When you are configuring an XFEM analysis, you can select a contact interaction property that defines the compressive behavior of the crack surfaces. This section describes the settings in the contact interaction property that apply to XFEM crack growth. For more information, see “Understanding interaction properties,” Section 15.4.
To specify a contact interaction property:
From the main menu bar, select Interaction
PropertyCreate.
In the Create Interaction Property dialog box that appears, do the following:
Name the interaction property.
Select the Contact type of interaction property.
Click Continue to close the Create Interaction Property dialog box.
From the menu bar in the contact property editor, select MechanicalNormal Behavior.
From the Constraint enforcement method field, select Penalty (Standard) to enforce contact constraints using the penalty method.
Toggle off Allow separation after contact if you want to prevent surfaces from separating once they have come into contact.
Choose the Linear enforcement behavior in the Behavior field to use the linear penalty method for the enforcement of the contact constraint.
Specify the contact stiffness in the Stiffness value field.
Choose Use default to have Abaqus calculate the penalty contact stiffness automatically.
Choose Specify, and enter a positive value for the linear penalty stiffness.
Specify a factor by which to multiply the chosen penalty stiffness in the Stiffness scale factor field.
Specify the Clearance at which contact pressure is zero. The default value is 0.
Click OK to create the contact property and to exit the Edit Contact Property dialog box.