Contact Pair dialog box/Mechanical Contact Pair (Abaqus)

Name	Defines the name of the modeling object.
Label	Specifies a unique numerical identifier for the modeling object.
Contact Pair Parameter
Sliding Type	Lets you specify the sliding contact formulation to use.FiniteUses the finite sliding contact formulation.SmallUses the small sliding contact formulation. This corresponds to the SMALL SLIDING parameter for the *CONTACT PAIR keyword. See *CONTACT PAIR in the Abaqus Keywords Reference Guide for more information.
Symmetric	Lets you specify that you want to use two contact pairs comprised of the same two surfaces but in which the roles of the master and slave surfaces are reversed.With Node to surface contact, using symmetric master and slave surfaces can improve results and prevent penetration of the slave surface by nodes on the master surface. The increased accuracy with this technique, however, comes at the expense of increased computational time.For more information, see Using symmetric master-slave pairs to improve contact modeling in Defining contact pairs in Abaqus/Standard in the Abaqus Analysis Guide.
Tied	Lets you control whether the surfaces in the contact pair are tied together for the duration of the analysis.Select No if you do not want to tie the surfaces together.Select Yes to tie the surfaces together. This option corresponds to the TIED parameter for the *CONTACT PAIR keyword and is not allowed in cases of self-contact.Note: If you select Yes, you must specify a value for the Adjust option. For more information, see *CONTACT PAIR in the Abaqus Keywords Guide.
Adjust	Lets you specify a value by which you want the software to adjust the initial positions of the surfaces specified in this option. Abaqus makes these adjustments are made at the beginning of the analysis. These adjustments do not create any strain. This parameter is required for tied contact and is not allowed with self-contact. This option corresponds to the ADJUST parameter for the *CONTACT PAIR keyword. For more information, see *CONTACT PAIR in the Abaqus Keywords Guide.
HCRIT	Lets you specify the distance by which a point on the slave surface must penetrate the master surface before Abaqus abandons the current increment and tries again with a smaller increment. Note: This parameter does not apply to contact pairs that use the finite-sliding, surface-to-surface contact formulationThis option corresponds to the HCRIT parameter for the *CONTACT PAIR keyword. For more information, see *CONTACT PAIR in the Abaqus Keywords Guide.
Smooth	Set this parameter equal to the degree of smoothing used for deformable or rigid master surfaces for node-to-surface contact. The value given must lie between 0.0 and 0.5. This parameter only applies if you select Node to surface from the Type list.This option corresponds to the SMOOTH parameter for the *CONTACT PAIR keyword. For more information, see *CONTACT PAIR in the Abaqus Keywords Guide for more information.
Type	Controls how Abaqus generates the contact constraint coefficients.Node to surfaceGenerates the contact constraint coefficients according to the interpolation functions at the point where the slave node projects onto the master surface.Surface to surfaceGenerates contact constraint coefficients such that stress accuracy is optimized for the specified surface type pairings. This parameter setting is ignored for contact pairs that include a node-based surface.
Extension Zone	Lets you specify a value that is equal to a fraction of the end segment or facet edge length by which Abaqus extends the master surface to avoid numerical roundoff errors associated with contact modeling. Specify a value between 0.0 and 0.2. The default is 0.1. Note: This parameter affects only node-to-surface contact.This option corresponds to the EXTENSION ZONE parameter for the *CONTACT PAIR keyword. For more information, see *CONTACT PAIR in the Abaqus Keywords Guide for more information.
Ignore Surface Thickness Effects (Shell and Membrane)	Appears for Abaqus Structural, Axisymmetric Structural, and Coupled Thermal-Structural analyses.Lets you ignore the surface thickness effects in contact calculations. The check box only impacts contact formulations that account for surface thickness by default (it does not affect finite-sliding, node-to-surface contact).This check box corresponds to the Abaqus NO THICKNESS parameter for the *CONTACT PAIR keyword.
Surface Behavior Parameter
Surface Behavior	Lets you define an alternative contact pressure-overclosure relationship.HardSpecifies a pressure-overclosure relationship without physical softening. This option corresponds to the PRESSURE-OVERCLOSURE=HARD parameter for the *SURFACE BEHAVIOR keyword.Softened contact relationshipSpecifies a softened contact relationship. You can use a softened contact to model a soft, thin layer on one or both contact surfaces. You can also use it for numerical reasons as they make resolving the contact condition easier.No SeparationPrevents the separation of two surfaces once contact has been established. This option corresponds to the NO SEPARATION parameter for the *SURFACE BEHAVIOR keyword.
Enforcement Method	Appears when Surface Behavior is set to Hard.Lets you specify the penalty method that Abaqus uses to enforce the contact constraint.DefaultUses the default friction method.Augmented LagrangeUses the augmented Lagrange method for enforcement of the contact constraint. The Augmented Lagrange method uses the same kind of stiff approximation as the Penalty Linear and Penalty Nonlinear methods, but it also uses augmentation iterations to improve the accuracy of the approximation.Penalty LinearSpecifies the linear penalty method for enforcement of the contact constraint. With the Penalty Linear option, the penalty stiffness is constant, so the pressure-overclosure relationship is linear. When you select Penalty Linear, Abaqus sets the default penalty stiffness to 10 times a representative underlying element stiffness. You can also select the User Specified option from the Penalty Stiffness list to specify the stiffness and scaling factor.Penalty NonlinearSpecifies the nonlinear penalty method for enforcement of the contact constraint. With the Penalty Nonlinear option, the penalty stiffness increases linearly between regions of constant low initial stiffness and constant high final stiffness, resulting in a nonlinear pressure-overclosure relationship.DirectDirectly enforces a given pressure-overclosure behavior per contact constraint without approximation or the use of augmentation iterations.For more information, see Contact constraint enforcement methods in Abaqus/Standard in the Abaqus Analysis Guide.
Pressure-Overclosure type	Appears when Surface Behavior is set to Softened contact relationship.Lets you specify the constitutive models to use to control the motion of the surfaces in a mechanical contact analysis.LinearDefines a linear pressure-overclosure relationship. In a linear pressure-overclosure relationship, the surfaces transmit contact pressure when the overclosure between them, measured in the contact (normal) direction, is greater than zero. The linear pressure-overclosure relationship is identical to a tabular relationship with two data points, where the first point is located at the origin.With the Linear option, you specify the slope of the pressure-overclosure relationship (k).ExponentialDefines an exponential pressure-overclosure relationship. In an exponential contact pressure-overclosure relationship, the surfaces begin to transmit contact pressure once the clearance between them, measured in the contact (normal) direction, reduces toc0. The contact pressure transmitted between the surfaces then increases exponentially as the clearance continues to diminish.With the Exponential option, you specify the value of the contact pressure at zero clearance (p0 and the clearance at which the contact pressure is zero (c0).TabularDefines a piecewise linear pressure-overclosure relationship in a tabular form. In a tabular relationship, the surfaces transmit contact pressure when the overclosure between them, measured in the contact (normal) direction, is greater than h1, where h1 is the overclosure at zero pressure.With the Tabular option, you specify the data pairs (h1 and p1) of pressure versus overclosure (where overclosure corresponds to negative clearance). You must specify the data as an increasing function of pressure and overclosure.
Slope of pressure-closure relationship	Appears when Pressure-Overclosure type is set to Linear.Lets you specify the slope of the pressure-overclosure relationship (k).
Clearance at zero contact pressure	Appears when Pressure-Overclosure type is set to Exponential.Lets you specify the clearance at which the contact pressure is zero (c0).
Pressure at zero clearance	Appears when Pressure-Overclosure type is set to Exponential.Lets you specify the value of the contact pressure at zero clearance (p0.
Pressure vs. Overclosure Data	Appears when Pressure-Overclosure type is set to Tabular.Lets you specify the data pairs (h1 and p1) of pressure versus overclosure (where overclosure corresponds to negative clearance). You must specify the data as an increasing function of pressure and overclosure. You can select an existing field or create one.
Friction Parameter
Set Friction	Introduces friction properties into the analysis.
Friction	Lets you specify the type of friction to introduce.FrictionlessSpecifies that the interaction between the contacting bodies is frictionless.RoughSpecifies completely rough (no slipping) friction. This option corresponds to the ROUGH parameter for the *FRICTION keyword.Elastic SlipSpecifies elastic slip. This option corresponds to the ELASTIC SLIP parameter for the *FRICTION keyword.Use the Elastic Slip box to specify the absolute magnitude of the allowable elastic slip velocity (γi ) to be used in the stiffness method for sticking friction. In all other analysis procedures set this parameter equal to the absolute magnitude of the allowable elastic slip (γi) to be used in the stiffness method for sticking friction.Slip ToleranceSpecifies a tolerance value to control the maximum elastic slip.Use the Slip Tolerance box to specify the value of Ff. defined as the ratio of allowable maximum elastic slip velocity to angular velocity times the diameter of the spinning body in a steady-state transport analysis or as the ratio of allowable maximum elastic slip to characteristic contact surface face dimension in all other analysis procedures).This option corresponds to the SLIP TOLERANCE parameter for the *FRICTION keywordLagrangeSpecifies the Lagrange multiplier for friction. This option corresponds to the LAGRANGE parameter for the *FRICTION keyword.StaticSpecifies the static coefficient for friction.
Static Coefficient	Available if Friction is set to Elastic Slip, Slip Tolerance, Lagrange, or Static.Specifies the value of the friction coefficient, μ, for the *FRICTION keyword. For more information, see *FRICTION in the Abaqus Keywords Reference Guide.Note: If you use a formula field to specify a friction coefficient that depends on slip rate, contact pressure, and temperature, the field overrides the static coefficient value. A warning message appears in the .diag file when you solve the model. For more information, see Slip-Rate, Contact Pressure and Temperature Dependent Friction below.
Coulomb Friction Model
Appears when Friction is set to Elastic Slip, Skip Tolerance, or Lagrange.
Coulomb Friction Type	Specifies the material behavior. Isotropic is available for Structural analyses.
Isotropic Coulomb Friction Model
Appears when Friction is set to Elastic Slip, Skip Tolerance, or Lagrange and Coulomb Friction Type is set to Isotropic.
Friction Coefficient Dependence	Specifies the friction coefficient for contact surfaces as dependent on slip rate, contact pressure, and temperature. The only value is Slip-Rate, Contact Pressure and Temperature Dependent Friction.
Slip-Rate, Contact Pressure and Temperature Dependent Friction	Specifies a friction coefficient that is dependent on slip rate, contact pressure, and temperature.Create or use an existing formula field to define the values for slip rate, contact pressure, and temperature, where:Slip-Rate: \gamma eqContact Pressure: pAverage temperature: \ThetaAverage temperature at the contact point between the two contact surfaces. If you do not enter a value, the software assumes the friction coefficient is independent of that value. For example, if you do not specify average temperature, the software assumes the friction coefficient is independent of average temperature. For more information about formula fields, see Formula fields.
Surface-Based Cohesive Behavior Properties
Include Cohesive Behavior	Includes surface-based cohesive behavior in the analysis.
Specify Cohesive Behavior	Lets you select the Cohesive Behavior modeling object to define surface-based cohesive behavior in a contact analysis.For more information, see Surface Based Coupling (Abaqus).
Include Damage Initiation	Includes material properties that define the initiation of damage for cohesive surfaces.
Specify Damage Initiation	Lets you select the Damage Initiation modeling object to specify material properties that define the initiation of damage for cohesive surfaces.For more information, see Defining damage modeling for Abaqus cohesive behavior.
Include Damage Evolution	Includes material properties that define the evolution of damage leading to eventual failure.
Specify Damage Evolution	Lets you select the Damage Evolution modeling object to specify material properties that define the evolution of damage leading to eventual failure.For more information, see Defining damage modeling for Abaqus cohesive behavior.
Specify Damage Stabilization	Includes viscosity coefficients used in the viscous regularization scheme for the damage model.
Specify Viscous Regulation	Lets you select the Damage Stabilization modeling object to specify viscosity coefficients used in the viscous regularization scheme for the damage model.For more information, see Defining damage modeling for Abaqus cohesive behavior.

Learn more

Defining contact pairs (Abaqus Structural and Thermal analyses)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Contact Pair dialog box/Mechanical Contact Pair (Abaqus), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });