Specifying pressure-overclosure relationships for mechanical contact property options

From the main menu bar, select InteractionPropertyCreate.
In the Create Interaction Property dialog box that appears, do the following:
- Name the interaction property. For more information about naming objects, see Using basic dialog box components.
- 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 Pressure-Overclosure field, select “Hard” Contact to use the classical Lagrange multiplier method of constraint enforcement in an Abaqus/Standard analysis and to use penalty contact enforcement in an Abaqus/Explicit analysis.
You can also toggle off Allow separation after contact if you want to prevent surfaces from separating once they have come into contact. This method is applicable only to Abaqus/Standard analyses.
If you select “Hard” Contact, you can also customize settings for the constraint enforcement method. For more information about constraint enforcement methods, see Contact constraint enforcement methods in Abaqus/Explicit. To specify these settings, select an option from the Constraint enforcement method list and do the following:
1. Select Default to enforce constraints using a contact pressure-overclosure relationship.
2. Select Augmented Lagrange (Standard) to enforce contact constraints using the augmented Lagrange method. This method is applicable only to Abaqus/Standard analyses.
  
  If you select this option, specify the following additional settings from the Contact Stiffness options:
  - From the Stiffness value field, either select Use default to have Abaqus calculate the penalty contact stiffness automatically or select Specify and enter a positive value for the penalty contact 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.
3. Select the Penalty (Standard) constraint enforcement method to enforce contact constraints using the penalty method. This method is applicable only to Abaqus/Standard analyses.
  
  If you select this option, specify the following additional settings from the Contact Stiffness options:
  - From the Behavior field, either select Linear to use the linear penalty method for the enforcement of the contact constraint or select Nonlinear to use the nonlinear penalty method for the enforcement of the contact constraint. For more information, see Penalty method.
  - Specify the contact stiffness.
    - For the linear penalty method, specify the contact stiffness in the Stiffness value field. You can select Use default to have Abaqus calculate the penalty contact stiffness automatically or you can select Specify and enter a positive value for the linear penalty stiffness.
    - For the nonlinear penalty method, specify the contact stiffness in the Maximum stiffness value field. You can select Use default to have Abaqus calculate the penalty contact stiffness automatically or you can select Specify and enter a positive value for the final nonlinear penalty stiffness.
  - Specify a factor by which to multiply the chosen penalty stiffness in the Stiffness scale factor field.
  - For the nonlinear penalty method, you can specify values for the following options:
    - Enter the ratio of the initial penalty stiffness over the final penalty stiffness in the Initial/Final stiffness ratio field.
    - Enter the scale factor for the upper quadratic limit $d$ , which is equal to the scale factor times the characteristic contact facet length, in the Upper quadratic limit scale factor field.
    - Enter the ratio ( $e$ − $c_{0}$ )/( $d$ − $c_{0}$ ) that defines the lower quadratic limit $e$ in the Lower quadratic limit ratio field.
  - Specify the Clearance at which contact pressure is zero. The default value is 0.
4. Select Direct (Standard) to enforce contact constraints directly without approximation or use of augmentation iterations.
From the Pressure-Overclosure field, select Exponential to define an exponential pressure-overclosure relationship. If you select this option, specify the following:
1. Enter the contact pressure at zero clearance, $p_{0}$ , and the clearance at which the contact pressure is zero, $c_{0}$ , in the data table.
2. Specify the limit on the contact stiffness that the model can attain, $k_{m a x}$ (applies only for Abaqus/Explicit analyses).
  - Choose Infinite (no slip) to set $k_{m a x}$ equal to infinity for kinematic contact and equal to the default penalty stiffness for penalty contact.
  - Choose Specify, and enter a value for the maximum stiffness.
From the Pressure-Overclosure field, select Linear to define a linear pressure-overclosure relationship. If you select this option, specify the following:
- Enter a positive value for the slope of the pressure-overclosure curve, k, in the Contact stiffness field.
From the Pressure-Overclosure field, select Tabular to define a piecewise-linear pressure-overclosure relationship in tabular form. If you select this option, specify the following:
- Enter data in ascending order of overclosure to define the overclosure as a function of pressure. The data table must begin with a zero pressure. The pressure-overclosure relationship is extrapolated beyond the last overclosure point by continuing the same slope.
From the Pressure-Overclosure field, select Scale Factor (General Contact, Explicit) to define a piecewise-linear pressure-overclosure relationship based on scaling the default contact stiffness. This option is available only for the general contact algorithm in Abaqus/Explicit. If you select this option, specify the following:
1. To define the overclosure measure as a percentage of the minimum element size, select factor in the Overclosure field and enter a positive value $r$ .
2. To define the overclosure measure directly, select measure in the Overclosure field and enter a positive value $d$ .
3. Enter a value, $s$ , greater than one to define the geometric scaling of the base stiffness in the Contact stiffness scale factor field.
4. Enter a positive value $s_{0}$ to define an additional scale factor for the base default contact stiffness in the Initial stiffness scale factor field. The default value is 1.
Click OK to create the contact property and to exit the Edit Contact Property dialog box. Alternatively, you can select another contact property option to define from the menus in the Edit Contact Property dialog box.