Defining surface-to-surface contact in an Abaqus/Explicit analysis

Certain interaction behaviors can be defined in Abaqus/Explicit only by using surface-to-surface 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 surface-to-surface 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 Surface-to-surface 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 master 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.) Click mouse button 2 to indicate you have finished selecting. 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 master surface that you select becomes highlighted in red in the viewport.

  5. Select the slave surface.

    1. In the prompt area, select one of the following:

      • Select Surface if you want to select a surface.

      • Select Node Region if you want to select a region from which to create a contact node set.

    2. Use one of the same methods described earlier to select the slave surface or region.

      The slave surface or region that you select becomes highlighted in magenta in the viewport.

      The Edit Interaction dialog box appears.

  6. The Switch Surfaces option allows you to interchange your master and slave surface selections without having to start over. The Switch Surfaces icon is available only if you selected Surface in the previous step.

  7. 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.

  8. Choose the sliding formulation.

    • Choose Finite sliding to use the finite-sliding formulation, which is the most general and allows any arbitrary motion of the surfaces.

    • Choose Small sliding to use the small-sliding formulation, which assumes that although two bodies may undergo large motions, there will be relatively little sliding of one surface along the other.

    The small-sliding formulation can be specified for interactions created in only the initial step or the first general analysis step. Interactions created in subsequent steps always use the finite-sliding formulation by default. For more information, see Contact formulations for contact pairs in Abaqus/Explicit.

  9. For contact interactions using the Small sliding formulation, you can specify an initial clearance between the nodes on the slave surface and the master surface. Clearance options are available only in the first general analysis step. Select a clearance type from the Initial clearance field, and enter all of the data necessary to define the clearance and contact direction. For more information, see Specifying initial clearance values precisely.

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

  11. Choose the weighting factor. For more information, see Contact formulations for contact pairs in Abaqus/Explicit.

  12. 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.

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

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