Defining ABAQUS Contacts for 3-D Models in HyperMesh - HM-4320

Transcription

1 Defining ABAQUS Contacts for 3-D Models in HyperMesh - HM-4320 For this tutorial it is recommended that you complete the introductory tutorial, Getting Started with HyperMesh - HM This tutorial explains how to use the ABAQUS Contact Manager for 3D models. The following exercises are included: Loading ABAQUS user profile and model Starting Abaqus Contact Manager Defining surfaces for solid elements Defining surfaces for shell elements Defining surfaces by set Defining surface interaction property Defining contact pair All files referenced in the HyperMesh tutorials are located in the < install_directory>/tutorials/hm/ directory. For detailed instructions on how to locate the installation directory <install_directory> at your site, see Finding the Installation Directory <install_directory>, or contact your system administrator. Loading ABAQUS User Profile and Model A set of standard user profiles is included in the HyperMesh installation. They include LSDYNA, NASTRAN, ABAQUS, ANSYS, OptiStruct, moldflow, MADYMO, and HyperMesh. While the user profiles change the appearance of some panels, they do not affect the internal behavior of each function. To load the ABAQUS user profile: 1. From the Geom page click the user prof. button. 2. Select Abaqus as the profile name and click OK. 3. Select Standard3D as template name and click OK. 4. Select the files panel. 5. Select the hm file subpanel. 6. Click retrieve and select <install_directory>/tutorials/hm/abaqus_contactmanager_3d_tutorial.hm. 7. Click Open. To start Contact Manager: 1. Load the ABAQUS user profile. 2. Click the Contact Manager button in the Abaqus Macro menu. This opens the Abaqus Contact Manager dialog.

2 3. Move the dialog window to the bottom-left corner of HyperMesh window and resize it to your liking. Defining Surfaces for Solid Elements In HyperMesh, you can define the *SURFACE, TYPE=ELEMENT card by using individual element IDs or sets with corresponding face identifiers. In this exercise, you will create surfaces by defining individual element IDs and corresponding faces. To create the "box1-top" surface: 1. Select the Surface tab in the Abaqus Contact Manager dialog. This opens the Create New Surface dialog. 3. Type box1-top in the Name: entry box. 4. Select Element based as the type of surface. 5. Click Color: button and select color Click Create button. This opens the Element Based Surface dialog for defining elements and corresponding faces for the surface. 7. Select the display panel from the permanent menu. 8. Click the upper switch and select comps. 9. Click the toggle to elems. 10. Use the right mouse button to deselect all components except BOX_ Click return to exit the panel. 12. Select the view panel from the permanent menu and select top from the pop-up menu. 13. Restore the Element Based Surface dialog (click the Contact Manager button or the icon in the task bar). 14. Select the Define tab in the Element Based Surface dialog. 15. Select 3D solid, gasket option from the Define surface for: radio buttons. 16. Click the Elements button. This opens the HyperMesh element selector panel. 17. Click the elems button. 18. Select by collector. 19. Check the BOX_1 component and click select. You will see the elements in BOX_1 component highlighted. 20. Click proceed to return to the Element Based Surface dialog. 21. Select Solid skin option from the Select faces by: radio buttons. 22. Select a color from the Solid skin color: button. 23. Click the Faces button. This creates a temporary skin of the selected elements and opens the HyperMesh element

3 selector panel. 24. Select an element from the top of the solid skin. 25. Click the elems button and select by face. You will see all faces at the top of the solid skin are highlighted. 26. Rotate the model in HyperMesh interface to verify all desired faces are selected. You can deselect any element (by right clicking) or add more if you like. 27. When you are satisfied with the element faces selected, click proceed to return to the Element Based Surface dialog. 28. Click the Add button to add these faces to the current surface. This creates special "face" elements (rectangles with dot in the middle) for display. You can reject the recently added "faces" by clicking the Reject button. You can also delete "faces" from the Delete Face page. 29. When satisfied with the surface definition, click Close to return to the Abaqus Contact Manager dialog. To create the "box2-top" surface: 1. Select the Surface tab in the Abaqus Contact Manager dialog and click the Display None button to undisplay all surfaces. This opens the Create New Surface dialog. 3. Type box2-top in the Name: entry box. 4. Select Element based as the type of surface. 5. Click Color: button and select color Click Create button. This opens the Element Based Surface dialog for defining elements and corresponding faces for the surface. 7. Select the display panel from the permanent menu. 8. Click the upper switch and select comps. 9. Click the toggle to elems. 10. Use the right mouse button to deselect all components except BOX_ Click return to exit the panel. 12. Select the view panel from the permanent menu and select top from the pop-up menu. 13. Restore the Element Based Surface dialog (by clicking the Contact Manager button or the icon on the task bar). 14. Select the Define tab on the Element Based Surface dialog. 15. Select 3D solid, gasket option from the Define surface for: radio buttons. 16. Click the Elements button. This opens the HyperMesh element selector panel. 17. Click the elems button, select by collector, check the BOX_2 component and click select. You will see the elements in BOX_2 component highlighted.

4 18. Click proceed to return to the Element Based Surface dialog. 19. Select Nodes on face option from the Select faces by: radio buttons. 20. Click the Nodes button to open the HyperMesh node selector panel. 21. Select two corner nodes (or three nodes) from the top of the selected solids as shown below. 22. Click proceed to return to the Element Based Surface dialog. 23. Write down at the Break Angle entry box. 24. Click the Add button to find all faces of the selected solids that fall within the break angle of the face defined by nodes. It adds these faces to the current surface and creates special "face" elements (rectangles with dot at the middle) for display. You can reject the recently added "faces" by clicking the Reject button. You can also delete "faces" from the Delete Face page. 25. When satisfied with the surface definition, click Close to return to the Abaqus Contact Manager dialog. To create the "cylinder-top" surface: 1. Select the Surface tab in the Abaqus Contact Manager dialog and click the Display None button to undisplay all surfaces. This opens the Create New Surface dialog. 3. Type cylinder-top in the Name: entry box. 4. Select Element based as the type of surface. 5. Click Color: button and select color Click Create button. This opens the Element Based Surface dialog for defining elements and corresponding faces for the surface. 7. Select the display panel from the permanent menu. 8. Click the upper switch and select comps. 9. Click the toggle to elems. 10. Use the right mouse button to deselect all components TOP_CYLINDER. 11. Click return to exit the panel. 12. Click the f button on the permanent menu. 13. Restore the Element Based Surface dialog (by clicking the Contact Manager button or the icon in the task bar.)

5 14. Select the Define tab in the Element Based Surface dialog. 15. Select 3D solid, gasket option from the Define surface for: radio buttons. 16. Click the Elements button. This opens the HyperMesh element selector panel. 17. Click the elems button, select by collector, check TOP_CYLINDER component and click select. This highlights the elements in TOP_CYLINDER component. 18. Click proceed to return to the Element Based Surface dialog. 19. Select Solid skin option from the Select faces by: radio buttons. 20. Select a color from the Solid skin color: button 21. Click the Faces button. This creates a temporary skin of the selected elements and open the HyperMesh element selector panel. 22. Select an element from the solid skin, click the elems button, select by face. You will see faces all around the solid skin are highlighted. 23. Rotate the model in the HyperMesh interface to verify all desired faces are selected. You can deselect any element (by right clicking) or add more if you like. 24. When you are satisfied with the element faces selected, click proceed to come back to the Element Based Surface dialog. 25. Click the Add button to add these faces to the current surface. This creates special "face" elements (rectangles with dot at the middle) for display. You can reject the recently added "faces" by clicking the Reject button. You can also delete "faces" from the Delete Face page. 26. When satisfied with the surface definition, click Close to return to the Abaqus Contact Manager dialog. Defining Surfaces for Shell Elements In HyperMesh, you can define the *SURFACE, TYPE=ELEMENT card by using individual shell element IDs or sets with corresponding SPOS/SNEG face identifiers. In this exercise, you will create surfaces by defining individual element IDs and corresponding normals to define the SPOS/SNEG faces. To create the "cylinder-bot" surface: 1. Select the Surface tab in the Abaqus Contact Manager dialog and click the Display None button to undisplay all surfaces. This opens the Create New Surface dialog. 3. Type"cylinder-bot in the Name: entry box. 4. Select Element based as the type of surface. 5. Click Color: button and select color Click Create button.

6 This opens the Element Based Surface dialog for defining elements and corresponding faces for the surface. 7. Select the Define tab in the Element Based Surface dialog. 8. Select 3D shell, membrane, rigid option from the Define surface for: radio buttons. 9. Select the display panel from the permanent menu. 10. Click the upper switch and select comps. 11. Click the toggle to elems. 12. Use the right mouse button to deselect all components except BOT_CYLINDER. 13. Click return to exit the panel. 14. Click the f button on the permanent menu. 15. Restore the Element Based Surface dialog (by clicking the Contact Manager button or the icon in the task bar). 16. Click the Elements button. This opens the HyperMesh element selector panel. 17. Click the elems button, select by collector, check BOT_CYLINDER component and click select. You will see the elements in BOT_CYLINDER component highlighted. 18. Click proceed to return to the Element Based Surface window. 19. The normals of the selected elements will be displayed at this point. If the normals are too big, click Reset, go to the view panel from the permanent menu and select front from the pop-up menu. Restore the Element Based Surface dialog and repeat steps You'll notice that all normals are pointing inwards. 20. Check the Reverse option. 21. Click the Add button to add these faces to the current surface. It will create special "face" elements (rectangles with dot at the middle) for display. You can reject the recently added "faces" by clicking the Reject button. You can also delete "faces" from the Delete Face page 22. Go to the Adjust Normal page and select Display normals option. The normals of all the "faces" in the current surface will be displayed. You'll notice that all normals are pointing outwards. 23. When satisfied with the surface definition, click Close to go back to the Abaqus Contact Manager dialog. Defining Surfaces by Set In HyperMesh, you can define the *SURFACE, TYPE=ELEMENT card by using individual element IDs or sets with corresponding face identifiers. In this exercise, you will create surfaces by defining a set and corresponding face identifiers. HyperMesh allows only one set in a surface. It also does not support combination of sets and individual elements in the same *SURFACE data line. To create the "box1-bot" surface: 1. Select the Surface tab in the Abaqus Contact Manager dialog and click the Display None button to undisplay all surfaces.

7 This opens the Create New Surface dialog. 3. Type box1-bot in the Name: entry box. 4. Select Element based as the type of surface. 5. Click Color: button and select color Click Create button. This opens the Element Based Surface dialog for defining elements and corresponding faces for the surface. 7. Select the Define tab in the Element Based Surface dialog. 8. Select Element set option from the Define surface for: radio buttons. 9. Select the display panel from the permanent menu. 10. Click the upper switch and select comps. 11. Click the toggle to elems. 12. Use the right mouse button to deselect all components except BOX_ Click return to exit the panel. 14. Go to the view panel from the permanent menu and select bottom from the pop-up menu. 15. Restore the Element Based Surface dialog (by clicking the Contact Manager button or the icon in the task bar). 16. Click the Element set: entry box and select box1-bot from the list of existing sets. 17. Click the Review Set button to highlight all the elements in the selected set. 18. Right click the Review Set button to reset the highlighting. 19. Click the Show Faces button. This creates a temporary skin of the selected element set and open the HyperMesh element selector panel. 20. Select an element from the bottom of the solid skin, click the elems button, select by face. You will see all faces at the bottom of the solid skin are highlighted. You can deselect any element (by right clicking) or add more if you like. 21. When you are satisfied with the element faces selected, click proceed to return to the Element Based Surface dialog. The face identifier tags (color coded) of the selected faces are displayed at this point. In performance graphics, the solid mesh sometimes blocks these tags. You might have to rotate the model a little to make these tags visible or switch to Standard graphics. Since all face identifiers tags for the bottom side of the box1-bot set are S3, you can use the S3 identifier for this set. 22. Click the Face: button and select S3 from the pull down menu. 23. Check the Display option and click the Update button. This adds the selected set and face identifier to the current surface. In addition, it creates a special display for the surface. NOTE: HyperMesh, by default, does not create any display for surfaces defined with sets. However, if you check the Display option before clicking Update, it will create a special display using contactsurface elements. The special display does not have any link to the set in HyperMesh database. Therefore, if you edit the set later on, the display would not reflect them automatically. In this case, you need to come to this page, check the Display option and click

8 Update button again. 24. Click Close to return to the Abaqus Contact Manager dialog. To create the "box2-bot" surface: 1. Select the Surface tab in the Abaqus Contact Manager dialog and click the Display None button to undisplay all surfaces. This opens the "Create New Surface" window. 3. Type box2-bot in the Name: entry box. 4. Select Element based as the type of surface. 5. Click Color: button and select color Click Create button. This opens the Element Based Surface dialog for defining elements and corresponding faces for the surface. 7. Select the Define tab in the Element Based Surface dialog. 8. Select Element set option from the Define surface for: radio buttons. 9. Select the display panel from the permanent menu. 10. Click the upper switch and select comps. 11. Click the toggle to elems. 12. Use the right mouse button to deselect all components except BOX_ Click return to exit the panel. 14. Go to the view panel from the permanent menu and select bottom from the pop-up menu. 15. Restore the Element Based Surface dialog (by clicking the Contact Manager button or the icon at the task bar). 16. Click the Create/Edit Sets button to opens the entity sets panel in HyperMesh. 17. Type box2-bot in the name = entry box, select elems option from upper switch, select all elements from the bottom of BOX_2 component and click create. 18. When you are done creating/editing the set, click return. The Element Based Surface dialog returns with the new set appearing in element set list. 19. Click the Element set: entry box and select box2-bot from the list of existing sets. 20. Click on the Review Set button to highlight all the elements in the selected set. 21. Right mouse click the Review Set button to reset the highlighting. 22. Click the Show Faces button. This creates a temporary skin of the selected element set and opens the HyperMesh element selector panel. 23. Select an element from the bottom of the solid skin, click the elems button, select "by face". You will see all faces at the bottom of the solid skin are highlighted. You can deselect any element (by right clicking) or add more if you like. 24. When you are satisfied with the element faces selected, click proceed to come back to the Element Based Surface dialog. The face identifier tags (color coded) of the selected faces display at this point. In performance

9 graphics, the solid mesh sometimes blocks these tags. You might have to rotate the model a little to make these tags visible or switch to Standard graphics. Since all face identifiers tags for the bottom side of the box1-bot set are S3, you can use the S3 identifier for this set. 25. Click the Face: button and select S3 from the pull down menu. 26. Uncheck the Display option, if checked and click the Update button to add the selected set and face identifier to the current surface. NOTE: HyperMesh, by default, does not create any display for surfaces defined with sets. 27. Click Close to return to the Abaqus Contact Manager dialog. You'll notice in the Surface: table that the Display options for the box2-bot surface is disabled. At this point, you have created all the surfaces required. 28. Click the Display All button to display all surfaces. Select the display panel from the permanent menu, select comps and click all. Go to the new panel from the permanent menu and select iso1 from the pop-up menu. You can review any surface by selecting from the table and clicking Review button. The selected surface will be highlighted with white and show up through solid mesh in performance graphics. If the surface is defined with sets (display option disabled), the underlying elements are highlighted. Right mouse click on all Review buttons to clear the highlighting. Defining Surface Interaction Property In this exercise, you will define the *SURFACE INTERACTION card with corresponding *FRICTION card.. To create the "friction1" surface interaction: 1. Select the Surface Interaction tab at the Abaqus Contact Manager dialog. This opens the Create New Surface Interaction dialog. 3. Type friction1 in the Name: entry box. 4. Click Create button. This opens the Surface Interaction dialog. 5. Select the Define page in the Surface Interaction dialog. 6. Select Friction option as surface interaction property. That makes the Friction tab active. 7. Select the Friction tab. 8. Select Default as the Friction type: and Direct option as friction co-efficient definition method. Selecting this option means that the Exponential decay and Anisotropic parameters will not be written to the input file. 9. Enter 1 at the No of data lines entry box and click set. A single row appears in the Direct table. 10. Click the first cell on the Friction Coeff column and enter NOTE for Direct and Anisotropic tables:

10 The column numbers in the table will change with the No of Dependencies selected. The row numbers can be defined at the No of data lines entry box. Clicking the corresponding Set button will update the table to have the specified number of rows For placing values in the table, click a cell to make it active and type in the values. The table works like a regular spreadsheet You can also read comma-delimited data from a text file by clicking the Read From a File button. This button opens up a file browser window. Select the file and click Open to export the comma-delimited data. The row number will be set to the number of data lines found in the file Clicking the right mouse button (Button-3) in the table shows a pull down menu with copy, cut and paste options. Comma-separated data can be copied/cut into or pasted from clipboard with these options. Relevant hot keys (for example, CTRL-C, CTRL-X and CTRL-V in Windows) will also work. Clicking the left mouse button (Button-1) in a cell activates that cell. Clicking into an already active cell moves the insertion cursor to the character nearest the mouse. Moving the mouse while the left mouse button (Button-1) is pressed strokes out a selection area. The left, right, up and down arrows move the active cell SHIFT-<arrow> extends the selection in that direction. CTRL-left arrow and CTRL right arrow move the insertion cursor within the cell. CTRL -slash selects all the cells. BACK SPACE deletes the character before the insertion cursor in the active cell. If multiple cells are selected, BACK SPACE deletes all selected cells. DELETE deletes the character after the insertion cursor in the active cell. If multiple cells are selected, DELETE deletes all selected cells. CTRL -A moves the insertion cursor to the beginning of the active cell. CTRL-E moves the insertion cursor to the end of the active cell. CTRL minus (-) and CTRL equal (=) decrease and increase the width of the column with the active cell in it. To interactively resize a row or column, move the mouse over the border while Button-1 or Button-3 (the right button on Windows) is pressed. 11. Click OK to go back to the Abaqus Contact Manager dialog. Defining Contact Pair In this exercise, you will define the *CONTACT PAIR card with corresponding surfaces and surface interaction. To create the "top-cylinder-box1" contact pair:

11 1. Go to the Interface page at the Abaqus Contact Manager dialog. This opens the Create New Interface dialog. 3. Type top-cylinder-box1 in the Name: entry box. 4. Select Contact pair as the type of interface. 5. Click Create button. This opens the Contact Pair dialog. 6. Select the Define tab in the Contact Pair dialog. 7. Click the Select slave surface: entry box to show a list of the existing surfaces. 8. Select box1-top from the list as the slave surface. 9. Click the corresponding Review button. The selected surface is highlighted with white and shows up through solid mesh in performance graphics. If the surface is defined with sets (display option disabled), the underlying elements are highlighted. Right mouse click on all Review buttons to clear the highlighting. NOTE: The corresponding Create New button opens the Create New Surface dialog for creating a new surface. When you are done creating and defining the surface, the Contact Pair window returns with the new surface selected as the slave surface. 10. Follow step 7 and 8 using the Select master surface: to select the cylinder-top as the master surface. 11. Click the Select surface interaction: entry box to show a list of the existing surface interactions. 12. Select friction1 from the list as the interaction property for the current contact pair. 13. Select the Parameter tab in the Contact Pair dialog. 14. Select SmallSliding from the available options. 15. Click OK to return to the Abaqus Contact Manager dialog. To create the "top-cylinder-box2" contact pair: Follow step 1 through 15 above to define the top-cylinder-box2 contact pair with box2-top as slave surface, cylinder-top as master and friction1 as the surface interaction. To create the "bot-cylinder-box1" contact pair: Follow step 1 through 15 above to define the bot-cylinder-box1 contact pair with box1-bot as slave surface, cylinder-bot as master and friction1 as the surface interaction. To create the "bot-cylinder-box2" contact pair: Follow steps 1 through 15 above to define the bot-cylinder-box2 contact pair with box2-bot as slave surface, cylinder-bot as master and friction1 as the surface interaction. At this point, you have created all the contact pairs required. You can review any contact pair by selecting from the table and clicking Review button. Both the master and slave surface will be highlighted highlighted with white color and show up through solid mesh in performance graphics. If a surface is defined with sets (display option disabled), the underlying elements are highlighted. Right mouse click on all Review button will clear the highlighting. 1. Click the Close button to close the Abaqus Contact Manager window.

12 General comments: The Edit... button opens the corresponding window for editing the selected interface, surface or surface interaction The Review button reviews the selected interface, surface and surface interaction as follows: For surface, it highlights the selected surface in HyperMesh window. The surfaces are highlighted with white and show up through solid mesh in performance graphics. If the surface is defined with sets (display option disabled), the underlying elements are highlighted in HyperMesh window. For interface, it highlights corresponding slave and master surfaces together in HyperMesh window. The surfaces are highlighted in the same fashion as mentioned above. For surface interaction, it highlights the names of all interfaces using the selected surface interaction in the Interface table. There is no graphical review for surface interaction. The Delete button deletes the selected interfaces, surfaces or surface interactions. This button accepts multiple selections from the Interface table. The Sync button updates the Contact Manager with the current HyperMesh database. If you create, update or delete any components, groups, properties or entity sets from HyperMesh panels while the Contact Manager is open, click the Sync button to update the Contact Manager with the changes If you minimize the Contact Manager dialog or it goes behind the HyperMesh window, clicking the Contact Manager button in the Abaqus Macro menu restores it. Bubble help exists for important buttons. Place the mouse on the buttons for a few moments to view it. Double clicking the interface, surface and surface interaction names in the table will open the corresponding edit windows. A Right mouse click on these names displays a pull down menu with options. Clicking a table border, pressing and holding the left or right mouse button and moving the mouse can resize columns in a table. Shift and Ctrl keys can be used with a left mouse click to select multiple items in a table (useful for deleting multiple items). See HyperMesh Tutorials for a complete list of tutorials.