The contact property editor contains the following menus from which you can choose options to include in the property definition:
Mechanical; see “Defining mechanical contact property options.”
Thermal; see “Defining thermal contact property options.”
Electrical; see “Defining electrical contact property options.”
The Contact Property Options list at the top of the editor displays the options currently included in the property definition; the list is updated as you add and delete options. You can add, delete, or change property options as follows:
Adding property options
Select the options needed to define your property from the Mechanical, Thermal, and Electrical menus. When you select an option, its name appears in the Contact Property Options list, and data fields associated with the option appear in the data area in the bottom half of the editor. Use the data fields to enter information for the currently selected option.
Deleting property options
In the Contact Property Options list, select the option that you want to delete, and click Delete on the right side of the editor. This procedure removes the option from both the options list and the property definition.
Changing option data
In the Contact Property Options list, select the option whose data you want to change. When the data fields associated with the option appear in the bottom half of the window, change the information that you have entered for the option as desired.
You can define mechanical contact property options to specify tangential behavior (friction and elastic slip), normal behavior (hard, soft, or damped contact and separation), and damping due to friction. The following sections describe how to specify the mechanical contact property models:
“Specifying frictional behavior for mechanical contact property options”
“Specifying pressure-overclosure relationships for mechanical contact property options”
“Specifying damping for mechanical contact property options”
“Specifying cohesive behavior properties for mechanical contact property options”
“Specifying cohesive damage properties for mechanical contact property options”
“Specifying fracture criterion properties for crack propagation”
“Specifying geometric properties for mechanical contact property options”
You can specify a friction model that defines the force resisting the relative tangential motion of the surfaces in a mechanical contact analysis. For more information, see “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
To specify frictional behavior:
From the main menu bar, select Interaction
PropertyCreate.
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,” Section 3.2.1.
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 MechanicalTangential Behavior.
In the editor that appears, click the arrow to the right of the Friction formulation field, and select how you want to define friction between the contact surfaces:
Select Frictionless if you want Abaqus to assume that surfaces in contact slide freely without friction.
Select Penalty to use a stiffness (penalty) method that permits some relative motion of the surfaces (an “elastic slip”) when they should be sticking. While the surfaces are sticking (i.e., 
), the magnitude of sliding is limited to this elastic slip. Abaqus will continually adjust the magnitude of the penalty constraint to enforce this condition. For more information, see “Stiffness method for imposing frictional constraints in Abaqus/Standard” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide, and “Stiffness method for imposing frictional constraints in Abaqus/Explicit” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
Select Static-Kinetic Exponential Decay to specify static and kinetic friction coefficients directly. In this model it is assumed that the friction coefficient decays exponentially from the static value to the kinetic value. Alternatively, you can enter test data to fit the exponential model. (This Friction formulation option also allows you to specify elastic slip.) For more information, see “Specifying static and kinetic friction coefficients” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
Select Rough to specify an infinite coefficient of friction. For more information, see “Preventing slipping regardless of contact pressure” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
Select Lagrange Multiplier (Standard only) to enforce the sticking constraints at an interface between two surfaces using the Lagrange multiplier implementation. With this method there is no relative motion between two closed surfaces until 
. For more information, see “Lagrange multiplier method for imposing frictional constraints in Abaqus/Standard” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
Select User-defined to define the shear interaction between the contact surfaces with user subroutine FRIC or VFRIC. For more information, see “User-defined friction model” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
If you selected the Penalty or Lagrange Multiplier (Standard only) friction formulation, perform the following steps:
Display the Friction tabbed page.
Choose the Directionality:
Choose Isotropic to enter a uniform friction coefficient.
Choose Anisotropic (Standard only) to allow for different friction coefficients in the two orthogonal directions on the contact surface. For more information, see “Using the anisotropic friction model in Abaqus/Standard” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
Toggle on Use slip-rate-dependent data if the friction coefficient is dependent on slip rate.
Toggle on Use contact-pressure-dependent data if the friction coefficient is dependent on the contact pressure.
Toggle on Use temperature-dependent data if the friction coefficient is dependent on temperature.
Click the arrows to the right of the Number of field variables field to specify the number of field variables on which the friction coefficient depends.
Enter the required data in the data table provided.
Display the Shear Stress tabbed page, and choose a Shear stress limit option:
Choose No limit if you do not want to limit the shear stress that can be carried by the interface before the surfaces begin to slide.
Choose Specify to enter an equivalent shear stress limit, 
. If you choose this option, sliding will occur if the magnitude of the equivalent shear stress reaches this value, regardless of the magnitude of the contact pressure stress. For more information, see “Using the optional shear stress limit” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
If you selected the Penalty friction formulation, display the Elastic Slip tabbed page, and specify how you want to define elastic slip:
If you are performing an Abaqus/Standard analysis, choose an option to Specify maximum elastic slip:
Choose Fraction of characteristic surface dimension to calculate the allowable elastic slip as a small fraction of the characteristic contact surface length.
Choose Absolute distance to enter the absolute magnitude of the allowable elastic slip, 
. (For a steady-state transport analysis set this parameter equal to the absolute magnitude of the allowable elastic slip velocity (
) to be used in the stiffness method for sticking friction.)
If you are performing an Abaqus/Explicit analysis, choose an Elastic slip stiffness option:
Choose Infinite (no slip) to deactivate shear softening.
Choose Specify to activate softened tangential behavior. Enter the slope of the curve that defines the shear traction as a function of the elastic slip between the two surfaces.
For more information, see “Shear stress versus elastic slip while sticking” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
If you selected the Static-Kinetic Exponential Decay friction formulation, perform the following steps:
Display the Friction tabbed page.
Choose an option for defining the exponential decay friction model:
Choose Coefficients to provide the static friction coefficient, the kinetic friction coefficient, and the decay coefficient directly.
Choose Test data to provide test data points to fit the exponential model.
If you selected the Coefficients definition option, enter the following in the data table provided:
Static friction coefficient, 
.
Kinetic friction coefficient, 
.
Decay coefficient, 
.
If you selected the Test data definition option, enter the following in the data table provided:
In the first row, enter the static friction coefficient, 
.
In the second row, enter the dynamic friction coefficient, 
and the reference slip rate, 
, at which is measured.
In the third row, enter the kinetic friction coefficient, 
. This value corresponds to the asymptotic value of the friction coefficient at infinite slip rate, 
. If this data line is omitted, Abaqus/Standard automatically calculates such that 
.
Display the Elastic Slip tabbed page, and specify how you want to define elastic slip:
If you are performing an Abaqus/Standard analysis, choose an option to Specify maximum elastic slip:
Choose Fraction of characteristic surface dimension to calculate the allowable elastic slip as a small fraction of the characteristic contact surface length.
Choose Absolute distance to enter the absolute magnitude of the allowable elastic slip, . (For a steady-state transport analysis set this parameter equal to the absolute magnitude of the allowable elastic slip velocity () to be used in the stiffness method for sticking friction.)
If you are performing an Abaqus/Explicit analysis, choose an Elastic slip stiffness option:
Choose Infinite (no slip) to deactivate shear softening.
Choose Specify to activate shear softening. Enter the slope of the curve that defines the shear traction as a function of the elastic slip between the two surfaces.
For more information, see “Shear stress versus elastic slip while sticking” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
If you selected the User-defined friction formulation, perform the following steps:
Click the arrows to the right of the Number of state-dependent variables field to indicate the number state variables that will be defined in user subroutine FRIC or VFRIC.
In the Friction Properties table, enter the values of properties needed by user subroutine FRIC or VFRIC. (For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.)
For more information, see “User-defined friction model” in “Frictional behavior,” Section 37.1.5 of the Abaqus Analysis User's Guide.
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.
You can define a constitutive model for the contact pressure-overclosure relationship that governs the motion of the surfaces in a mechanical contact analysis. For more information, see “Contact pressure-overclosure relationships,” Section 37.1.2 of the Abaqus Analysis User's Guide.
To specify contact pressure-overclosure relationships:
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,” Section 3.2.1.
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,” Section 38.2.3 of the Abaqus Analysis User's Guide. To specify these settings, select an option from the Constraint enforcement method list and do the following:
Select Default to enforce constraints using a contact pressure-overclosure relationship.
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.
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” in “Contact constraint enforcement methods in Abaqus/Standard,” Section 38.1.2 of the Abaqus Analysis User's Guide.
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 
, which is equal to the scale factor times the characteristic contact facet length, in the Upper quadratic limit scale factor field.
Enter the ratio (
–
)/(–) that defines the lower quadratic limit in the Lower quadratic limit ratio field.
Specify the Clearance at which contact pressure is zero. The default value is 0.
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:
Enter the contact pressure at zero clearance, 
, and the clearance at which the contact pressure is zero, , in the data table.
Specify the limit on the contact stiffness that the model can attain, 
(applies only for Abaqus/Explicit analyses).
Choose Infinite (no slip) to set 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:
To define the overclosure measure as a percentage of the minimum element size, select factor in the Overclosure field and enter a positive value 
.
To define the overclosure measure directly, select measure in the Overclosure field and enter a positive value .
Enter a value, 
, greater than one to define the geometric scaling of the “base” stiffness in the Contact stiffness scale factor field.
Enter a positive value 
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.
You can define a damping model that defines forces resisting the relative motions of the contacting surfaces in a mechanical contact analysis. For more information, see “Contact damping,” Section 37.1.3 of the Abaqus Analysis User's Guide.
To specify contact damping:
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,” Section 3.2.1.
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 MechanicalDamping.
In the editor that appears, click the arrow to the right of the Definition field, and select an option for determining the dimensionality of the damping coefficient:
Select Damping coefficient to specify the damping coefficient with units of pressure per relative velocity. For more information, see “Specifying the damping coefficient such that the damping force is directly proportional to the rate of relative motion between the surfaces” in “Contact damping,” Section 37.1.3 of the Abaqus Analysis User's Guide.
Select Critical damping fraction (Explicit only) to specify a unitless damping coefficient in terms of the fraction of critical damping associated with the contact stiffness; this method is available only for Abaqus/Explicit. For more information, see “Specifying the damping coefficient as a fraction of critical damping in Abaqus/Explicit” in “Contact damping,” Section 37.1.3 of the Abaqus Analysis User's Guide.
Choose an option for specifying the Tangent fraction (the ratio of the tangential damping coefficient to the normal damping coefficient):
Choose Use default to accept the default tangent fraction value. For Abaqus/Standard the default is 0.0, so the damping coefficient for the tangential direction is zero. For Abaqus/Explicit the default value for the tangent fraction is 1.0, so the damping coefficient for the tangential direction is equal to the damping coefficient for the normal direction.
Choose Specify value to enter a value for the tangent fraction.
Choose a shape for the curve that describes the relationship between clearance and the damping coefficient:
Choose Step (Explicit only) if you are performing an Abaqus/Explicit analysis. The damping coefficient will remain at the specified constant value while the surfaces are in contact and at zero otherwise.
Choose Linear (Standard only) to define a damping coefficient that increases linearly from zero at a particular clearance value () to its full value when the surfaces are in contact.
Choose Bilinear (Standard only) to define a damping coefficient that increases linearly from zero at a particular clearance value () to its full value when clearance has been reduced to another value (
). As clearance continues to decrease from to zero, the damping coefficient remains constant at its full value.
Enter the appropriate data in the table provided:
If you are performing an Abaqus/Explicit analysis, enter a value for the damping coefficient or for the critical damping fraction (depending on your selection in Step 5.)
If you are performing an Abaqus/Standard analysis and selected Linear (Standard only) in the previous step, enter the following:
In the first row, enter a value for the damping coefficient.
In the second row, enter a value for , the clearance at which the damping coefficient is zero.
If you are performing an Abaqus/Standard analysis and selected Bilinear (Standard only) in the previous step, enter the following:
In the first row, enter a value for the damping coefficient.
In the second row, enter a value for , the clearance at which the damping coefficient reaches its full value.
In the third row, enter a value for , the clearance at which the damping coefficient is zero.
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.
You can define cohesive behavior properties that are accounted for in surface contact interactions. For more information, see “Surface-based cohesive behavior,” Section 37.1.10 of the Abaqus Analysis User's Guide.
In addition, you complete the definition of a crack propagation capability by defining a fracture-based cohesive behavior surface interaction. You activate the crack propagation by assigning it to the pair of surfaces that are initially partially bonded. If the fracture criterion is met, crack propagation occurs between these two surfaces. Cohesive behavior is also used to specify the elastic behavior of the bonds.
To specify cohesive behavior contact properties:
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,” Section 3.2.1.
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 MechanicalCohesive Behavior.
Toggle on Allow cohesive behavior during repeated post-failure contacts to modify the default post-failure behavior when progressive damage has been defined. By default, cohesive behavior is not enforced for nodes on the slave surface once ultimate failure has occurred at those nodes. When this option is toggled on, Abaqus/CAE enforces cohesive behavior for recurrent contacts at nodes on the slave surface subsequent to ultimate failure.
From the Eligible Slave Nodes options, select one of the following:
Select Any slave nodes experiencing contact to define cohesive behavior not only for all nodes of the slave surface that are in contact with the master surface at the start of a step, but also for slave nodes that are not initially in contact but may come in contact during the course of a step.
Select Only slave nodes initially in contact to restrict cohesive behavior to only those nodes of the slave surface that are in contact with the master surface at the start of a step.
Select Specify the bonding node set in the surface-to-surface Std interaction to restrict cohesive behavior to a subset of slave nodes defined when you specify initial bonded contact conditions. This option is available only for Abaqus/Standard analyses.
From the Traction-separation Behavior options, accept the default contact penalty enforcement method or toggle on Specify stiffness coefficients and perform the following additional steps:
Specify whether you want to specify stiffness coefficients for Uncoupled or Coupled traction behavior.
Toggle on Use temperature-dependent data if the traction-separation behavior is dependent on temperature.
Click the arrows to the right of the Number of field variables field to specify the number of field variables on which the traction-separation behavior depends.
Enter the required data in the data table provided.
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.
You can define damage initiation, evolution, and stabilization properties that will be accounted for in surface contact interactions. For more information, see “Surface-based cohesive behavior,” Section 37.1.10 of the Abaqus Analysis User's Guide.
To specify damage properties for mechanical contact:
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,” Section 3.2.1.
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 MechanicalDamage.
From the Initiation tabbed page, perform the following steps:
From the Criterion list, choose one of the following:
Select Maximum nominal stress to specify a damage initiation criterion based on the maximum nominal stress criterion for cohesive elements.
Select Maximum separation to specify a damage initiation criterion based on the maximum separation value.
Select Quadratic traction to specify a damage initiation criterion based on the quadratic traction–interaction criterion for cohesive elements.
Select Quadratic separation to specify a damage initiation criterion based on the quadratic separation–interaction criterion for cohesive elements.
Toggle on Use temperature-dependent data if the damage initiation behavior is dependent on temperature.
Click the arrows to the right of the Number of field variables field to specify the number of field variables on which the damage initiation behavior depends.
Enter the required data in the data table provided.
If you want to specify damage evolution criteria; toggle on Specify damage evolution, click the Evolution tab, and perform the following steps:
From the Type options, select one of the following:
Select Displacement to define the evolution of damage as a function of the total displacement (for elastic materials in cohesive elements) or the plastic displacement (for bulk elastic-plastic materials) after the initiation of damage.
Select Energy to define the evolution of damage in terms of the energy required for failure (fracture energy) after the initiation of damage.
From the Softening options, select one of the following:
Select Linear to specify a linear softening stress-strain response (after the initiation of damage) for linear elastic materials or a linear evolution of the damage variable with deformation (after the initiation of damage) for elastic-plastic materials.
Select Exponential to specify an exponential softening stress-strain response (after the initiation of damage) for linear elastic materials or an exponential evolution of the damage variable with deformation (after the initiation of damage) for elastic-plastic materials.
Select Tabular to specify the evolution of the damage variable with deformation (after the initiation of damage) in tabular form. This option is available only for damage evolution defined in terms of displacement.
If you want to specify mode-dependent behavior, toggle on Specify mixed mode behavior and select one of the following options:
Select Tabular to specify the fracture energy or displacement (total or plastic) directly as a function of the shear-normal mode mix for cohesive elements. This method must be used to specify the mixed-mode behavior for cohesive elements when damage evolution is defined in terms of displacement.
Select Power law to specify the fracture energy as a function of the mode mix by means of a power law mixed-mode fracture criterion.
Select Benzeggagh-Kenane to specify the fracture energy as a function of the mode mix by means of the Benzeggagh-Kenane mixed-mode fracture criterion.
If you specified Tabular for the mixed mode behavior, select one of the following:
Select Energy to define the mode mix in terms of a ratio of fracture energy in the different modes.
Select Traction to define the mode mix in terms of a ratio of traction components.
If you toggled on Specify mixed mode behavior and selected either Power law or Benzeggagh-Kenane as the fracture criterion, you can specify the exponent in the power law or the Benzeggagh-Kenane criterion that defines the variation of fracture energy with mode mix for cohesive elements. Toggle on Specify power-law/criterion and enter a value for the exponent in the field.
Toggle on Use temperature-dependent data if the damage evolution behavior is dependent on temperature.
Click the arrows to the right of the Number of field variables field to specify the number of field variables on which the damage evolution behavior depends.
Enter the required data in the data table provided.
If you want to specify viscous regularization of the constitutive equations defining surface-based cohesive behavior; toggle on Specify damage stabilization, click the Stabilization tab, and specify a viscosity coefficient.
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.
You can specify the fracture criterion that is used to model crack propagation using the virtual crack closure technique (VCCT) in an Abaqus/Standard model. The fracture criterion specifies the critical energy release rates. For more information, see “Crack propagation analysis,” Section 11.4.3 of the Abaqus Analysis User's Guide.
To specify fracture criterion properties for crack propagation:
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,” Section 3.2.1.
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 MechanicalFracture Criterion.
Select the Type of criterion for crack propagation along initially partially bonded surfaces—the virtual crack closure technique (VCCT) criterion or the enhanced virtual crack closure technique (Enhanced VCCT) criterion. The virtual crack closure techniques are available only in an Abaqus/Standard analysis.
If you are using the crack propagation criterion in an enriched region, choose the direction of crack growth relative to the local 1-direction when the fracture criterion is satisfied. The crack can extend at a direction normal to the direction of the maximum tangential stress (default), normal to the element local 1-direction, or parallel to the element local 1-direction.
Select the mixed mode behavior:
Select BK to specify the fracture energy as a function of the mode mix by means of the Benzeggagh-Kenane mixed mode fracture criterion.
Select Power to specify the fracture energy as a function of the mode mix by means of a power law mixed mode fracture criterion.
Select Reeder to specify the fracture energy as a function of the mode mix by means of the Reeder mixed mode fracture criterion.
If desired, specify the tolerance within which the crack propagation criterion must be satisfied. The default is 0.2.
If desired, specify the tolerance within which the unstable crack propagation criterion must be satisfied to allow multiple nodes at and ahead of the crack tip to debond without cutting back the increment size in one increment when the VCCT criterion is satisfied for an unstable crack problem. The default value is infinity.
If desired, specify the viscosity coefficient used in the viscous regularization. The default value is 0.0.
If you selected VCCT for the type of fracture criterion, define the energy release rates (for both crack onset and crack propagation) at each mode: 
, 
, and 
.
If you selected Enhanced VCCT for the type of fracture criterion, do the following:
Define the energy release rates for crack onset at each mode: , , and .
Define the energy release rates for crack propagation at each mode: 
, 
, and 
.
If you selected either Reeder or BK as the fracture criterion, define the exponent in the Reeder law or the Benzeggagh-Kenane model, 
.
If you selected Power as the fracture criterion, define the three exponents in the power law model, 
, 
, and 
.
Toggle on Use temperature-dependent data if the fracture criterion is dependent on temperature.
Click the arrows to the right of the Number of field variables field to specify the number of field variables on which the fracture criterion depends.
Enter the required data in the data table provided.
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.
You can define additional geometric properties that will be accounted for in surface contact interactions.
To specify geometric contact properties:
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,” Section 3.2.1.
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 MechanicalGeometric Properties.
If you are performing an Abaqus/Standard analysis, you can specify an out-of-plane surface thickness for two-dimensional models or a cross-sectional area for every node on a node-based surface. Enter this value in the Out-of-plane surface thickness or cross-sectional area (Standard) field.
If you are performing an Abaqus/Explicit analysis, you can specify the thickness of an interfacial layer between the two interacting surfaces. Toggle on Thickness of interfacial layer (Explicit), and enter the thickness.
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.
You can define thermal contact property options to specify thermal conductance, heat generation, and thermal radiation due to friction. The following sections describe how to specify the thermal contact property models:
You can specify thermal conductance to define conductive heat transfer between closely adjacent (or contacting) surfaces. For more information, see “Modeling conductance between surfaces” in “Thermal contact properties,” Section 37.2.1 of the Abaqus Analysis User's Guide.
To specify thermal conductance:
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,” Section 3.2.1.
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 ThermalThermal Conductance.
The Edit Contact Property dialog box appears.
In the editor that appears, click the arrow to the right of the Definition field, and select an option for defining thermal conductance:
Select Tabular to enter data relating thermal conductance to the clearance or pressure between the contact surfaces.
Select User-defined to define thermal conductance in user subroutine GAPCON. If you select this option, skip to Step 9.
Indicate whether you want to define thermal conductance as a function of the clearance between the surfaces, the contact pressure between the surfaces, or both.
If you want to define thermal conductance as a function of clearance, display the Clearance Dependency tabbed page, and do the following:
Toggle on Use temperature-dependent data if the data are dependent on temperature.
Toggle on Use mass flow rate-dependent data (Standard only) if the data are dependent on the average mass flow rate per unit area, 
.
Click the arrows to the right of the Number of field variables field to specify the number of field variables on which the data depend.
In the data table, define thermal conductance as a function of gap clearance.
The tabular data must start at zero clearance (closed gap) and define thermal conductance as clearance increases. You must provide at least two pairs of points. The value of thermal conductance drops to zero immediately after the last data point, so there is no conductance when the clearance is greater than the value corresponding to the last data point. If conductance is not also defined as a function of contact pressure, it will remain constant at the zero clearance value for all pressures.
If you want to define thermal conductance as a function of contact pressure, display the Pressure Dependency tabbed page, and do the following:
Toggle on Use temperature-dependent data if the data are dependent on temperature.
Toggle on Use mass flow rate-dependent data (Standard only) if the data are dependent on the average mass flow rate per unit area, .
Click the arrows to the right of the Number of field variables field to specify the number of field variables on which the data depend.
In the data table, define thermal conductance as a function of contact pressure at the interface.
The tabular data must start at zero contact pressure (or, in the case of contact that can support a tensile force, the data point with the most negative pressure) and define thermal conductance as pressure increases. The value of thermal conductance remains constant for contact pressures outside of the interval defined by the data points. If conductance is not also defined as a function of clearance, it is zero for all positive values of clearance and discontinuous at zero clearance
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.
You can specify heat generation due to the dissipation of energy created by the mechanical or electrical interaction of contacting surfaces. For more information, see “Modeling heat generated by nonthermal surface interactions” in “Thermal contact properties,” Section 37.2.1 of the Abaqus Analysis User's Guide.
To specify heat generation:
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,” Section 3.2.1.
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 ThermalHeat Generation.
In the editor that appears, specify the Fraction of dissipated energy caused by friction or electric currents that is converted to heat:
Choose Use default (1.0) to convert all of the dissipated energy to heat.
Choose Specify to enter the fraction of your choice.
Specify the Fraction of converted heat distributed to slave surface:
Choose Use default (0.5) to distribute the heat equally between the master and slave surfaces.
Choose Specify to enter the fraction of the heat to be distributed to the slave surface. The remaining fraction will be distributed to the master surface.
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.
You can specify radiative heat transfer between closely adjacent surfaces. For more information, see “Modeling radiation between surfaces when the gap is small” in “Thermal contact properties,” Section 37.2.1 of the Abaqus Analysis User's Guide.
To specify radiation:
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,” Section 3.2.1.
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 ThermalRadiation.
In the editor that appears, enter values for the emissivity, 
, of the master and slave surfaces.
In the table provided, define the view factor as a function of clearance.
The view factor should have a value between 0.0 and 1.0. At least two pairs of points are required. The tabular data must start at zero clearance (closed gap) and define the view factor as the clearance increases. The value of the view factor drops to zero immediately after the last data point, so there is no radiative heat transfer when the clearance is greater than the value corresponding to the last data point.
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.
You can define electrical contact property options to specify gap conductance.
You can specify gap conductance between closely adjacent or contacting surfaces. The conductance is proportional to the difference in electric potentials across the interface. The conduction is a function of the clearance (separation) between the surfaces and can be a function of the contact pressure. For more information, see “Electrical contact properties,” Section 37.3.1 of the Abaqus Analysis User's Guide.
To specify electrical gap conductance:
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,” Section 3.2.1.
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 ElectricalElectrical Conductance.
The Edit Contact Property dialog box appears.
In the editor that appears, click the arrow to the right of the Definition field, and select an option for defining electrical conductance:
Select Tabular to enter data relating electrical conductance to the separation between the contact surfaces.
Select User-defined to define the conductance in user subroutine GAPELECTR. If you select this option, skip to Step 9.
Indicate whether you want to define electrical conductance as a function of the clearance between the surfaces, the contact pressure between the surfaces, or both.
If you want to define electrical conductance as a function of clearance, display the Clearance Dependency tabbed page, and do the following:
Toggle on Use temperature-dependent data if the data are dependent on temperature.
Click the arrows to the right of the Number of field variables field to specify the number of field variables on which the data depend.
In the data table, define electrical conductance as a function of gap clearance.
The tabular data must start at zero clearance (closed gap) and define electrical conductance as clearance increases. You must provide at least two pairs of points. The value of electrical conductance drops to zero immediately after the last data point, so there is no conductance when the clearance is greater than the value corresponding to the last data point. If conductance is not also defined as a function of contact pressure, it will remain constant at the zero clearance value for all pressures.
If you want to define electrical conductance as a function of contact pressure, display the Pressure Dependency tabbed page, and do the following:
Toggle on Use temperature-dependent data if the data are dependent on temperature.
Click the arrows to the right of the Number of field variables field to specify the number of field variables on which the data depend.
In the data table, define electrical conductance as a function of contact pressure at the interface.
The tabular data must start at zero contact pressure (or, in the case of contact that can support a tensile force, the data point with the most negative pressure) and define electrical conductance as pressure increases. The value of electrical conductance remains constant for contact pressures outside of the interval defined by the data points. If conductance is not also defined as a function of clearance, it is zero for all positive values of clearance and discontinuous at zero clearance
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.