You can define self-contact in any step, including the initial step. Select Interaction
Create from the main menu bar and select the surface. You can define self-contact between an edge of a wire, a face of a solid, or a face of a shell. 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. For a brief overview of self-contact, see “Understanding interactions,” Section 15.3.
You can obtain contact data for a specific self-contact interaction by using the output request editors in the Step module. In the Domain section of the editors, select Interaction and the name of the self-contact interaction. For more information, see “Creating an output request,” Section 14.12.1.
To define self-contact:
From the main menu bar, select InteractionCreate.
Tip:
You can also create a self-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 Self-contact type of interaction.
Click Continue to close the Create Interaction dialog box.
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,” Section 6.2.) 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.
In the Edit Interaction dialog box that appears, 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.
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 Surface to surface constraint enforcement method (see below), 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, you can select the constraint enforcement method. For more information, see “Defining contact pairs in ABAQUS/Standard,” Section 29.2.1 of the ABAQUS Analysis User's Manual.
If you choose the Surface to surface constraint enforcement method, 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, 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 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.
Click OK to create the interaction and to close the editor.
