HM-4420: Define ANSYS Contacts for Models in HyperMesh

In this step, you will load the ANSYS user profile in HyperMesh.

1. Start HyperMesh Desktop.
2. In the User Profile dialog, set the user profile to Ansys.

In this step, you will open a model file in HyperMesh.

1. From the menu bar, click File > Open > Model.
2. In the Open Model dialog, open the hm-ansys_contact_manager_2-d_tutorial.hm file.
   The model loads in the graphics area.
3. Optional: If the load collector is displayed, click in the Model Browser next to the load collector to turn off the display of the element.

   
   
   Figure 1.

4. In the graphics area, click once to make it the current window for keyboard commands.
5. Fit the model to the graphics area by pressing F.

   
   
   Figure 2.

In this step, you will open the Contact Browser in HyperMesh.

In this step, you will create a target surface in HyperMesh.

1. In the first pane of the Contact Browser, right-click and select Create > Contact Surfaces from the .context menu

   
   
   Figure 3.

   HyperMesh creates and opens a contact surface in the Entity Editor.
2. In the Entity Editor, enter a name and ID, and select a color for the contact surface.
3. For Elements, click 0 Elements > Elements.

   
   
   Figure 4.

4. In the panel area, set the first selector to add shell edges.
5. Check the reverse normals checkbox.
6. For face angle, enter 30.0.
7. Set the entity selector to elems, then select the free edges indicated in Figure 5.

   
   
   Figure 5.

   Tip: Quickly select elements with window selection by pressing Shift while clicking and dragging your mouse.
8. Use the nodes selector to select two nodes along the free edges you selected in step 7.

   
   
   Figure 6.

9. Click Add.
   All of the edges of the selected elements are added to the surface.

   
   
   Figure 7.

10. Click return to exit the panel.
11. Review the contact surface.
    1. In the Contact Browser, right-click on contactsurf_1 and select Review from the context menu.
    2. Isolate the contact surface for a better visual display.
       The surface created here will be considered the target (secondary) surface during analysis.

In this step, you will create a contact surface in HyperMesh.

1. In the first pane of the Contact Browser, right-click and select Create > Contact Surfaces from the context menu.
   HyperMesh creates and opens a contact surface in the Entity Editor.
2. In the Entity Editor, enter a name and ID, and select a color for the contact surface.
3. For Elements, click 0 Elements > Elements.
4. In the panel area, set the first selector to add shell edges.
5. For face angle, enter 30.0.
6. Check the reverse normals checkbox.
7. Set the entity selector to free edges, then select the top free edges of the rectangular box as indicated in Figure 8.

   
   
   Figure 8.

8. Click add.

   
   
   Figure 9.

   Surfaces are created on the top edge of the rectangular box.
9. Click return to exit the panel.

In this step, you will create a contact pair.

1. In the second pane of the Contact Browser, right-click and select Create > Contact Pair from the context menu.
   HyperMesh creates and opens a contact pair in the Entity Editor.

   
   
   Figure 10.

2. In the Entity Editor, enter a name and ID, and select a color for the contact pair.
3. Attach the contact (master) surface.
   1. For Master IDs, click 0 Contactsurfs > Contactsurfs.

      
      
      Figure 11.

   2. In the Select Contactsurfs dialog, select contactsurf_2 and click OK.

      
      
      Figure 12.

   3. Under MASTER, right-click on ETType, and select Create from the context menu.

      
      
      Figure 13.

   4. In the Create Sensors dialog, define the sensor.
      • Enable KeyOpt12.
      • Select 0-Standard from the list.

      By default, the Element Type is set to CONTA171. Keyopts determine the behavior of contacts during analysis. KeyOpt12 defines the type of contact.
   5. Click Close.

      
      
      Figure 14.

4. Attach the target (secondary) surface.
   1. For Secondary IDs, click 0 Contactsurfs > Contactsurfs.
   2. In the Select Contactsurfs dialog, select contactsurf_1 and click OK.
      In this contact pair, contactsurf_1 acts as the target (secondary) surface. This surface will be exported with the element type Targe169.
   3. Under SECONDARY, right-click on ETType and select Create from the context menu.
   4. Define the sensor in the Create Sensors dialog.
      • Enable KeyOpt4.
      • Select 111-ROTZ, UY, UX from the list.

      By default, the Element Type is set to Targe169. The target (secondary) surface will be exported with the elements type TARGE169.
   5. Click Close.
5. Create and attach the contact property.
   A contact property for a pair is always required, as the solver recognizes the pair only by the property ID associated with the main and secondary surfaces. Same property IDs are shared by the main and secondary surfaces. If a property ID is missing for a contact surface, then it will not be considered as part of the contact pair and it will not recognized.
   1. In the Entity Editor, right-click on Property and select Create from the context menu.
   2. Define the property in the Create Properties dialog.
      • For FKN, enter 1.0.
      • For FTOLN, enter 0.1.
      • For TAUMAX, enter 1e20.
      • For FKOP, enter 1.0.
      • For FKT, enter 1.0.
      • For FHTG, enter 1.0.
      • For RDVF, enter 1.0.
      • For FWGT, enter 0.5.
      • For FACT, enter 1.0.
   3. Click Close.
6. Create and attach the contact material.
   The properties MU (coefficient of friction) and EMIS (Thermal Emissivity) are available to define. If you are creating a structural contact, select MU; if you are creating a thermal contact, select EMIS. In this exercise you will be creating a structural contact.
   1. In the Entity Editor, right-click on Material and select Create from the context menu.
   2. Define the material in the Create Materials dialog.
      • Select the MU (coefficient of friction) checkbox.
      • For MP_MU_LEN, enter 1.
      • For C, enter 0.45.
   3. Click Close.

In this step, you will review the contact pair you created in step Create a Contact Pair.

1. In the second pane of the Contact Browser, select the contact pair created in Create a Contact Pair.
   The contact pair entity details display in the Entity Editor.
2. Right-click on the contact pair and select Isolate Attached > Elements to review the contact area.

   
   
   Figure 15.

In this step, you will add the following Control Cards.

1. Click Setup > Create > Control Cards from the menu bar.
   The Control Cards panel opens.
2. To exit the PREP7 preprocessor and enter the SOLU preprocessor click /SOLU.

   
   
   Figure 16.

3. Click return.

   
   
   Figure 17.

4. Since you are solving the model for static analysis, click ANTYPE.

   
   
   Figure 18.

5. Set type to STATIC and status to NEW.

   
   
   Figure 19.

6. Click return.
7. Click SOLVE.
   Tip: If you do not see the SOLVE Control Card, click next.

   
   
   Figure 20.

8. Click return to exit the card image.
9. Click return to exit the Control Cards panel.