Products: Abaqus/Standard Abaqus/CAE
“Defining surface-to-surface contact,” Section 15.13.6 of the Abaqus/CAE User's Manual
“Defining self-contact,” Section 15.13.7 of the Abaqus/CAE User's Manual
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;
can be used for problems where the standard controls do not effectively establish the desired contact conditions; and
can be used in some situations to control whether supplementary contact constraints are created.
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.
In addition, you can specify supplementary contact constraints on individual contact pairs as described below in “Supplementary contact constraints.”
| Input File Usage: | To apply contact controls to all contact pairs and contact elements: |
*CONTACT CONTROLS 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: Interaction |
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: |
*CONTACT CONTROLS, RESET To reset the controls for a specific contact pair: *CONTACT CONTROLS, SLAVE=slave surface, MASTER=master surface, RESET |
| Abaqus/CAE Usage: | Interaction module: contact interaction editor: Contact controls: (Default) |
You cannot reset all contact controls at once in Abaqus/CAE. |
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 33.1.3). 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.
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: | *CONTACT CONTROLS, APPROACH, MASTER=master surface, 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. |
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: |
*CONTACT CONTROLS, STABILIZE To specify a scale factor for the default damping coefficient: *CONTACT CONTROLS, STABILIZE=factor To specify the damping coefficient directly: *CONTACT CONTROLS, STABILIZE damping coefficient |
| Abaqus/CAE Usage: | Interaction module: Abaqus/Standard contact controls editor: Stabilization: Automatic stabilization, Factor: factor or Stabilization coefficient: damping coefficient |
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: | *CONTACT CONTROLS, STABILIZE , ramp-down factor |
| Abaqus/CAE Usage: | Interaction module: Abaqus/Standard contact controls editor: Stabilization: Automatic stabilization or Stabilization coefficient, Fraction of damping at end of step: ramp-down factor |
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: | *CONTACT CONTROLS, STABILIZE , , damping range |
| Abaqus/CAE Usage: | Interaction module: Abaqus/Standard contact controls editor: Stabilization: Automatic stabilization or Stabilization coefficient, Clearance at which damping becomes zero: Specify: damping range |
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: | *CONTACT CONTROLS, STABILIZE, TANGENT FRACTION=value |
| Abaqus/CAE Usage: | Interaction module: Abaqus/Standard contact controls editor: Stabilization: Automatic stabilization or Stabilization coefficient, Tangent fraction: value |
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 “softened” pressure-overclosure relationships and the augmented Lagrangian or penalty contact constraint enforcement. 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).
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: | *CONTACT CONTROLS, AUTOMATIC TOLERANCES |
| Abaqus/CAE Usage: | Interaction module: Abaqus/Standard contact controls editor: toggle on Automatic overclosure tolerances |
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 33.1.2, for more information.
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 “Contact constraint enforcement methods in Abaqus/Standard,” Section 34.1.2.
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 “Contact constraint enforcement methods in Abaqus/Standard,” Section 34.1.2.
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 33.1.5, for information on controlling the onset of friction.
The penalty stiffness used to enforce tangential constraints in linear perturbation steps generally differs from the penalty stiffness used to enforce sticking in a general step. In perturbation steps Abaqus/Standard activates the tangential contact constraints when the corresponding normal constraint is active in the base state and the contact property (surface interaction) definition includes a friction model. By default, the tangential penalty stiffness is equal to the default normal penalty stiffness.
You can scale the tangential penalty stiffness to simulate sticking/slipping conditions on a step-by-step basis. This scaling only affects the perturbation step in which it is specified; it will not carry over to subsequent steps. If you want the same scale factor applied in a series of perturbation steps, you must specify the scale factor explicitly in each step.
Some procedures that rely on a frequency analysis, such as complex frequency analysis and subspace-based steady-state dynamic analysis, are influenced by the scaling of the tangential stiffness that was in effect for the prior frequency analysis and the scaling of the tangential stiffness that is in effect for these steps. In such cases consistent scaling is recommended for these steps. For other mode-based procedures based on a frequency analysis, the scaling of the tangential stiffness is ignored and only the effect of the previous frequency analysis is considered.
| Input File Usage: | To modify the tangential penalty stiffness for all contact pairs in a linear perturbation step: |
*CONTACT CONTROLS, PERTURBATION TANGENT SCALE FACTOR=factor To modify the tangential penalty stiffness for a specific contact pair in a linear perturbation step: *CONTACT CONTROLS, PERTURBATION TANGENT SCALE FACTOR=factor, SLAVE=slave surface, MASTER=master surface |
| Abaqus/CAE Usage: | Modifying the tangential penalty stiffness in linear perturbation steps is not supported in Abaqus/CAE. |
Supplementary contact constraints are sometimes helpful for improving convergence behavior or for improving the smoothness and accuracy of the contact pressure and underlying element stress. Supplementary constraints are applicable if all of the following circumstances apply to your model:
A contact formulation other than finite-sliding, surface-to-surface contact is used.
A softened pressure-overclosure relationship is specified or the penalty or augmented Lagrange contact enforcement method is used.
The slave surface of the contact pair is based on a second-order element type except in the following cases:
The slave surface is based on modified 10-node tetrahedral elements (C3D10M, etc.) and the small-sliding, surface-to-surface formulation is used.
The slave surface is based on two-dimensional elements with three-node facets and the small sliding, surface-to-surface formulation is used.
The slave surface is based on modified 6-node triangular elements (CPS6M, etc.) with any contact formulation.
| Input File Usage: | *CONTACT PAIR, INTERACTION=interaction_property_name, SUPPLEMENTARY CONSTRAINTS=SELECTIVE slave_surface_name, master_surface_name |
Use the following option to add the supplementary contact constraints: *CONTACT PAIR, INTERACTION=interaction_property_name, SUPPLEMENTARY CONSTRAINTS=YES slave_surface_name, master_surface_name Use the following option to forgo the supplementary contact constraints: *CONTACT PAIR, INTERACTION=interaction_property_name, SUPPLEMENTARY CONSTRAINTS=NO slave_surface_name, master_surface_name |
| Abaqus/CAE Usage: | For contact formulations other than the finite-sliding, surface-to-surface formulation: |
Interaction module: Create Interaction: Surface-to-surface contact (Standard): select the master surface; click Surface; select the slave surface; Interaction editor; Use supplementary contact points: Selectively, Always, or Never; Contact interaction property: interaction_property_name |
