Using Altair®HyperMesh® to interfacewith LS-DYNA®For technical support, contact us at:Phone (248) 614-2425.Mon – Thurs: 8:00 AM to 7:00 PM (EST).Fri: 8:00 AM to 5:00 PM (EST).Ask for HyperMesh SupportFax (248) 614-2410Email hmsupport@Web FTP Site:Address or Login ftpPassword <your email address>Copyright © 2003 Altair Engineering, Inc., All rights reserved.Using Altair® HyperMesh® to Interface with LS-DYNA®Trademark Acknowledgments:Altair HyperMesh is a registered trademark of Altair Engineering, Inc.All other trademarks and registered trademarks are the property of their respective owners.HW_LS-DYNA_Training_6.0.doc Created on 10/31/2003 1:04 PMPage ii Using Altair HyperMesh to interface with LS-DYNA Altair Engineering, Inc.Table of ContentsTable of Contents (iii)Introduction (1)Setting up HyperMesh to interface to LS-DYNA (1)Chapter 1: Crashing Tubes (3)Exercise 1: Prepare for Modeling (4)Exercise 2: Creating material collectors (5)Exercise 3: Define the section cards for the components (7)Exercise 4: Define the boundary conditions (9)Exercise 5: Defining the Contact between the tubes (12)Exercise 6: Setting up the analysis run (15)Exercise 7: Export the Dyna Deck and running the analysis (16)Chapter 2: Post-Processing using HyperView (17)The HyperView Screen Display (17)The HyperView Menu (19)Exercise 1: Open a d3plot file (20)Exercise 2: Animating the Results and manipulating the view (21)Exercise 3: Using View Controls (23)Displaying results (25)Exercise 4: Displaying the Results Contour (26)Exercise 5: Reviewing the Deformed Shape (28)Exercise 6: Creating a measure plot (30)Exercise 7: Saving the H3D file (31)Chapter 3: Airbag model (35)Exercise 1: Retrieve the file and load the LS-DYNA user profile (36)Exercise 2: Define the airbag (37)Exercise 3: Define the initial velocity for the head (39)Exercise 4: Define the acceleration for the head (40)Exercise 5: Define contact between airbag and head (42)Exercise 6: Define contact for the airbag (43)Exercise 7: Define the contact between the RigidPlate and the Airbag (44)Altair Engineering, Inc. Using Altair HyperMesh to interface with LS-DYNA Page iiiExercise 8: Define the *DEFORMABLE_TO_RIGID card (46)Exercise 9: review the analysis parameters and export the LS-DYNA Deck (49)Chapter 4: Post processing airbag results (51)Exercise 1: Plot the Airbag Volume (52)Exercise 2: Plot the Energy (53)Exercise 3: Adding the Animation (54)Exercise 4: Creating and Using a Report Template (54)Chapter 5: Create Joints (57)Exercise 1: Retrieve a HyperMesh binary database (57)Exercise 2: Creation of a spherical joint (*CONSTRAINED_JOINT_SPHERICAL) (59)Exercise 3: Creation of extra node for rigid body (*CONSTRAINED_EXTRA_NODES_NODE) (61)Exercise 4: Creation of a revolute joint (*CONSTRAINED_JOINT_REVOLUTE) (63)Chapter 6: Bumper impacting a deformable barrier (67)Exercise 1: Retrieve a HyperMesh binary database (68)Exercise 2: Update the inertia properties of the Vehicle Mass (68)Exercise 3: Definition of Boundary Conditions (70)Exercise 4: Apply the initial velocity (*INITIAL_VELOCITY) (72)Exercise 5: Constrain the Crashboxes to the Vehicle Mass (74)Exercise 6: Define Contacts (75)Exercise 7: Create *DATABASE_CROSS_SECTION (78)Exercise 8: Definition of a Rigid Wall (*RIGID_WALL_PLANAR_FINITE) (81)Exercise 9: Setting up output requests (84)Exercise 10: Review of output requests and other control card definitions (84)Chapter 7: Post-Processing the bumper analyis (87)Exercise 1: Loading the LS-DYNA animation results (88)Exercise 2: Creating a plot using the secforc file (89)Exercise 3: Loading the digital video AVI file (90)Page iv Using Altair HyperMesh to interface with LS-DYNA Altair Engineering, Inc.IntroductionSetting up HyperMesh to interface to LS-DYNATo efficiently work with LS-DYNA, the user needs to load the LS-DYNA user profile. The user profile sets the HyperMesh feoutput template and LS-DYNA specific macro file so that the models created can be formatted for LS-DYNA.To use HyperMesh with a specific solver, a feoutput template for the solver has to be loaded. This template contains the solver specific formatting instructions that HyperMesh will use when writing the binary HyperMesh database as a solver input deck. HyperMesh has three main templates for LS-DYNA. dyna.key supports the Keyword input format, dyna.seq supports the sequential input format of LS-DYNA, and dyna.lrg supports the large format that is also a sequential input format. Additionally, the template curves.key is provided to output the curves defined in the database. The dyna.key template is loaded when the LsDyna user profile is selected.The LS-DYNA macro file contains a number of specific tools to help the user review model information and shortcuts to help create many of the LS-DYNA input cards.To load the LS-DYNA user profile1. Click the user prof… button on the Geom page of HyperMesh to bring upthe User Profile selection dialog.2. Select LsDyna from the drop down menu.3. Click OK to close the dialog and load the LS-DYNA user profile.Altair Engineering, Inc. Using Altair HyperMesh to interface with LS-DYNA Page 1IntroductionPage 2 Using Altair HyperMesh to interface with LS-DYNA Altair Engineering, Inc.Chapter 1: Crashing TubesIn this chapter, set up a simulation of two tubes crashing against one another. The entire process can be broken down into 3 steps:Prepare for modeling•Open a HyperMesh binary database containing the finite element mesh.•Create the material, section and part definitions for the modelCreate the boundary conditions•Constrain the ends of the fixed tube (*BOUNDARY_SPC_NODE)•Apply an initial velocity along the X direction to the moving tube (*INITIAL_VELOCITY)•Define the contact(*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE)Set up the problem•Set up the output requests and problem control cardsUnitsUnits used in this model are as follows:Time Milliseconds (ms)Length Millimeters (mm)Force Kilonewtons (kN)Mass Kilograms (kg)Altair Engineering, Inc. Using Altair HyperMesh to interface with LS-DYNA Page 3Chapter 1: Crashing TubesExercise 1: Prepare for ModelingIn this step, open a HyperMesh file containing the model geometry, then create the material, section, and part definitions required to set up the model.Dyna keyword card organizationIn LS-DYNA the model geometry information (nodes and elements) is organized by the *PART card. The *PART card corresponds to a component within HyperMesh. Within the *PART card, references are made to a*SECTION_SHELL and a *MAT card to define the section and material properties.In HyperMesh, the *PART, *SECTION and *MAT cards are assigned to database entities called Collectors. Because of the relationships required between the Dyna keywords, the order in which HyperMesh collectors are created becomes important. To avoid further editing and updating of the model, the material(*MAT) and property (*SECTION) collectors need to be created before components (*PART).Retrieve a HyperMesh binary database:1. Select the files panel.2. Select the hm file subpanel.3. Click retrieve… and select tubes.hm.4. Click Open to close the file browser and load the model into HyperMesh.5. Click return to exit the files panel and go back to the main menu. Comments: The model file retrieved consists of two tubes. The blue tube will be the designated target and the nodes at its extremities will be fully fixed. The red tube will be given an initial velocity in the positive X direction and will impact the blue tube.Page 4 Using Altair HyperMesh to interface with LS-DYNA Altair Engineering, Inc.Chapter 1: Crashing TubesExercise 2: Creating material collectorsIn this section, create a material definition card for the tubes, material type 24 (*MAT_PIECEWISE_LINEAR_PLASTICITY).Comments: This material offers different possibilities to define the effective stress versus effective plastic strain. HyperMesh fully supports all these approaches. The user can describe the material’s data by typing the values directly in the material card, select a *DEFINE_TABLE or, as described in this example, can select an LCSS ID to specify the curve for material behavior. Import of a curveThe creation of the material requires a curve containing the stress versus plastic strain information. We import this curve using the xy plots / read curves panel located on the Post page. In HyperMesh, curves are stored and organized in xy plots. If no xy plots exist when a curve is created, a xy plot will be created automatically.1. Enter the xy plots panel in the Post page2. Optionally select the plots panel and create a xy plot where to store thecurve.3. Select the read curves panel.4. Click the browse… button and select the file named curve.txt.5. Click Open to complete the selection in the file browser.6. Click input to read the curve.7. Click return, click exit.HyperMesh is able to import curve data in a comma delimited ASCII format. Multiple curves can be defined in the same file, with each curve defined in it’s own block. Each block starts with an XYDATA statement and ends with the ENDDATA statement. Within the curve block, each data point has it’s own line, and is simply the x value, a comma separator, and the y value, as shown in the example below.Altair Engineering Using the LS_DYNA Interface with Altair HyperMesh Page 5Chapter 1: Crashing TubesXYDATA,2.000e-03,2.300e-01……2.300e-01,2.800e-01ENDATADefine Mat Type 24 (*MAT_PIECEWISE_LINEAR_PLASTICITY): This material is used by the shell elements representing the tubes8. Enter the collectors panel and select the create subpanel9. Click the switch corresponding to the collector type and select mats fromthe pop up menu.10. Click name = and enter steel.11. Click card image = and select MATL24.12. Click create/edit.13. Click [Rho] to activate the data entry field and enter 7.8E-9 Kg/ mm3.14. Click [E] and enter 210 KN/mm2.15. Click [Nu] and enter 0.3 for Poisson’s ratio.16. Click [SIGY] and enter 0.2 for the yield stress.17. Double click [LCSS] and select the curve1.18. Click return to exit the card editor and go back to the collectors panel. Page 6 Using Altair HyperMesh to interface with LS-DYNA Altair Engineering, Inc.Exercise 3: Define the section cards for thecomponentsIn this step, create the *SECTION_SHELL card to specify the shell element thickness. For simplicity, all of the elements will be specified as being 1.5 mm thick.1. In the create subpanel of the collectors panel, set the collector type toprops.2. Click name = and enter section 1.5.3. Click the switch under creation method and select card image.4. Click card image and select SectShll.5. In the material= field, select steel6. Click create/edit.7. Click [T1] and enter 1.5. This specifies the shell thickness.8. Click return to exit the card editor.Comments: In LS-Dyna the material reference for the elements is defined on the *PART card, for this reason the user does not have to select any material when a property is created. On the other hand, in order to support other solvers HyperMesh must create a reference between any property collector and a material; therefore, if the field material= is left blank at the moment of the property creation, HyperMesh will add a dummy material so that this reference can be established. This dummy material will not create any problem to the Dyna run but its deletion is suggested. In the process of creating a property, the user can enter one of the existing materials to make this reference. This will prevent HyperMesh from creating a dummy material, which will need to be deleted later. Update the components to use the new materialIn this section, update the components to specify the material used. For both of the tube components, use the steel material.9. Enter the collectors panel and select the update subpanel10. Click the switch corresponding to the collector type and select compsfrom the pop up menu.11. Click the yellow comps selector and check both of the tube components.12. Click select to complete the selection and return to the collectors panel.13. Click in the material field and select steel14. Click update15. Check the material id checkbox.16. Click update. A confirmation message will appear in the header barindicating that the component collectors have been updated.Load the *PART card for the existing components and specify the section card to be usedIn this step, the *PART card will be created for each of the components in the model. On each of the *PART cards, the section id will be defined.17. Select the card image sub panel.18. Set the collector type to comps.19. Click in the name field and select the fixed tube component.20. Click in the card image field and select Part.21. Click load / edit.22. Optionally enter a comment string to describe this Part.23. Activate the sid selector and choose the section 1.5.24. Click return to exit the card editor and go back to the collectors panel.Repeat this procedure to load the *PART card image and specify thesection for the moving tube component.Exercise 4: Define the boundary conditionsIn this step, define the boundary conditions for the tube model. This includes defining initial velocity, constraints and contact.Applying the velocity (*INITIAL_VELOCITY)Apply a velocity of 30 mm/ms to the moving tube component.The initial velocity can be defined in different ways in LS-DYNA:•To apply velocity to a component (*PART) or to a set of components (*SET_PART_LIST) use the card *INITIAL_VELOCITY_GENERATION.This card is created in HyperMesh using the loadcols panel.•To apply velocity to a set of nodes (*SET_NODE_LIST) use the card *INITIAL_VELOCITY. Also this card is created in HyperMesh using theloadcols panel.•To apply velocity to individual nodes use the card*INITIAL_VELOCITY_NODE. This card is created in HyperMesh using the velocity panel in the BC’s page.In this exercise create a set containing all the nodes in the moving tube and then apply the *INITIAL_VELOCITY using the set of nodes.Defining a set of nodes1. Select the entity sets panel in the BCs page.2. Enter nodes for velocity in the name field.3. Set the entity selector in the middle of the panel to nodes.4. Click on the yellow nodes selector and choose by collectors from thepop up menu.5. Check moving tube and click select.6. Click create to create the *SET_NODE_LIST.7. Click return.Defining the initial velocity8. Enter the collectors panel and select the create subpanel.9. Set the collector type to loadcols.10. Enter init_vel for the name =.11. Select the InitialVel card image12. Click create/edit.13. Activate the [NSID] field, then click the yellow NSID button in the cardpreview image and select the nodes for velocity set.14. Set the initial velocity to 30 mm/ms by entering 30 in the VX field.15. Click return to exit the card editor and go back to the collectors panel. Defining the constraints (*BOUNDARY_SPC_NODE)Define the constraints for the free ends of the fixed tube component. The nodes will be fixed in all six degrees of freedom. A predefined set of nodes is already available under the name of nodes for SPC.Start by creating a load collector. At this point, you should still be in the collectors panel.16. Select the create subpanel17. Set the collector type to loadcols.18. Enter SPC in the name field19. Set the creation method to no card image.20. Optionally pick a color for the load collector.21. Click create.22. Click return to exit the collectors panel and go back to the main menu. Set the HyperMesh Constraint Configuration to*BOUNDARY_SPC_NODEEntities created in HyperMesh can often be used to define more than one type of Dyna entity. For example the constraints panel in HyperMesh can create both *BOUNDARY_SPC_NODE and *BOUNDARY_PRESCRIBED_MOTION_NODE cards. To ensure that the correct information for the specific Dyna entity is defined for the model, the entity type should be specified before the entity’s creation.For entities created using panels on the BCs page use the load types panel to specify the correct type; for entities created using panels in 1D, 2D, 3D use the elem types panel.23. Select the Load Types panel on the BCs page.24. Click on constraint and select BoundSPC from the pop up menu.25. Click return.Creating the constraints26. Select to the constraints panel on the BCs page.27. Click on the yellow nodes selector and choose by sets from the pop upmenu.28. Select the nodes for SPC set and click select. This will return you to theconstraints panel. The nodes at the free ends should be highlighted.29. Check all 6 dof (degrees of freedom) checkboxes.30. Click create. The constraints have been created for each of the selectednodes.31. Click return to go back to the main menu.Exercise 5: Defining the Contact between thetubesIn this step, define the contact between the two tubes using*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE. The moving tube will be the master surface, and the fixed tube will be the slave surface.In LS-DYNA the selection of master and slave entities defining the contact is very flexible. For example the *CONTACT_SURFACE_TO_SURFACE can be defined using one of these options: segment set, shell element set, part set, part, node set, or using the entire model.In this exercise we use the selection *SET_SEGMENT for both master and slave.The panel contactsurf has been introduced in HyperMesh to efficiently support the *SET_SEGMENT card. The user can now create, update and renumber set segments as well as change their orientation. (The set segment orientation can be different from the element normal orientation).A set segment can be created also to treat contacts between solids faces or beams. The graphic representation of the contact surf is a pyramid whose orientation reflects the set segment orientation.Defining the slave surface for the contact (*SET_SEGMENT)1. Go to the set_segment panel on the BCs page.2. Select the elems subpanel.3. Enter slave for name =4. Select the setSegment card image5. Optionally select a color for the contactsurf6. Click on the yellow elems selector and choose by collector from the popup menu.7. Select the fixed tube and click select8. Click create.Zoom in the model to better visualize the graphic representation of the contactsurf entity. Over each element there is now a pyramid that in this case is pointing out. By default, the orientation of the contact surf is the same as the normal of the element underneath.Defining the master surface for the contact (*SET_SEGMENT) At his point, you should still be in the contactsurfs / elems panel.9. Enter master for name =10. Select the setSegment card image11. Optionally select a color for the contactsurf12. Click on the yellow elems selector and choose by collector from the popup menu.13. Check moving tube and click select.14. Click create.15. Click return to go back to the main menu.Defining contact(*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE)16. Go to the interfaces panel on the BCs page.17. Select the create sub panel.18. Enter contact for the name19. Click in the type field and select SurfaceToSurface20. Click create.21. Select the add subpanel22. Set the master entity type to csurfs and select master using the yellowcontactsurfs selector.23. Click update on the master line to define the master contact surface.24. Set the slave entity type to csurfs and select slave using the yellowcontactsurfs selector. Be sure to select update for the slave line to finish the definition.25. Select the card image subpanel and click edit.26. Click the switch below options and select Automatic.27. Click return to exit the card editor.28. Click return to go back to the main menu.Exercise 6: Setting up the analysis runControl Cards definitionThe control cards panel allows you to set solver specific data such as defining the termination time, the output frequencies for results, and other control options for the run.1. Select the control cards panel on the BCs pageDefine the Termination (*CONTROL_TERMINATION)2. Click Termination in the control cards panel.3. Click ENDTIM and enter 1.5 as termination time for the analysis.4. Click return.Define the Dbase Opts (Control Cards for Ascii Output)5. Click Dbase Opts.The Dbase Opts card is on the second page of control cards. Click thegreen next button on the right side of the panel to access it.6. Enter the value 0.1 as time interval between outputs for:GLSTAT (*DATABASE_GLSTAT)MATSUM (*DATABASE_MATSUM)SPCFORCE (*DATABASE_SPCFORCE7. Click return.Define the DB Bin PLOT (*DATABASE_BINARY_PLOT)8. Click DB Bin PLOT.9. Enter the value 0.1 in the field DT as the time interval between outputs forthe binary d3plot results files.10. Click return.11. Click return once more to go back to the main menu.Exercise 7: Export the Dyna Deck and running theanalysis1. Select files from the main menu.2. Select the export sub-panel.3. Make sure that the template field still shows the dyna.key file.4. Click write as… to bring up the file browser and enter the name of the LS-DYNA file you will create: tubes.key5. Click Save. HyperMesh writes the deck, and it displays a message once itis complete.6. Click return to access the main menu.Use the LS-DYNA manager program from the PC’s start menu to run the analysis.From the solvers menu, select Start LS-DYNA analysis, then browse for the tubes.key input file. Once it is loaded, click OK to start the analysis.Chapter 2: Post-Processing using HyperViewThis section provides an introduction to the HyperView interface and aims to make you comfortable using some of its basic features for post processingLS-DYNA d3plot files. This section covers:•The use of the HyperView interface•The use of the mouse•The use of the page and window control features•The use of the view options and controls•Loading a d3plot file into HyperView•Animating transient analysis results from the tubes analysis.•Displaying results contours.•Creating a measure plot from the results animationThe HyperView Screen DisplayThe image on the next page shows the initial screen display when HyperView starts. The screen display is divided into the following areas: the Menu contains several menu options each with its own drop-down menu allowing you to perform general functions such as opening text files, managing pages, handling graphics, and using the various tools that accompany HyperView; the graphics/text display area is where models, plots, and animations display; on the left side of the tool bar is the client selector where you can select one of four client types; the remaining controls access the various tools available for the selected client; the panel area is where the options for the various tools of each client display; and the view controls contains tools to control the orientation of the display. The following sections discuss each of these areas.Altair Engineering, Inc. Using Altair HyperMesh to interface with LS-DYNA Page 17Chapter 2: Post-Processing using HyperViewPage 18 Using Altair HyperMesh to interface with LS-DYNA Altair Engineering, Inc.The HyperView environment includes four data clients . Select the client you wish to use from the list in the Data client drop down menu . Data clients allow the visualization of different types of engineering data from many differentsources. These are the four data clients with a description of the files each type can process:Animation Client : Displays CAE model and analysis results information fromsupported CAE solvers for finite element, kinematic, andmultibody analysis. Additional solver formats are supportedvia translators that convert solver results to Altair's compactH3D binary format.XY PlottingClient : A powerful data analysis tool that interfaces with many popular file formats. The sophisticated math engine iscapable of processing complex mathematical expressionswith large data sets. Altair's Templex text and numericprocessor allows the introduction of advanced annotationsand notes.Video Client :Displays and synchronizes digital video data to CAE andXY Plot information. AVI, BMP, TIFF and JPEG file formats are supported. Tool bar PanelareaViewcontrolsMenuGraphics/textdisplay areaData clientdrop downmenuselectorChapter 2: Post-Processing using HyperViewAltair Engineering Using the LS_DYNA Interface with Altair HyperMesh Page 19Text Client : Allows text files to be viewed and edited directly in theHyperView environment. Altair's Templex language can beused to embed mathematical functionality.A file in HyperView can comprise multiple pages. Each page can hold one or more windows with each window holding one type of datum. Multi-window files may have all four clients represented.The HyperView MenuThe menu across the top of the HyperView screen display consists of PC-style drop down menus. The top level menu choices vary, according to the active data client.To see the choices for each client, from the Tool bar click the Client selection arrow to activate the drop down menu, then select the desired client. Or click in the display on the window of your choice. Active windows have a highlighted border.Some menus are common to all clients (File , Edit View , Page , Study and Help ). File Perform file operations pertaining to the HyperView session. Open andsave session files, set preferences, export curve and animation data,print functions, etc.Session files are used to save the entire HyperView session – allpages and window layouts. Load the data files for the individualclients using the client’s tool bar file functions. EditCut and paste operations for windows and pages. View Options affecting the overall layout of the HyperView session. Turn on or off common components, like the status bar at the bottom of the screen display, full screen mode, session browser, large icon mode,animation mini bar, or expand an active window to fill the graphicsarea.Page Page functions control the window layout, cycle through the pages, titledisplay and animation controls. The page functions are duplicated onthe right side of the tool bar.StudyThe Study menu is used to launch the Altair HyperStudy, a tool forparametric and optimization studies based on Design of Experiments(DOE)Chapter 2: Post-Processing using HyperViewPage 20 Using Altair HyperMesh to interface with LS-DYNA Altair Engineering, Inc.Help Launch the online help and review message logs.Client specific function menus are typically duplicated on the left side of the Tool bar. The following briefly describes the function menus for each of the clients. Animation Client function menusGraphics All of the panels and functions for the animation client can beaccessed here as well as on the left side of the tool bar. In addition,the current model properties can be used to review statistical andgeneral model information.Tools Start Custom Wizards, generate report templates, create customTemplex functions and control animation client options.Plotting client function menusPlotOptions affecting the look of the plotting client window, such as headers and footers, background colors, legends and notes. CurveOptions affecting the individual data curves, such as curve attributes, scales, etc. Tools Statistical and reporting functions for the curve data.Video and Text Editor clientsThe Video and Text Editor clients each have a single function menu.Video Control the appearrence of the video client window with headers andfooters, create notes and measures, or activate the filmstrip displaymode.TextEditorSearch text, control text attributes or edit text. Exercise 1: Open a d3plot fileThis exercise discusses the procedure to open D3Plot file in the HyperView animation client.1. Start HyperView using the shortcut in your working directory. Theanimation client is the default.。
