Specifying predefined friction parameters or contact forces

You can specify geometric constants and internal contact forces for predefined connector friction models and a friction-generating contact force and internal contact forces for user-defined connector friction models. You use the Predefined Friction Parameters tabbed page in the connector section editor to specify geometric constants and internal contact forces for predefined connector friction models. You use the Contact Force tabbed page in the connector section editor to specify a friction-generating contact force and internal contact forces for user-defined connector friction models. For more information, see Connector Friction Behavior.

This task shows you how to:

See Also
Defining friction
Specifying connector derived components

Specify predefined friction parameters

  1. Display the connector section editor by following the procedure outlined in Defining friction, and enter the necessary data.
  2. Select Predefined as the Friction model.
  3. Select the Predefined Friction Parameters tabbed page.
  4. Specify the geometric constants and internal contact forces depending on the connection type that you have selected. To display the connection type description that defines the required data entries, see Connection types.

Specify a friction-generating contact force and internal contact forces

  1. Display the connector section editor by following the procedure outlined in Defining friction, and enter the necessary data.
  2. Select User-defined as the Friction model.
  3. Select the Contact Force tabbed page.
  4. If desired, toggle on Specify component to define a friction-generating contact force/moment using an intrinsic connector component or a derived connector component.

    • Choose Intrinsic component, and select the force/moment that is consistent with the available component of relative motion for which you are defining the friction-generating contact force/moment.

    • Choose Derived component, and click to define a connector derived component. For more information, see Specifying connector derived components.

  5. If Specify component is toggled off, you must enter a value for the internal contact force in the data table in the Internal Contact Force portion of the Contact Force tabbed page. If desired, you can do the following to specify the internal contact force:

    Use independent components

    Toggle on Use independent components, choose Position or Motion, and select the available components of relative position or constitutive motion to be used as independent variables. Enter the connector relative position or constitutive motion in the direction specified by the independent component in the corresponding field of the table.

    Accum Slip

    Toggle on Use accumulated slip dependence, and enter the accumulated slip in the slip direction.

    Temp

    Toggle on Use temperature-dependent data, and enter the temperature.

    Field 1, Field 2, etc.

    Specify the Number of field variables, and enter the value of the first field variable, the value of the second field variable, etc.

    Internal Contact Force

    Specify the internal contact force data.

  6. To modify the behavior settings for the regularization (Abaqus/Explicit analyses only) or the extrapolation of the data, use the procedure described in Specifying behavior settings for tabular data.