Specifying frictional behavior for mechanical contact property options

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.

• 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., ${\tau }_{eq}<{\tau }_{crit}$), 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 and Stiffness method for imposing frictional constraints in Abaqus/Explicit.

• 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.

• Select Rough to specify an infinite coefficient of friction. For more information, see Preventing slipping regardless of contact pressure.

• 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 ${\tau }_{eq}={\tau }_{crit}$. For more information, see Lagrange multiplier method for imposing frictional constraints in Abaqus/Standard.

• 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.

If you selected the Penalty or Lagrange Multiplier (Standard only) friction formulation, perform the following steps:

1. Display the Friction tabbed page.
2. 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 Anisotropic friction with directional preference associated with contact orientation.

3. Toggle on Use slip-rate-dependent data if the friction coefficient is dependent on slip rate.
4. Toggle on Use contact-pressure-dependent data if the friction coefficient is dependent on the contact pressure.
5. Toggle on Use temperature-dependent data if the friction coefficient is dependent on temperature.
6. 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.
7. Enter the required data in the data table provided.
8. 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, ${\tau }_{max}$. 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.

9. 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, ${\gamma }_i$. (For a steady-state transport analysis set this parameter equal to the absolute magnitude of the allowable elastic slip velocity ($\dot{{\gamma }_i}$) 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.

If you selected the Static-Kinetic Exponential Decay friction formulation, perform the following steps:

1. Display the Friction tabbed page.
2. 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.

   For more information, see Specifying static and kinetic friction coefficients.

3. If you selected the Coefficients definition option, enter the following in the data table provided:

   • Static friction coefficient, ${\mu }_s$.

   • Kinetic friction coefficient, ${\mu }_k$.

   • Decay coefficient, $d_c$.

   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, ${\mu }_1$.

   • In the second row, enter the dynamic friction coefficient, ${\mu }_2$ and the reference slip rate, ${\dot{\gamma }}_2$, at which ${\mu }_2$ is measured.

   • In the third row, enter the kinetic friction coefficient, ${\mu }_{\mathrm{\infty }}$. This value corresponds to the asymptotic value of the friction coefficient at infinite slip rate, ${\dot{\gamma }}_{\mathrm{\infty }}$. If this data line is omitted, Abaqus/Standard automatically calculates ${\mu }_{\mathrm{\infty }}$ such that $\left({\mu }_2-{\mu }_{\mathrm{\infty }}\right)/\left({\mu }_1-{\mu }_{\mathrm{\infty }}\right)=0.05$.

4. 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, ${\gamma }_i$. (For a steady-state transport analysis set this parameter equal to the absolute magnitude of the allowable elastic slip velocity ($\dot{{\gamma }_i}$) 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.

If you selected the User-defined friction formulation, perform the following steps:

1. 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.
2. 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.)

   For more information, see User-defined friction model.

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.