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.”
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 and Thermal 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:
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 30.1.5 of the ABAQUS Analysis User's Manual.
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 “Frictional behavior,” Section 30.1.5 of the ABAQUS Analysis User's Manual.
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 30.1.5 of the ABAQUS Analysis User's Manual.
Select Rough to specify an infinite coefficient of friction. For more information, see “Preventing slipping regardless of contact pressure” in “Frictional behavior,” Section 30.1.5 of the ABAQUS Analysis User's Manual.
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 30.1.5 of the ABAQUS Analysis User's Manual.
If you selected the Penalty or Lagrange Multiplier (Standard only) friction formulation, perform the following steps:
Display the Friction tabbed page.
Select the Directionality option of your choice:
Select Isotropic to enter a uniform friction coefficient.
Select 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 30.1.5 of the ABAQUS Analysis User's Manual.
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 select an option for Shear stress limit:
Select 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.
Select Specify to enter an equivalent shear stress limit, 
. If you select 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 30.1.5 of the ABAQUS Analysis User's Manual.
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, select an option to Specify maximum elastic slip:
Select Fraction of characteristic surface dimension to calculate the allowable elastic slip as a small fraction of the characteristic contact surface length.
Select 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, select an Elastic slip stiffness option:
Select Infinite (no slip) to deactivate shear softening.
Select Specify to activate softened tangential behavior. Then 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 30.1.5 of the ABAQUS Analysis User's Manual.
If you selected the Static-Kinetic Exponential Decay friction formulation, perform the following steps:
Display the Friction tabbed page.
Select an option for defining the exponential decay friction model:
Select Coefficients to provide the static friction coefficient, the kinetic friction coefficient, and the decay coefficient directly.
Select 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 section 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, select an option to Specify maximum elastic slip:
Select Fraction of characteristic surface dimension to calculate the allowable elastic slip as a small fraction of the characteristic contact surface length.
Select 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, select an Elastic slip stiffness option:
Select Infinite (no slip) to deactivate shear softening.
Select Specify to activate shear softening. Then 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 30.1.5 of the ABAQUS Analysis User's Manual.
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 “Defining a friction model in user subroutine FRIC or VFRIC” in “Frictional behavior,” Section 30.1.5 of the ABAQUS Analysis User's Manual.
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 30.1.2 of the ABAQUS Analysis User's Manual.
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 Constraint enforcement method field, choose the method that will be used to enforce contact constraints.
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.
Select Penalty (Standard) to enforce contact constraints using the penalty method. This method is applicable only to ABAQUS/Standard analyses.
If you selected the Default constraint enforcement method, choose the relationship that you will use to define the contact model 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. For more information, see “Contact formulation for ABAQUS/Explicit contact pairs,” Section 29.4.4 of the ABAQUS Analysis User's Manual.
Toggle off Allow separation after contact if you want to prevent surfaces from separating once they have come into contact.
Select Exponential to define an exponential pressure-overclosure relationship.
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).
Select Infinite (no slip) to set equal to infinity for kinematic contact and equal to the default penalty stiffness for penalty contact.
Select Specify, and enter a value for the maximum stiffness.
Select Linear to define a linear pressure-overclosure relationship.
Enter a positive value for the slope of the pressure-overclosure curve, k, in the Contact stiffness text field.
Select Tabular to define a piecewise-linear pressure-overclosure relationship in tabular form.
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.
Select Scale Factor (General Contact) 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.
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 one.
If you selected the Augmented Lagrange or Penalty constraint enforcement method, enter data to define the contact behavior.
Toggle off Allow separation after contact if you want to prevent surfaces from separating once they have come into contact.
Specify the contact stiffness in the Contact stiffness field.
Select Use default to have ABAQUS calculate the penalty contact stiffness automatically.
Select Specify, and enter a positive value for the contact penalty stiffness.
Specify a factor by which to multiply the chosen penalty stiffness in the Contact stiffness scale factor field.
Specify the Clearance at which contact pressure is zero. The default 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 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 30.1.3 of the ABAQUS Analysis User's Manual.
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 30.1.3 of the ABAQUS Analysis User's Manual.
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 30.1.3 of the ABAQUS Analysis User's Manual.
Select an option for specifying the Tangent fraction (the ratio of the tangential damping coefficient to the normal damping coefficient):
Select 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.
Select Specify value to enter a value for the tangent fraction.
Select a shape for the curve that describes the relationship between clearance and the damping coefficient:
Select 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.
Select 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.
Select 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 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. Enter this thickness in the Thickness of interfacial layer (Explicit) field.
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 30.2.1 of the ABAQUS Analysis User's Manual.
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 and/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 30.2.1 of the ABAQUS Analysis User's Manual.
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:
Select Use default (1.0) to convert all of the dissipated energy to heat.
Select Specify to enter the fraction of your choice.
Specify the Fraction of converted heat distributed to slave surface:
Select Use default (0.5) to distribute the heat equally between the master and slave surfaces.
Select 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 30.2.1 of the ABAQUS Analysis User's Manual.
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 viewfactor as a function of clearance.
The viewfactor 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 viewfactor as the clearance increases. The value of the viewfactor 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.