29.2.12 Adjusting contact controls in ABAQUS/Standard

Products: ABAQUS/Standard  ABAQUS/CAE  



Contact controls in ABAQUS/Standard:

  • should not be modified from the default settings for the majority of problems;

  • can be used for problems where the standard contact controls do not provide cost-effective solutions; and

  • can be used for problems where the standard controls do not effectively establish the desired contact conditions.

Problems that benefit from adjustments to the contact controls in ABAQUS/Standard are generally large models with complicated geometries and numerous contact interfaces.

Applying contact controls

You can apply contact controls on a step-by-step basis to all of the contact pairs and contact elements that are active in the step or to individual contact pairs. This makes it possible to apply contact controls to a specific contact pair to take the simulation through a difficult phase. Contact controls remain in effect until they are either changed or reset to their default values. If in any given step the contact controls are declared for both the entire model and for a specific contact pair, the controls for the specific contact pair will override those for the entire model for that contact pair.

Input File Usage:           To apply contact controls to all contact pairs and contact elements:
contact control options

To apply contact controls to a specific contact pair:

*CONTACT CONTROLS, SLAVE=slave surface, MASTER=master surface
contact control options

Repeat this option to apply contact controls to several contact pairs.

ABAQUS/CAE Usage: Contact controls in ABAQUS/CAE can be applied only to specific contact pairs:

Interaction module: InteractionContact ControlsCreate: ABAQUS/Standard contact controls Contact interaction editor: Contact controls: contact controls name

Resetting contact controls

You can reset all contact controls to their default values, or you can reset the controls for a specific contact pair.

Input File Usage:           To reset all contact controls:

To reset the controls for a specific contact pair:

*CONTACT CONTROLS, SLAVE=slave surface, 
MASTER=master surface, RESET


Interaction module: contact interaction editor: Contact controls: (Default)

You cannot reset all contact controls at once in ABAQUS/CAE.

Automatic stabilization of rigid body motions in contact problems

ABAQUS/Standard offers two capabilities that automatically control rigid body motions in static problems before contact closure and friction restrain such motions. You can activate either capability in a particular step.

It is recommended that you first try to stabilize rigid body motion through modeling techniques (modifying geometry, imposing boundary conditions, etc.). The automatic stabilization capabilities are meant to be used in cases in which it is clear that contact will be established, but the exact positioning of multiple bodies is difficult during modeling. They are not meant to simulate general rigid body dynamics; nor are they meant for contact chattering situations or to resolve initially tight clearances between mating surfaces.

When either form of automatic stabilization is used, ABAQUS/Standard activates viscous damping for relative motions of the contact pair at all slave nodes, in the same manner as contact damping (see Contact damping, Section 30.1.3). Unlike most contact controls, which carry over to subsequent steps until they are modified or reset, automatic stabilization damping is applied only for the duration of the step in which it is specified. In subsequent steps the stabilization is removed, even if contact was not established or if rigid body motions appear later because of complete separation of the contact pair. If needed, you should specify stabilization for subsequent steps as well.

There are some important differences between the two stabilization methods.

Stabilization based on the initial opening distance

This method is meant specifically to address situations where a single rigid body mode exists normal to the contact direction. It applies damping only in the contact direction to a specific contact pair that you select and calculates the damping coefficient automatically such that contact is established in the first part of the step. The first increment of a step that has this form of stabilization activated will always produce at least two attempts: ABAQUS uses the first attempt to calculate the damping coefficient.

In the first half of the step the viscous damping is maintained at a constant value, and in the second half of the step it is decreased linearly to zero. If no stabilization is applied in the next step, the solution is continuous since the viscous forces at the end of the previous step are already zero. Care should be exercised in cases that require a restart analysis to be run from the middle of a step in which this form of stabilization is used. If the original step is terminated before restart (see Truncating a step” in “Restarting an analysis, Section 9.1.1), convergence difficulties may occur because viscous forces will then be removed abruptly. Contact controls should be activated in a continuation step of this kind.

Usually, stabilization based on the initial opening distance is used only in the first step of an analysis. However, it can be used in an analysis step subsequent to the first for the purpose of establishing contact between separated bodies that do not have rigid body motions initially. During the step in which this form of stabilization is activated, the applied loading should be restricted to that necessary to establish contact, and additional deformation of the bodies during the step should not be significant.

Input File Usage:           
SLAVE=slave surface

ABAQUS/CAE Usage: Stabilization based on the initial opening distance is not supported in ABAQUS/CAE. Use the more general stabilization based on the stiffness of the underlying elements (described below) instead.

Stabilization based on the stiffness of the underlying elements

This method is meant to address more general situations. By default, the damping coefficient:

  • is calculated automatically for each contact constraint based on the stiffness of the underlying elements and the step time,

  • is applied to all contact pairs equally in the normal and tangential directions,

  • is ramped down linearly over the step,

  • is active only when the distance between the contact surfaces is smaller than a characteristic surface dimension, and

  • is zero for contact modeled with contact elements (such as gap contact elements, tube-to-tube contact elements, etc.).

Although the automatically calculated damping coefficient will typically provide enough damping to eliminate the rigid body modes without having a major effect on the solution, there is no guarantee that the value is optimal or even suitable. This is particularly true for thin shell models, in which the damping may be too high. Hence, you may have to increase the damping if the convergence behavior is problematic or decrease the damping if it distorts the solution. The first case is obvious, but the latter case requires a post-analysis check. There are several ways to carry out such checks. The simplest method is to consider the ratio between the energy dissipated by viscous damping and a more general energy measure for the model, such as the elastic strain energy. These quantities can be obtained as output variables ALLSD and ALLSE, respectively. More detailed information can be obtained by comparing the contact damping stresses CDSTRESS (with the individual components CDPRESS, CDSHEAR1, and CDSHEAR2) to the true contact stresses CSTRESS (with the individual components CPRESS, CSHEAR1, and CSHEAR2). If the contact damping stresses are too high, you should decrease the damping. The comparison should be made after contact is firmly established; the contact damping stresses will always be relatively high when contact is not yet or only partially established.

The easiest way to increase or decrease the amount of damping is to specify a factor by which the automatically calculated damping coefficient will be multiplied. Typically, you should initially consider changing the default damping by (at least) an order of magnitude; if that addresses the problem sufficiently, you can do some subsequent fine-tuning. In some cases a larger or smaller factor may be needed; this is not a problem as long as a converged solution is obtained and the dissipated energy and contact damping stresses are sufficiently small.

It is also possible to specify the damping coefficient directly. This is particularly useful if ABAQUS is not able to calculate a sensible damping value. For example, this may be the case if the slave surface is a node-based surface, in which case the properties of the underlying elements are not available. Direct specification of the damping value is not easy and may require some trial and error. For efficiency reasons this may best be done on a similar model of reduced size. If the damping coefficient is specified directly, any multiplication factor specified for the default damping coefficient is ignored.

Input File Usage:           To use the default damping coefficient:

To specify a scale factor for the default damping coefficient:


To specify the damping coefficient directly:

damping coefficient 


Interaction module: ABAQUS/Standard contact controls editor: Stabilization: Automatic stabilization, Factor: factor or Stabilization coefficient: damping coefficient

Specifying the stabilization ramp-down factor

You can specify the ramp-down factor at the end of the step. By default, this value is equal to zero, so that the damping vanishes completely at the end of the step. Entering a nonzero value for this factor can be useful in cases where the rigid body modes are not fully constrained at the end of the step; for example, if the problem is frictionless and sliding motions can occur but there is no net force in the sliding direction. In that case it is usually desirable to maintain the small damping in the next step by using the value used for the ramp-down as the multiplication factor for the damping coefficient. If needed, you can maintain this damping level by setting the ramp-down factor equal to one.

Input File Usage:           
 , ramp-down factor


Interaction module: ABAQUS/Standard contact controls editor: Stabilization: Automatic stabilization or Stabilization coefficient, Fraction of damping at end of step: ramp-down factor

Specifying the damping range

By default, the opening distance over which the damping is applied (the damping range) is equal to the characteristic slave surface facet dimension; if such a dimension is not available (for example, in the case of a node-based surface), a characteristic element length obtained for the whole model is used. The damping is 100% of the reference value for openings less than half the damping range and from there is ramped to zero for an opening equal to the damping range. Alternatively, you can specify the damping range directly, overriding the calculated value. This can be useful if the damping should work only for a narrow gap, or if the damping should be in effect regardless of the opening distance. In the latter case a large value should be entered.

Input File Usage:           
 , , damping range


Interaction module: ABAQUS/Standard contact controls editor: Stabilization: Automatic stabilization or Stabilization coefficient, Clearance at which damping becomes zero: Specify: damping range

Specifying tangential damping

By default, the damping in the tangential direction is the same as the damping in the normal direction. However, if a lower or higher value is desired, you can decrease or increase the tangential damping or set it to zero.

Input File Usage:           


Interaction module: ABAQUS/Standard contact controls editor: Stabilization: Automatic stabilization or Stabilization coefficient, Tangent fraction: value

Contact controls associated with normal contact constraints

These controls allow you to specify that nodes on the contact interfaces can violate “hard” contact conditions. In addition, these controls can be used to modify the behavior of the augmented Lagrangian or penalty contact constraint enforcement. The “softened” and the no separation pressure-overclosure relationships cannot be modified by the contact controls.

A node can violate the contact condition in one of two ways. First, ABAQUS/Standard may consider that there is no contact at that node, even though the node has penetrated the master surface by a small distance. Second, ABAQUS/Standard may consider that there is contact at a node, even though the normal pressure transmitted between the contacting surfaces at the node is negative (that is, a tensile stress is being transmitted).

Specifying that tolerances for contact separation and penetration should be applied automatically

You can have ABAQUS/Standard automatically calculate separation and penetration tolerances. These tolerances are derived from the convergence tolerances currently active in the problem (see Convergence criteria for nonlinear problems, Section 7.2.3).

The automatic penetration tolerance is equal to twice the largest allowable displacement correction. The automatic separation tolerance, when multiplied by the area associated with the contact point, is set to 10 times the largest allowable residual during the first two iterations and is set to the largest allowable residual during any subsequent iteration. If convergence should occur in the first two iterations with these automatic tolerances, at least one more additional iteration is made, with the separation tolerance equal to the largest allowable residual. The objective of these automatic tolerances is to help with problems that exhibit contact chatter and normally require several iterations just to determine which nodes are in contact and which nodes are open.

Input File Usage:           


Interaction module: ABAQUS/Standard contact controls editor: toggle on Automatic overclosure tolerances

Directly specifying the maximum allowable penetration and tensile pressure

You can directly specify the maximum allowable penetration distance () and tensile contact pressure () that ABAQUS/Standard will accept without changing the contact status. You can also specify the number of nodes that are permitted to violate the default contact conditions in any increment. These controls are associated with the modified “hard” contact relationship, in which ABAQUS/Standard ignores insignificant changes in contact conditions. See Contact pressure-overclosure relationships, Section 30.1.2, for more information.

Modifying the behavior of the augmented Lagrangian or penalty contact constraint enforcement

For augmented Lagrangian contact you can specify the allowable penetration (either directly or as a fraction of a characteristic contact surface dimension) that is permitted to violate the impenetrability condition. In addition, for augmented Lagrangian or penalty contact you can scale the default penalty stiffness calculated by ABAQUS/Standard. Controls for the augmented Lagrange and penalty constraint enforcement methods are discussed in Constraint enforcement methods for ABAQUS/Standard contact pairs, Section 29.2.3.

Modifying the usage of the normal pressure contact Lagrange multiplier for contact constraint enforcement

You can directly specify the usage of the normal pressure contact Lagrange multiplier for contact constraint enforcement. Not using the Lagrange multiplier may lead to numerical problems when high penalty stiffness is used. However, the absence of the Lagrange multiplier may lead to more efficient solutions. For example, without the Lagrange multiplier the global stiffness matrix usually is positive definite in static linear elastic contact problems, while being just nonsingular otherwise. The matrix positive definiteness allows for more efficient equation reordering leading to reduced computational time and memory requirements during the solution of linear equation systems. Information on the default use of Lagrange multipliers and controls for modifying the defaults appears in Constraint enforcement methods for ABAQUS/Standard contact pairs, Section 29.2.3.

Contact controls associated with tangential contact constraints

By default, tangential contact constraints are applied as soon as contact is established. In most cases, this will yield satisfactory results and reasonable convergence. However, experience has shown that applying the normal constraint in the increment when contact is established and applying the tangential constraints in the subsequent increment can sometimes lead to improved convergence, particularly if frictional stresses have a strong effect on contact stresses.

In such cases you can change the default behavior to delay friction to the increments subsequent to the increment in which a contact point closes. This is not recommended if the contact zone changes rapidly as the analysis progresses; in that case, the absence of friction immediately after closure can lead to rapid, nonphysical oscillations in the frictional forces. See Application of frictional constraints during changes in contact state” in “Frictional behavior, Section 30.1.5, for information on controlling the onset of friction.

Efficiently accounting for changes in contact connectivity in the equation solver

In finite-sliding simulations a slave node may come into contact with any of the elements underlying the master surface. If the equation system is not allowed to change, an association has to be made between the slave node and all the master surface nodes, which may result in a large wavefront. This problem is compounded for three-dimensional deformable master surfaces with a large number of underlying elements. This may result in a wavefront so large that there is insufficient memory to solve the finite element equilibrium equations.

ABAQUS/Standard typically employs an “active topology” algorithm to efficiently treat connectivity changes during an analysis; however, ABAQUS/Standard will instead use a “contact patch” algorithm by default on a step-by-step basis under any of the following conditions:

User control over the choice of algorithms is available, but it is generally recommended that you allow ABAQUS/Standard to make this choice (see the active_topology parameter in Execution procedure for ABAQUS/Standard and ABAQUS/Explicit, Section 3.2.2, and Using the ABAQUS environment settings, Section 3.3.1). Both algorithms are automated. User control over the contact patch algorithm is sometimes needed for three-dimensional contact pairs, as discussed below.

Contact patch algorithm

The contact patch algorithm is rarely used and will most likely be removed in a future version of ABAQUS/Standard.

With the contact patch algorithm, the wavefront can be reduced by minimizing the allowable area of contact on the master surface per slave node during a given period of time. When a slave node slides off its contact patch, a new association between the slave node and the elements underlying the master surface in the immediate neighborhood has to be made; that is, a new contact patch is defined, the elements are reordered to optimize the wavefront, and the analysis is continued.

Figure 29.2.12–1 illustrates the concept of the contact patch for three-dimensional deformable-to-deformable contact simulations.

Figure 29.2.12–1 Definition of maximum slide distance.

The point on the master surface closest to each slave node is computed for the current geometry. The closest point is then used as the center of the sphere of radius R (maximum slide distance), as shown in Figure 29.2.12–1 for slave nodes 2 and 7. Any facet of the master surface that has at least one node inside this sphere will be part of the allowable area of contact for the slave node. For example, the allowable area of contact for slave node 2 in Figure 29.2.12–1 consists of facets 1, 2, 3, 11, 12, and 13; and the allowable area of contact for node 7 consists of facets 4 and 14.

When the contact patch algorithm is used, ABAQUS/Standard will, by default, select and adjust the contact patch size and position to reduce the analysis time. The initial patch size is selected as a small multiple of the master surface characteristic facet length. ABAQUS/Standard monitors the relative displacement increment size of each slave node. If the relative displacement increment is small compared to the contact patch, the contact patch may be reduced in size to obtain a more optimal wavefront. If the relative displacement increment is large compared to the contact patch, the patch size is increased to avoid frequent redefinition of contact patches and element reordering.

Adjusting the contact patch size

You can overwrite the patch size calculated by ABAQUS/Standard when the contact patch algorithm is used by specifying the maximum slide distance for finite-sliding simulations with three-dimensional deformable master surfaces. In this case the maximum slide distance and patch location will remain fixed until the maximum slide distance is respecified. The maximum slide distance must be applied to a particular contact pair. When a maximum slide distance is respecified for a contact pair, a new patch of the specified size is created around the point of contact at the beginning of the step. This is true even if the specified value of the slide distance remains the same. If a slide distance of zero is specified, the default (automatic) algorithm will be used from that point forward.

Specifying a maximum slide distance can be effective in reducing the wavefront if the relative motion of the slave and master surfaces is limited, such as may typically arise in “structural” contact problems and in cases of master surfaces with very few underlying elements where the whole surface should be included. However, each update of the contact patch entails significant cost, so fine tuning of the contact patch size can significantly affect analysis performance.

ABAQUS/Standard only uses the contact patch algorithm in the situations described above. Adjusting the slide distance control parameter associated with the contact patch algorithm does not invoke the contact patch algorithm. A warning message is issued if the slide distance control parameter is specified when the active topology algorithm is in effect (the slide distance control parameter has no affect on the active topology algorithm).

Input File Usage:           Use the following option to specify a maximum slide distance when the contact patch algorithm is used:
*CONTACT CONTROLS, SLIDE DISTANCE=maximum slide distance, 
MASTER=master surface, SLAVE=slave surface

ABAQUS/CAE Usage: Use the following input to specify a maximum slide distance when the contact patch algorithm is used:

Interaction module: ABAQUS/Standard contact controls editor: toggle on Specify slide distance: maximum slide distance

Restarting an analysis using the contact patch algorithm

If a slave node slips off its allowable area of contact, ABAQUS/Standard issues a warning message and forces a cutback. If the cutbacks cause ABAQUS/Standard to terminate the analysis, the problem can be restarted. In such a case you must end the analysis at the time of restart (see Truncating a step” in “Restarting an analysis, Section 9.1.1) and specify a different patch size to force ABAQUS/Standard to redefine the contact patches at the start of the restart analysis.