A self-contact definition can be used as an alternative to general contact to model contact interactions between different areas of a single surface. Certain interaction behaviors can be defined only by using self-contact. For a brief overview of self-contact and other types of interactions available in Abaqus, see “Understanding interactions,” Section 15.3, and “Contact interaction analysis: overview,” Section 31.1.1 of the Abaqus Analysis User's Manual.
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 31.3.1 of the Abaqus Analysis User's Manual, and “Defining contact pairs in Abaqus/Explicit,” Section 31.5.1 of the Abaqus Analysis User's Manual.
You can obtain contact data for a specific self-contact interaction by using the field and history output request editors in the Step module. In the Domain section of the editors, select Interaction and choose the name of the self-contact interaction from the menu that appears. For more information, see “Creating an output request,” Section 14.12.1.
The procedure for defining self-contact depends on whether you are performing an analysis using Abaqus/Standard or Abaqus/Explicit. This section provides instructions for using the interaction editor to define the different surface-to-surface contact options. The following topics are covered:
Certain interaction behaviors can be defined in Abaqus/Standard only by using self-contact; see “Contact simulation capabilities in Abaqus/Standard” in “Contact interaction analysis: overview,” Section 31.1.1 of the Abaqus Analysis User's Manual, for more information.
To define self-contact in an Abaqus/Standard analysis:
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 (Standard) 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 31.3.1 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.
Select the discretization method.
Select Node to surface to use the node-to-surface discretization method.
Select Surface to surface to use the surface-to-surface discretization method.
Different fields become available depending upon your discretization method selection.
For contact interactions using the Node to surface discretization method, you can specify the following:
Enter a smoothing factor in the Degree of smoothing field. For more information, see “Smoothing master surfaces for the finite-sliding, node-to-surface formulation” in “Contact formulations in Abaqus/Standard,” Section 33.1.1 of the Abaqus Analysis User's Manual.
By default, a selective scheme of supplementary contact constraints is used. You can specify when to Use supplementary contact points as follows:
Choose Selectively to use a selective scheme of supplementary contact constraints.
Choose Never to forgo the use of supplementary contact constraints.
Choose Always to add supplementary contact constraints when applicable.
For contact interactions using the Surface to surface discretization method, you can specify the following:
By default, shell and membrane thicknesses are included in the contact calculations. You can toggle on Exclude shell/membrane element thickness to ignore shell and membrane thickness. Contact interactions using the Node to surface discretization method do not account for surface thickness.
Choose the Constraint position.
Choose Node centered to center contact constraints at slave nodes.
Choose Face centered to center contact constraints within slave faces.
Choose the Contact tracking algorithm.
Choose Single configuration (state) to use the state-based tracking algorithm.
Choose Two configurations (path) to use the path-based tracking algorithm.
Select a contact interaction property. If desired, click Create to create the interaction property; see “Defining a contact interaction property,” Section 15.14.1, for more information.
If you choose the Surface to surface discretization method, the contact interaction property that you select cannot specify a “hard” contact pressure-overclosure relationship. For more information, see “Contact constraint enforcement methods in Abaqus/Standard,” Section 33.1.2 of the Abaqus Analysis User's Manual, and “Defining mechanical contact property options” in “Defining a contact interaction property,” Section 15.14.1.
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/Standard contact controls appear in the list. For more information, see “Specifying contact controls in an Abaqus/Standard analysis,” Section 15.13.8.
Click OK to create the interaction and to close the editor.
Certain interaction behaviors can be defined in Abaqus/Explicit only by using self-contact; see “Contact simulation capabilities in Abaqus/Explicit” in “Contact interaction analysis: overview,” Section 31.1.1 of the Abaqus Analysis User's Manual, for more information.
To define self-contact in an Abaqus/Explicit analysis:
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 (Explicit) 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/Explicit,” Section 31.5.1 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.
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.
Select a contact interaction property. If desired, click Create to create the interaction property; see “Defining a contact interaction property,” Section 15.14.1, for more information.
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,” Section 15.13.9.
Click OK to create the interaction and to close the editor.