You can specify contact controls for surface-to-surface contact and self-contact interactions in an ABAQUS/Standard analysis. For a detailed discussion, see “Adjusting contact controls in ABAQUS/Standard,” Section 29.2.12 of the ABAQUS Analysis User's Manual.
Warning: Contact controls are intended for advanced users. The default settings of these controls are appropriate for most analyses. Using nondefault values of these controls may greatly increase the computational time of the analysis, produce inaccurate results, or cause convergence problems.
To specify contact controls in an ABAQUS/Standard analysis:
From the main menu bar, select Interaction
Contact ControlsCreate.
In the Create Contact Controls dialog box that appears, do the following:
Name the contact controls.
Select ABAQUS/Standard contact controls as the type of contact controls.
Click Continue to close the Create Contact Controls dialog box.
The Edit Contact Controls dialog box appears.
In the General portion of the editor, you can specify general controls for contact problems.
In the Friction onset field, select when the application of friction occurs.
Select Immediate to apply friction when contact occurs.
Select Delayed to delay the application of friction until the increment after contact occurs.
The slide distance is relevant only for finite-sliding simulations with three-dimensional deformable master surfaces when the “contact patch” algorithm is used instead of the “active topology” algorithm to account for changes in contact connectivity. When the contact patch algorithm is used, ABAQUS/Standard computes a suitable sliding distance for the slave nodes and reorders the equations when needed. If you want to specify the maximum slide distance that slave nodes can slide on the master surface, toggle on Specify slide distance near the middle of the dialog box and enter a value. If this slide distance is exceeded, the analysis will terminate. For more information, see “Efficiently accounting for changes in contact connectivity in the equation solver” in “Adjusting contact controls in ABAQUS/Standard,” Section 29.2.12 of the ABAQUS Analysis User's Manual.
If you want ABAQUS/Standard to automatically compute an overclosure tolerance and a separation pressure tolerance to prevent chattering in contact, toggle on Automatic overclosure tolerances near the middle of the dialog box. Alternatively, you can specify the following values:
Max number of points that can violate contact. Enter the maximum number of points that are permitted to violate the contact conditions in any increment. The amount by which the condition can be violated is limited by the values specified for Max tensile stress/force and Max overclosure distance (you must specify a value greater than zero for at least one of these parameters). The default value is 0.
Max tensile stress/force. Enter the maximum value of tensile stress (tensile force in GAP- or ITT-type contact elements) that ABAQUS/Standard will allow to be transmitted at a contact point. If any point in contact has a tensile stress/force across the contact interface greater than this value, the contact status will change, causing another iteration regardless of the number specified for Max number of points that can violate contact. The default value is 0.
Max overclosure distance. Enter the maximum overclosure distance allowed at a slave node that is considered to be open. If any point in contact is overclosed by more than this value, the contact status will change, causing another iteration regardless of the number specified for Max number of points that can violate contact. The default value is 0.
In the Enforce using Lagrange multipliers field, select one of the following to control the use of Lagrange multipliers in enforcing contact constraints:
Select Use analysis product default to let ABAQUS automatically determine whether or not Lagrange multipliers will be used.
Select Off to enforce the contact constraints without Lagrange multipliers.
Select On to enforce the contact constraints with Lagrange multipliers.
In the Stabilization portion of the editor, you can specify controls relating to automatic stabilization of rigid body motions in contact problems using viscous damping.
Select one of the following:
Select Automatic stabilization to use the default damping coefficient calculated automatically by ABAQUS/Standard. If desired, you can enter a value for the Factor by which the default damping coefficient will be multiplied.
Select Stabilization coefficient to specify the damping coefficient directly, and enter a value.
In the Tangent fraction field, enter a value for the fraction of the normal stabilization by which to modify the tangential stabilization. By default, the tangential and normal stabilization are the same.
Enter a value for the Fraction of damping at end of step.
Specify the Clearance at which damping becomes zero.
Select Computed to use the default clearance value calculated by ABAQUS/Standard.
Select Specify to enter a value for the clearance at which the damping becomes zero.
In the Augmented Lagrange portion of the editor, you can specify controls for interactions defined with a contact interaction property that uses augmented Lagrangian surface behavior.
In the Stiffness scale factor field, enter a value for the factor by which ABAQUS/Standard will scale the default penalty stiffnesses to obtain the stiffnesses used for the contact pairs. The default value is 1.
In the Penetration tolerance field, select one of the following to specify the allowable penetration that is permitted to violate the impenetrability condition:
Select Absolute, and enter a value for the allowable penetration.
Select Relative, and enter the ratio of the allowable penetration to the characteristic contact surface face dimension. The default value is 0.001.
Click OK to create the contact controls and to close the editor.
