HM-4420: Define ANSYS Contacts for Models in HyperMesh

In this tutorial you will learn how to set up edge to edge contacts, set up contacts manually, and create edge to edge contacts between circular and rectangular parts of a model.

Before you begin, it is recommended that you complete HM-1000: Getting Started with HyperMesh and Exploring the ANSYS Interface.

Also, copy the hm-ansys_contact_manager_2-d_tutorial.hm from <hm.zip>/interfaces/ansys/ to your working directory.

In HyperMesh, you can create contact pairs manually or with the Autocontact tool. The edge of the circular body acts as a Target (secondary) surface, and the top edge of the rectangular part acts as a contact (main) surface.

Restriction: This tutorial is only applicable for HyperMesh 14.0.130 and on.

Load the ANSYS User Profile

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

  1. Start HyperWorks.
  2. From the menu bar, click File > Solver Interface > Ansys.

Retrieve the Model File

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

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

Open the Contact Browser

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

From the Model ribbon, Contacts tool group, click the Contact Browser tool.


Figure 2.

Create Target (Secondary) Surface

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.
  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.

Create Contact (Main) Surface

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.

Create a Contact Pair

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 (main) surface.
    1. For Main IDs, click Unspecified then click the three dots.


      Figure 11.
    2. In the Advanced Selection dialog, select contactsurf_2 and click OK.


      Figure 12.
    3. Under MAIN, right-click on ETType, and select Create/Edit 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, Unspecified then click the three dots.
    2. In the Advanced Selection 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/Edit 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 Create and select Contact Properties from the context menu.
    2. Define the property under the Real Constants.
      • 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.
  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.

Review the Contact Pair

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.

Add /SOLU, ANTYPE, and SOLVE in the Control Cards

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

Restriction: Only complete this step if your model needs to be solved in ANSYS.
  1. In the panel area, click Analysis > Control Cards.
    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.