Defining gasket behavior in the thickness direction

Abaqus/Standard measures the thickness-direction deformation as the closure between the bottom and top faces of the gasket element; therefore, the thickness-direction behavior must always be defined in terms of closure. In all cases you can define the thickness-direction behavior as a function of temperature and/or field variables. For more information, see the following sections:

  1. From the menu bar in the Edit Material dialog box, select OtherGasketGasket Thickness Behavior.

    (For information on displaying the Edit Material dialog box, see Creating or editing a material.)

  2. Click the arrow to the right of the Type field, and specify how you want to define gasket thickness-direction behavior:

  3. Click the arrow to the right of the Units field, and specify a unit system for defining thickness-direction behavior:

    • Select Stress to define thickness-direction behavior in terms of pressure versus closure. This option is available for all gasket element types.

    • Select Force to define thickness-direction behavior in terms of force versus closure or force per unit length versus closure, depending on the element type with which this behavior is used. This option is valid only for link elements and three-dimensional line elements.

      If you select this option, you can select Contact Area from the Suboptions menu to define contact area or contact width versus closure curves to output an average pressure through variable CS11. See Specifying a gasket contact area or contact width for average pressure output” for detailed instructions.

    For more information about selecting a unit system, see Choosing a unit system used to define the thickness-direction behavior.

  4. Display the Loading tabbed page.

  5. Click the arrow to the right of the Yield onset method field, and select a method for defining the onset of yield:

    • Select Relative slope drop to define yield onset as the point at which the slope of the loading curve decreases by a certain percentage from the maximum slope recorded up to that point. Enter the relative drop value in the field provided. The default is 0.1 (or 10%).

    • Select Closure value to specify a closure value at which yield occurs. Enter the closure value in the field provided.

  6. In the Tensile stiffness factor field, enter a the fraction of the initial compressive stiffness that defines the stiffness in tension. The default is 0.001. For more information, see Numerical stabilization of the thickness-direction behavior.

  7. Toggle on Use temperature-dependent data to define the gasket thickness behavior as a function of temperature.

    A column labeled Temp appears in the Data table.

  8. Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the gasket thickness behavior depends.

  9. In the Data table, define loading in terms of pressure versus closure, force versus closure, or force per unit length versus closure. Enter values for temperature and field variables if applicable. For detailed information on how to enter data, see Entering tabular data.

  10. Display the Unloading tabbed page, and toggle on Include user-specified unloading curves if desired. The user-specified unloading curves are in addition to the default unloading curve, which is the scaled portion of the loading curve before the point of yield onset.

    If you leave this option toggled off, skip to Step 13.

  11. Toggle on Use temperature-dependent data to define the unloading curve as a function of temperature.

    A column labeled Temp appears in the Data table.

  12. Click the arrows to the right of the Number of field variables field to increase or decrease the number of field variables on which the unloading curve depends.

  13. In the Data table, specify the unloading curve:

    • If you selected Damage in Step 2, provide data points of pressure (or force or force per unit length) versus elastic closure up to a given maximum closure. Enter values for temperature and field variables if applicable. For more information, see Defining a nonlinear elastic model with damage.

    • If you selected Elastic-Plastic in Step 2, provide data points of pressure (or force or force per unit length) versus closure (elastic plus plastic) for each given plastic closure in ascending values of closure. For more information, see Defining a nonlinear elastic-plastic model.

    For detailed information on how to enter data, see Entering tabular data.

  14. Click OK to close the Edit Material dialog box. Alternatively, you can select another material behavior to define from the menus in the Edit Material dialog box (see Browsing and modifying material behaviors, for more information).