Defining self-contact in an Abaqus/Explicit analysis

Certain interaction behaviors can be defined in Abaqus/Explicit only by using self-contact; see Contact simulation capabilities in Abaqus/Explicit for more information.

Related Topics
Interaction editors
Customizing contact controls
In Other Guides
About contact pairs in Abaqus/Explicit

  1. From the main menu bar, select InteractionCreate.

    Tip: You can also create a self-contact interaction using the tool in the Interaction module toolbox.

  2. In the Create Interaction dialog box that appears, do the following:

    • Name the interaction. For more information about naming objects, see Using basic dialog box components.

    • Select the step in which the interaction will be created.

    • Select the Self-contact (Explicit) type of interaction.

  3. Click Continue to close the Create Interaction dialog box.

  4. Use one of the following methods to select the surface:

    • Use an existing surface to define the region. On the right side of the prompt area, click Surfaces. Select an existing surface from the Region Selection dialog box that appears, and click Continue.

      Note:

      The default selection method is based on the selection method you most recently employed. To revert to the other method, click Select in Viewport or Surfaces on the right side of the prompt area.

    • Use the mouse to select a region in the viewport. (For more information, see Selecting objects within the current viewport.) Certain connectivity restrictions apply to contact surfaces depending on the type of contact formulation. For detailed information, see About contact pairs in Abaqus/Explicit.

      If the model contains a combination of mesh and geometry, click one of the following from the prompt area:

      • Click Geometry if you want to select the surface from a geometry region.

      • Click Mesh if you want to select the surface from a native or orphan mesh selection.

      You can use the angle method to select a group of faces or edges from geometry or a group of element faces from a mesh. For more information, see Using the angle and feature edge method to select multiple objects.

    The Edit Interaction dialog box appears.

  5. Choose the mechanical constraint formulation.

    • Choose Kinematic contact method to use a kinematic predictor/corrector contact algorithm.

    • Choose Penalty contact method to use the penalty contact algorithm.

    For more information, see Contact constraint enforcement methods in Abaqus/Explicit.

  6. Select a contact interaction property. If desired, click to create the interaction property; see Defining a contact interaction property, for more information.

  7. If desired, click the arrow next to the Contact controls field and select the customized contact controls to use for this interaction. Only previously created Abaqus/Explicit contact controls appear in the list. For more information, see Specifying contact controls in an Abaqus/Explicit analysis.

  8. To deactivate and reactivate the contact interaction, toggle Active in this step. The contact pair is active in the step in which it was created.

  9. Click OK to create the interaction and to close the editor.