HM-4320: Define Abaqus Contacts for 3D Models

In this step you will load the user profile and model.

1. Start HyperMesh Desktop.
2. In the User Profile dialog, set the user profile to Abaqus, Standard 3D.
3. Open a model file by clicking File > Open > Model from the menu bar, or by clicking on the Standard toolbar.
4. In the Open Model dialog, open the abaqus_contactManager_3D_tutorial.hm file.
   The model appears in the graphics area.

   
   
   Figure 1.

In this step you will start the contact browser.

From the menu bar, click Tools > Contact Browser. The Abaqus Contact Browser opens.

Figure 2.

In this step you will define surfaces for solid elements.

1. In the Abaqus Contact Manager, click the Surface tab.
2. Click New.
   The Create New Surface dialog opens.
3. In the Name field, type box1-top.
4. Set Type to Element based.
5. Click the box next to Color and select a color.
6. Click Create.
   The Element Based Surface dialog opens, from which you can define elements and corresponding faces for the surface.
7. In the Model Browser, Component folder, right-click on BOX_1 and select Isolate from the context menu.
8. On the Standard Views toolbar, click (XY Top Plane View).
9. In the Element Based Surface dialog, click the Define tab.
10. Set the Define surface for to 3D solid, gasket.
11. Click Elements.
12. In the panel area, click elems >> by collector.
13. Select the component, BOX_1.
14. Click select.
    The elements in the BOX_1 component highlight.

    
    
    Figure 3.

15. Click proceed to return to the Element Based Surface dialog.
16. Set Select faces by to Solid skin.
17. Select a color form the Solid skin color button.
18. Click Faces.
    HyperMesh creates a temporary skin of the selected elements.
19. Select an element from the top of the solid skin.
20. In the panel area, click elems >> by face.
    All faces at the top of the solid skin highlight.
21. Rotate the model to verify all desired faces are selected.
22. Optional: Deselect any element by right-clicking or add more if you like.
23. When you are satisfied with the element faces selected, click proceed to return to the Element Based Surface dialog.
24. Click Add to add these faces to the current surface.
    HyperMesh creates special face elements (rectangles with a dot in the middle) for display.

    
    
    Figure 4.

25. Optional: Reject the recently added faces by clicking Reject. You can also delete faces from the Delete page.
26. When satisfied with the surface definition, click Close to return to the Abaqus Contact Manager.

In this step you will create the box2-top surface.

1. In the Abaqus Contact Manager, click the Surface tab.
2. Click Display None to turn off the display of all surfaces.
3. Click New.
   The Create New Surface dialog opens.
4. In the Name field, type box2-top.
5. Set Type to Element based.
6. Click the box next to Color and select a color.
7. Click Create.
   The Element Based Surface dialog opens, from which you can define elements and corresponding faces for the surface.
8. In the Model Browser, Component folder, right-click on BOX_2 and select Isolate from the context menu.
9. On the Standard Views toolbar, click (XY Top Plane View).
10. In the Element Based Surface dialog, click the Define tab.
11. Set Define surface for to 3D solid, gasket.
12. Click Elements.
13. In the panel area, click elems >> by collector.
14. Select the component, BOX_2.
15. Click select.
    The elements in BOX_2 highlight.
16. Click proceed to return to the Element Based Surface dialog.
17. Set Select faces by to Nodes on face.
18. Click Nodes.
19. Select two corner nodes (or three nodes) from the top of the selected solids as shown below.

    
    
    Figure 5.

20. In the panel area, click proceed to return to the Element Based Surface dialog.
21. In the Break Angle field, type 30.00.
22. Click Add to find all faces of the selected solids that fall within the break angle of the face defined by nodes.
    HyperMesh adds these faces to the current surface and creates special face elements (rectangles with a dot in the middle) for display.

    
    
    Figure 6.

23. Optional: Reject the recently added faces by clicking Reject. You can also delete faces from the Delete page.
24. When satisfied with the surface definition, click Close to return to the Abaqus Contact Manager.

In this step you will create the cylinder-top surface.

1. In the Abaqus Contact Manager, click the Surface tab.
2. Click Display None to turn off the display of all surfaces.
3. Click New.
   The Create New Surface dialog opens.
4. In the Name field, type cylinder-top.
5. Set Type to Element based.
6. Click the Color button and select a color.
7. Click Create.
   The Element Based Surface dialog opens, from which you can define elements and corresponding faces for the surface.
8. In the Model Browser, Component folder, right-click on TOP_CYLINDER and select Isolate from the context menu.
9. In the Element Based Surface dialog, click the Define tab.
10. Set Define surface for to 3D solid, gasket.
11. Click Elements.
12. In the panel area, click elems >> by collector.
13. Select the component, TOP_CYLINDER.
14. Click select.
    Elements in the TOP_CYLINDER component highlight.
15. Click proceed to return to the Element Based Surface dialog.
16. Set Select faces by to Solid skin.
17. Select a color from the Solid skin color button.
18. Click Faces.
    HyperMesh creates a temporary skin of the selected elements.
19. Select an element from the solid skin.
20. In the panel area, click elems >> by face.
    The faces around the solid skin highlight.
21. Rotate the model to verify all desired faces are selected.
22. Optional: Deselect any element by right-clicking, or add more if you like.
23. When you are satisfied with the element faces selected, click proceed to return to the Element Based Surface dialog.
24. Click Add to add these faces to the current surface.
    HyperMesh creates special face elements (rectangles with a dot at the middle) for display.

    
    
    Figure 7.

25. Optional: Reject the recently added faces by clicking Reject. You can also delete faces from the Delete page.
26. When satisfied with the surface definition, click Close to return to the Abaqus Contact Manager.

In this step you will create surfaces by defining individual element IDs and corresponding normals to define the SPOS/SNEG faces.

1. In the Abaqus Contact Manager, click the Surface tab.
2. Click Display None to turn off the display of all surfaces.
3. Click New.
   The Create New Surface dialog opens.
4. In the Name field, type cylinder-bot.
5. Set Type to Element based.
6. Click the Color button and select a color.
7. Click Create.
   The Element Based Surface dialog opens, from which you can define elements and corresponding faces for the surface.
8. Click the Define tab.
9. Set Define surface for to 3D shell, membrane, rigid.
10. In the Model Browser, Component folder, right-click on BOT_CYLINDER and select Isolate from the context menu.
11. In the Element Based Surface dialog, click Elements.
12. In the panel area, click elems >> by collector.
13. Select the component, BOT_CYLINDER.
14. Click select.
    The elements in BOT_CYLINDER highlight.
15. Click proceed.
16. The normals of the selected elements will be displayed at this point. If the normals are too big, click (YZ Front Plane View) on the Standard Views toolbar.
17. Check the Reverse option.
18. Click Add to add these faces to the current surface.
    HyperMesh creates special face elements (rectangles with a dot at the middle) for display.

    
    
    Figure 8.

19. Optional: Reject the recently added faces by clicking Reject. You can also delete faces from the Delete page.
20. Click the Adjust Normal tab.
21. Click Display normals. Notice that all normals are pointing outwards.

    
    
    Figure 9.

22. When satisfied with the surface definition, click Close to return to the Abaqus Contact Manager.

In this step you will create surfaces by defining a set and corresponding face identifiers.

1. In the Abaqus Contact Manager, click the Surface tab.
2. Click Display None to turn off the display of all surfaces.
3. Click New.
   The Create New Surface dialog opens.
4. In the Name field, type box1-bot.
5. Set Type to Element based.
6. Click the Color button and select a color.
7. Click Create.
   The Element Based Surface dialog opens, from which you can define elements and corresponding faces for the surface.
8. Click the Define tab.
9. Set Define surface for to Element set.
10. In the Model Browser, Component folder, right-click on BOX_1 and select Isolate from the context menu.
11. On the Standard Views toolbar, click (YX Bottom Plane View).
12. In the Element Based Surface dialog, set Element set to box1-bot.
13. Click Review Set to highlight all elements in the selected set.
14. Right-click on Review Set to reset the highlighting.
15. Click Show Faces.
    HyperMesh creates a temporary skin of the selected element set.
16. Select an element from the bottom of the solid skin.
17. In the panel area, click elems >> by face.
    The faces on the bottom of the solid skin highlight.
18. Optional: Deselect any element by right-clicking, or add more if you like.
19. When you are satisfied with the element faces selected, click proceed to return to the Element Based Surface dialog.

    At this point, the face identifier tags (color coded) of the selected faces are displayed. 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.

20. Click the right arrow key to move the box1-bot set into the table.
21. In the table, click on the Face pull-down menu and select S3.
22. Select the Display checkbox and then click Update.
    HyperMesh adds the selected set and face identifier to the current surface. In addition it creates a special display for the surface.

    By default, HyperMesh does not create a display for surfaces defined with sets. However, if you select the Display checkbox before clicking Update, it will create a special display using contact surface elements. The special display does not have any link to the set in the HyperMesh database. Therefore, if you edit the set later on, the display will not reflect them automatically. In this case, you need to come to this page, select the Display checkbox and click Update again.

    
    
    Figure 10.

23. Click Close to return to the Abaqus Contact Manager.

In this step you will create the box2-bot surface.

1. In the Abaqus Contact Manager, click the Surface tab.
2. Click Display None to turn off the display of all surfaces.
3. Click New.
   The Create New Surface dialog opens.
4. In the Name field, type box2-bot.
5. Set Type to Element based.
6. Click the Color button and select a color.
7. Click Create.
   The Element Based Surface dialog opens, from which you can define elements and corresponding faces for the surface.
8. Click the Define tab.
9. Set Define surface for to Element set.
10. In the Model Browser, Component folder, right-click on BOX_2 and select Isolate from the context menu.
11. On the Standard Views toolbar, click (YX Bottom Plane View).
12. In the Element Based Surface dialog, click Create/Edit Sets.
13. In the panel area, type box2-bot in the name field.
14. Click elems >> by collector.
15. Select the component, BOX_2.
16. Click select.
17. Click create.

    
    
    Figure 11.

18. When you are done creating/editing the set, click return.
19. Set Element set to box2-bot.
20. Click Review Set to highlight the elements in the selected set.
21. Right-click on Review Set to reset the highlighting.
22. Click Show Faces.
    HyperMesh creates a temporary skin of the selected element set.
23. Select an element from the bottom of the solid skin.
24. In the panel area, click elems >> by face.
    All faces on the bottom of the solid skin highlight.
25. Optional: Deselect any element by right-clicking or add more if you like.
26. When you are satisfied with the element faces selected, click proceed to return to the Element Based Surface dialog.

    At this point, the face identifier tags (color coded) of the selected faces display. 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.

27. Click the right arrow to move the box2-bot set into the table.
28. In the table, click on the Face pull-down menu and select S3.
    Note: Because all face identifier tags for the bottom side of the box2-bot set are S3, you can use the S3 identifier for this set.
29. Clear the Display checkbox if it is selected, then click Update to add the selected set and face identifier to the current surface.
    Note: By default, HyperMesh does not create any display for surfaces defined with sets.
30. Click Close to return to the Abaqus Contact Manager.
    Note: In the Surface table the Display option for the box2-bot surface is disabled.
    At this point, you have created all required surfaces.
31. Click Display All to display all surfaces.
32. In the Model Browser, right-click on the Components folder and select Show from the context menu.
    All components display.
33. On the Standard View toolbar, click (Isometric).

    
    
    Figure 12.

34. Review a surface by selecting it from the table and clicking Review. Selected surfaces will be highlighted in red, while the rest of the model displays in gray. If the surface is defined with sets (display option disabled), the underlying elements are highlighted. Right-click on Review to clear the highlighting.

In this step you will define the *SURFACE INTERACTION card with a corresponding *FRICTION card.

1. In the Abaqus Contact Manager, click the Surface Interaction tab.
2. Click New.
   The Create New Surface Interaction dialog opens.
3. In the Name field, type friction1.
4. Click Create.
   The Surface Interaction dialog opens.
5. Click the Define tab.
6. Under Select mechanical interaction properties, select Friction.
7. Click the Friction tab.
8. Set Friction type to Default.
9. In the second pane, select Direct.
   Note: Selecting this option means that the exponential decay and Anisotropic parameters will not be written to the input file.
10. In the No of data lines field, type 1.
    A single row appears in the Direct table.
11. In the Friction Coeff column, click the first cell and type 0.05.
    For Direct and Anisotropic tables:

    • Change the number of columns in the table by specifying a value in the No of Dependencies field; change the number of rows in the table by specifying a value in the No of data lines field.
    • Enter values in the table by clicking a cell to make it active and then typing in values. The table works like a regular spreadsheet.
    • Read comma-delimited data from a text file by clicking Read From a File. In the File Browser, select a 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.
    • Access copy, cut, and paste options by right-click in the table. 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.
    • Activate cells by left-clicking in a cell. Clicking into an already active cell moves the insertion cursor to the character nearest the mouse.
    • Highlight cells by left-clicking while moving the mouse over a cell.
    • Move the active cell using the left, right, up, and down arrows.
    • Extend the selection in a specific direction using Shift-<arrow>.
    • Move the insertion cursor within a cell using Ctrl-left arrow and Ctrl –right arrow.
    • Selects all cells using Ctrl -slash.
    • Delete the character before the insertion cursor in the active cell using Backspace. If multiple cells are selected, Backspace deletes all selected cells.
    • Remove the character after the insertion cursor in the active cell using Delete. If multiple cells are selected, Delete removes all selected cells.
    • Move the insertion cursor to the beginning of the active cell using Ctrl-A. Move the insertion cursor to the end of the active cell using Ctrl-E.
    • Decrease and increase the width of the column with the active cell in it using Ctrl-minus (-) and Ctrl-equal (=).
    • Interactively resize a row or column by left-clicking or right-clicking on a border while moving the mouse.
12. Click OK to return to the Abaqus Contact Manager.

In this step you will define the *CONTACT PAIR card with corresponding surfaces and surface interaction.

1. In the Abaqus Contact Manager, click the Interface tab.
2. Click New.
   The Create New Interface dialog opens.
3. In the Name field, type top_cylinder_box1.
4. Set Type to Contact pair.
5. Click Create.
   The Contact Pair dialog opens.
6. Click the Define tab.
7. Set Surface to box1-top.
8. Click Slave >> to identify box1-top as the secondary surface and move it into the table.
9. Click Review.
   The selected surface highlights red. If the surface is defined with sets (display option disabled), the underlying elements highlight. Right-click on Review to clear the highlighting.

   Clicking New opens the Create New Surface dialog, from which you can create a new surface. When you are done creating and defining the surface, the Contact Pair dialog returns with the new surface selected as the secondary surface.

   
   
   Figure 13.

10. Repeat Steps 10.7 and 10.8, selecting cylinder-top and clicking Master>> to identify it as the master surface.
    Note: To more clearly see the surfaces available for selection, click . This opens an enhanced browser where you can easily search for the appropriate item. You can also click Filter to filter the items displayed.
11. Set Interaction to friction1.
    Note: To more clearly see the interactions available for selection, click . This opens an enhanced browser where you can easily search for the appropriate item. You can also click Filter to filter the items displayed.
12. Click the Parameter tab.
13. Select the Small sliding checkbox.
14. Click OK to return to the Abaqus Contact Manager.

In this step you will create the top-cylinder-box2 contact pair.

In this step you will create the bot-cylinder-box1 contact pair.

In this step you will create the bot-cylinder-box2 contact pair.