You can use the Edit Material dialog box to define the following types of gasket behavior:
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:
To define gasket behavior in the thickness direction:
From the menu bar in the Edit Material dialog box, select Other
Gasket Gasket Thickness Behavior.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.6.1.)
Click the arrow to the right of the Type field, and specify how you want to define gasket thickness-direction behavior:
Select Elastic-Plastic to define an elastic-plastic model. For more information, see “Defining a nonlinear elastic-plastic model” in “Defining the gasket behavior directly using a gasket behavior model,” Section 26.6.6 of the ABAQUS Analysis User's Manual.
Select Damage to define a damage elasticity model. For more information, see “Defining a nonlinear elastic model with damage” in “Defining the gasket behavior directly using a gasket behavior model,” Section 26.6.6 of the ABAQUS Analysis User's Manual.
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” in “Defining gasket behavior,” Section 12.10.5, for detailed instructions.
Display the Loading tabbed page.
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. Then 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. Then enter the closure value in the field provided.
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” in “Defining the gasket behavior directly using a gasket behavior model,” Section 26.6.6 of the ABAQUS Analysis User's Manual.
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.
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.
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,” Section 3.2.7.
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.
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.
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.
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” in “Defining the gasket behavior directly using a gasket behavior model,” Section 26.6.6 of the ABAQUS Analysis User's Manual.
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” in “Defining the gasket behavior directly using a gasket behavior model,” Section 26.6.6 of the ABAQUS Analysis User's Manual.
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,” Section 12.6.2, for more information).
When you define the thickness-direction behavior of the gasket in terms of force or force per unit length versus closure, ABAQUS/Standard provides the thickness-direction force or force per unit length as output variable S11. In this case you can define either a contact width or contact area versus closure curve that will be used to obtain the average “contact” pressure at each integration point as output variable CS11.
For more information, see “Defining the contact area for average contact pressure output” in “Defining the gasket behavior directly using a gasket behavior model,” Section 26.6.6 of the ABAQUS Analysis User's Manual.
To specify contact area or width:
Define gasket thickness-direction behavior as described in “Defining gasket behavior in the thickness direction” in “Defining gasket behavior,” Section 12.10.5.”
From the Suboptions menu in the Edit Material dialog box, select Contact Area.
A Suboption Editor appears.
Toggle on Use temperature-dependent data to define the data as a function of temperature.
A column labeled Temp appears in the Data table.
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 data depend.
In the Data table, define the contact area or contact width versus closure curve. Include temperature and field variable data if applicable. For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.
Click OK to return to the Edit Material dialog box.
ABAQUS/Standard measures the relative displacement between the bottom and top of the gasket element along the local 2- or 3-directions to define the transverse shear in the gasket. You can use the Edit Material dialog box to specify the elastic transverse stiffness as stress (or force, or force per unit length) per unit displacement. For more information, see “Defining the transverse shear behavior of the gasket” in “Defining the gasket behavior directly using a gasket behavior model,” Section 26.6.6 of the ABAQUS Analysis User's Manual.
Defining gasket transverse shear behavior:
From the menu bar in the Edit Material dialog box, select OtherGasket Gasket Transverse Shear Elastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.6.1.)
Click the arrow to the right of the Units field, and select the unit system in which you will define the transverse shear behavior:
Select Stress to define the transverse shear stiffness in terms of stress per unit displacement.
Select Force to define the transverse shear stiffness in terms of force per unit displacement or force per unit length per unit displacement, depending on the element type to which this behavior refers.
Toggle on Use temperature-dependent data to define the shear stiffness as a function of temperature.
A column labeled Temp appears in the Data table.
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 shear stiffness depends.
In the Data table, specify the shear stiffness. Include temperature and field variable data if applicable. For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.
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,” Section 12.6.2, for more information).
You can define the linear elastic behavior of the gasket by providing Young's modulus and Poisson's ratio. These data can be a function of temperature and/or field variables. If you do not specify the linear elastic behavior of the gasket, the gasket has no membrane stiffness. In this case you must ensure that the nodes of the elements are restrained adequately in the directions orthogonal to the thickness direction of the gasket.
Defining gasket membrane behavior:
From the menu bar in the Edit Material dialog box, select OtherGasket Gasket Membrane Elastic.
(For information on displaying the Edit Material dialog box, see “Creating or editing a material,” Section 12.6.1.)
Toggle on Use temperature-dependent data to define the data as a function of temperature.
A column labeled Temp appears in the Data table.
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 data depend.
In the Data table, enter Young's modulus and Poisson's ratio data. Include temperature and field variable data if applicable. For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.
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,” Section 12.6.2, for more information).