To define surface-to-surface contact:

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.

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,” Section 3.2.1.

Select the step in which the interaction will be created.

Select the Surface-to-surface contact type of interaction.

Click Continue to close the Create Interaction dialog box.

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,” Section 6.2.) Click mouse button 2 to indicate you have finished selecting. You must select a region from only one part instance; the region that you select cannot span multiple part instances.

If the model contains a combination of orphan mesh instances and native geometric part instances, click one of the following from the prompt area:

• Click Geometry if you want to select the surface from a native geometric part instance.

• Click Mesh if you want to select the surface from an orphan mesh instance.

You can use the angle method to select a group of faces or edges from a native geometric part instance or a group of element faces from an orphan mesh part instance. For more information, see “Using the angle method to select multiple objects,” Section 6.2.3.

The master surface that you select becomes highlighted in red in the viewport.

Select the slave surface.

In the prompt area, click the arrow next to the text field and 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.

Use one of the same methods described earlier to select the slave surface or region. As with the master surface, the surface or region that you select cannot span multiple part instances.

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

After you select the slave surface, the Edit Interaction dialog box appears. The Switch button allows you to interchange your master and slave surface selections without having to start over.

In the Edit Interaction dialog box, do the following:

If you will be performing an ABAQUS/Explicit analysis, choose the mechanical constraint formulation. For more information, see “Contact formulation for ABAQUS/Explicit contact pairs,” Section 21.4.4 of the ABAQUS Analysis User's Manual.

Choose the sliding formulation. For more information, see “Contact formulation for ABAQUS/Standard contact pairs,” Section 21.2.2 of the ABAQUS Analysis User's Manual, and “Contact formulation for ABAQUS/Explicit contact pairs,” Section 21.4.4 of the ABAQUS Analysis User's Manual.

• If you will be performing an ABAQUS/Standard analysis and you choose the Small sliding formulation, you can select the constraint enforcement method. For more information, see “Using the small-sliding formulation” in “Contact formulation for ABAQUS/Standard contact pairs,” Section 21.2.2 of the ABAQUS Analysis User's Manual.

• If you choose the Surface to surface constraint enforcement method for small-sliding contact, you can specify whether or not shell and membrane thicknesses should be included in the contact calculations. Contact interactions using the Node to surface constraint enforcement method do not account for surface thickness.

If you will be performing an ABAQUS/Standard analysis, specify the slave node adjustment option of your choice. For more information, see “Adjusting initial surface positions and specifying initial clearances in ABAQUS/Standard contact pairs,” Section 21.2.3 of the ABAQUS Analysis User's Manual.

Select a contact interaction property. If desired, click Create to create the interaction property.

If you will be performing an ABAQUS/Standard analysis, enter the interference fit options, if desired. The interference fit options are available only in the first general analysis step. For more information, see “Adjusting initial surface positions and specifying initial clearances in ABAQUS/Standard contact pairs,” Section 21.2.3 of the ABAQUS Analysis User's Manual.

If you will be performing an ABAQUS/Explicit analysis, choose the weighting factor. For more information, see “Contact formulation for ABAQUS/Explicit contact pairs,” Section 21.4.4 of the ABAQUS Analysis User's Manual.

If desired, click the arrow next to the Contact controls field and select the customized contact controls to use for this interaction. The list of contact controls is filtered based on the type of analysis that you are performing; for example, if you are performing an ABAQUS/Standard analysis, only ABAQUS/Standard contact controls that were previously specified will appear in the list. For more information, see “Specifying contact controls in an ABAQUS/Standard analysis,” Section 15.12.3, and “Specifying contact controls in an ABAQUS/Explicit analysis,” Section 15.12.4.

Note:  You can display help on a particular editor feature by selecting HelpOn Context from the main menu bar and then clicking the editor feature of interest.

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