

Click Element Set twice.

3.

Click set, then select Spar2.

4.

Click proceed.

5.

For Results type, select FBD Forces – All Loads. This operation scans the database for available loadsteps with FBD Forces – All Loads results and populates the Loadsteps list box.

6.

For Loadsteps, Select SUBCASE 9, SUBCASE 11, SUBCASE 14, SUBCASE 16.

7.

Check the options for Create appropriate loadsteps, and for Output file, browse to the desired location and enter spar2_fbd_forces.fem.

Proprietary Information of Altair Engineering

p.544

Altair HyperMesh 2019 Tutorials

8.

p.545

Click Add to Export. This operation turns on the display of all load collectors associated with the currently selected FBD result type for all selected loadsteps. Additional loadsteps can be selected and accepted, which will append to the current display on each click of accept. In addition, a new element set or FBD result type can be selected and appended to the current display on each click of accept. To clear the display click Reset.

9.

Click Export. This operation will export the currently displayed loads and all other associated/required cards to the output file selected. This file can subsequently be imported into another HyperMesh database (typically called the detailed model) and the loads contained therein can be "attached" to the structure of the detailed model as boundary conditions with the addition of a rigid body constraint. This process will be carried out in the next step.

10. Click Reset. This operation clears the current display. 11. Click Close to exit the FBD Export Manager utility. 12. (Optional) On the File menu, click Save as…, and save the HyperMesh database as icw_final.hm. 13. From the menu bar, select File, then Exit to exit HyperMesh.

Step 4: Import FBD forces from .fem file into detailed model and solve. 1.

Load the model file, spar2_ex2.hm.

2.

From the menu bar, select File > Import > Solver Deck to open the Import tab.

3.

Select File type: OptiStruct, and browse for file: spar2_fbd_forces.fem.

4.

Click Import. This operation imports the free body loads from the global model into the detailed model of Spar2. The next process is to "attach" the free body loads to the detailed model, perform some clean-up operations, define new loadsteps with the free body loads and a rigid body constraint, and solve the detailed model. This process will be accomplished in the remainder of this step.

5.

From the menu bar, select Mesh, then Check, then Nodes, then Equivalence to go to the Edges panel. The nodes of the imported loads are equivalenced with those of the detailed model which are overlaying each other as a consequence of importing the free body loads.

6.

Toggle the selector from comps to elems.

7.

Click elems >> displayed.

8.

Click preview equiv. Eighteen nodes should be found, one at each load.

9.

Click equivalence to combine nodes that were imported and attached to the loads with those that are a part of the detailed mesh of Spar2. Note:

When the detailed Spar2 mesh was constructed, attention to where these interface nodes were located was taken into account by placing fixed points on the surfaces at these locations. The fixed points maintain a node at that

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

p.546

location from the automesher and thus guarantee that a node will exist where a load is located. This method is only one of several potential methods. Other options could include importing the loads which do not line up with any other nodes in the detailed mesh and then connecting the loads to the detailed mesh with R-type elements (RBE2 or RBE3). Several other possibilities could also exist and best methods and practices should be considered depending on the problem type. 10. Click return to exit the Edges panel. to open the Delete panel.

11. Click Delete 12. Click comps.

13. Select TempMass. 14. Click select. 15. Click delete entity to delete the TempMass component entity. 16. Click return to exit the Delete panel. 17. On the Model tab, select the LoadCollector folder, right-click to bring up the context menu, and select Hide to remove all loads from the graphics area. 18. To define a rigid body constraint perform the following: •

Create a load collector for the rigid body constraint definition. From the menu bar, select Collectors, then Create, then Load Collectors to to open the Create Load Collector dialog box.

•

In the Name field enter Const.

•

Select color red.

•

Set Card Image to none.

•

Click create. Note:

This operation sets the current load collector to the newly created Const load collector. The current load collector is the collector which any newly created load (constrains in this case) are placed into.

•

Assign an analysis system to the nodes for which the rigid body constraint will be applied. From the menu bar, select Mesh, then Assign, then Node Analysis System to go to the Systems: Assign subpanel.

•

Select the three nodes highlighted in the following image.

•

Click system.

•

Select system 102 on left-middle end (x-axis along length, y-axis along web, zaxis normal to web). Note:

You may have to display the Longeron2 system collector from the Model browser (Model tab) to display system 102.

•

Click set displacement.

•

Click return to exit the Systems panel.

Proprietary Information of Altair Engineering

Altair HyperMesh 2019 Tutorials

•

Assign a constraint to left-bottom node. From the menu bar, select BCs, then Create, then Constraints to go to the Constraints panel.

•

Select the left-bottom node.

•

Select dof1, dof2, and dof3. Make sure all other dofs are unselected.

•

Click create.

•

Select the left-top node.

•

Select dof1 and dof3. Make sure all other dofs are unselected.

•

Click create.

•

Select the right-bottom node.

•

Select dof3. Make sure all other dofs are unselected.

•

Click create.

•

Click return to exit the Constraints panel.

19. To update the loadsteps for all four free body load cases, perform the following: •

From the menu bar, select Setup, then Edit, then LoadSteps to go to the LoadSteps panel.

•

Click name = and select SUBCASE 9.

•

Toggle type to linear static.

•

Select SPC, click =, and select Const load collector.

•

Click update.

•

Repeat steps for SUBCASE 11, SUBCASE 14, and SUBCASE 16.

20. From the menu bar, select Setup > Create > Control Cards to go to the Control Cards panel. 21. Click FORMAT. 22. For number_of_formats enter 2, and then hit ENTER on the keyboard. There are now two FORMAT buttons. 23. Click each FORMAT button and set them to HM and OUTPUT2, respectively. 24. Click return to specify output file formats for HyperMesh .res (HM) and .op2 which can be used in HyperView to post-process the results. 25. Click GLOBAL_OUTPUT_REQUEST

Proprietary Information of Altair Engineering

p.547

Altair HyperMesh 2019 Tutorials

26. Click DISPLACEMENT and STRESS. 27. Click return to request displacement output for both output formats. 28. Click return to exit the Control Cards panel. 29. From the menu bar, select File > Save As…, and save the model as spar2_ex2_analysis.hm. 30. From the Analysis page, click OptiStruct to run the model. 31. For run options, toggle to analysis. 32. For export options, toggle to all. 33. Click OptiStruct to export the solver deck and run the analysis in OptiStruct. If – optiskip appears in the options field, clear the field before clicking OptiStruct. 34. Once OptiStruct finishes, click return to exit the OptiStruct panel. 35. In the Post menu, click Deformed panel and review the results of the analysis. 36. Click Simulation = and select SUB9 – PosShear PosMoment PosT. 37. Click data type = and select Displacements. 38. Click deform to produce the deformed shape of Spar2 in the graphics area for the selected simulation. 39. Click return to exit the Deformed panel. 40. In the Post menu, click contour to go to the Contour panel and review the results of analysis. 41. Click Simulation = and select SUB9 – PosShear PosMoment PosT. 42. Click data type = and select Von Mises Stress. 43. Select the legend subpanel. 44. Toggle find maximum to maximum = and enter 100000. 45. Click contour to produce the contour plot in the graphics area. 46. (Optional) Continue to use the contour panel to review additional results. 47. Click return to exit the Contour panel. 48. (Optional) From the menu bar, select File, then Save. This operation saves the current HyperMesh database, spar2_ex2_analysis.hm.

Proprietary Information of Altair Engineering

p.548

Altair HyperMesh 2019 Tutorials

49. From the menu bar, select File, then Exit to exit HyperMesh.

Proprietary Information of Altair Engineering

p.549