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. Certain connectivity restrictions apply to contact surfaces depending on the type of contact formulation. For detailed information, see “Defining contact pairs in ABAQUS/Standard,” Section 29.2.1 of the ABAQUS Analysis User's Manual and “Defining contact pairs in ABAQUS/Explicit,” Section 29.4.1 of the ABAQUS Analysis User's Manual.

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.

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 29.4.4 of the ABAQUS Analysis User's Manual.

Choose the sliding formulation. For more information, see “Contact formulation for ABAQUS/Standard contact pairs,” Section 29.2.2 of the ABAQUS Analysis User's Manual, and “Contact formulation for ABAQUS/Explicit contact pairs,” Section 29.4.4 of the ABAQUS Analysis User's Manual.

If you will be performing an ABAQUS/Standard analysis, you can select the constraint enforcement method. By default, shell and membrane thicknesses are included in contact calculations for the following combinations of sliding formulation and constraint enforcement method: Small sliding and Node to surface; Small sliding and Surface to surface; and Finite sliding and Surface to surface. You can toggle on Exclude shell/membrane element thickness to ignore shell and membrane thickness for any of these combinations.

Contact interactions using the Finite sliding formulation and Node to surface constraint enforcement method do not account for surface thickness. For more information, see “Accounting for shell and membrane thickness” in “Contact formulation for ABAQUS/Standard contact pairs,” Section 29.2.2 of the ABAQUS Analysis User's Manual.

For contact interactions using the Finite sliding formulation, you can specify a smoothing factor in the Degree of smoothing for master surface field. For more information, see “Smoothing master surfaces for the finite-sliding, node-to-surface formulation” in “Contact formulation for ABAQUS/Standard contact pairs,” Section 29.2.2 of the ABAQUS Analysis User's Manual.

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 29.2.5 of the ABAQUS Analysis User's Manual, and “Defining tied contact in ABAQUS/Standard,” Section 29.2.7 of the ABAQUS Analysis User's Manual.

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. Click the Clearance tab, 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 “Defining a precise initial clearance or overclosure for small-sliding contact” in “Adjusting initial surface positions and specifying initial clearances in ABAQUS/Standard contact pairs,” Section 29.2.5 of the ABAQUS Analysis User's Manual, and “Specifying initial clearance values precisely” in “Adjusting initial surface positions and specifying initial clearances in ABAQUS/Explicit contact pairs,” Section 29.4.5 of the ABAQUS Analysis User's Manual.

Select a contact interaction property. If desired, click Create to create the interaction property; see “Defining a contact interaction property,” Section 15.13.1, for more information.

If you are performing an ABAQUS/Standard analysis and you choose the Finite sliding formulation and the Surface to surface constraint enforcement method, the contact interaction property that you select cannot specify a “hard” contact pressure-overclosure relationship. For more information, see “Constraint enforcement methods for ABAQUS/Standard contact pairs,” Section 29.2.3 of the ABAQUS Analysis User's Manual, and “Defining mechanical contact property options” in “Defining a contact interaction property,” Section 15.13.1.

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 “Modeling contact interference fits in ABAQUS/Standard,” Section 29.2.4 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 29.4.4 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.