Modifying Global Element Assignments

When you create an Abaqus case, Abaqus for CATIA V5 creates a Global Element Assignment object. The Global Element Assignment object for each case (Nonlinear Structural, Explicit Dynamics, or Thermal) defines the default Abaqus element formulation for each combination of element topology and order. The element type selected by Abaqus for CATIA V5 depends on the dimensionality of the part and the meshing technique that you apply to it. For example, by default Abaqus for CATIA V5 selects S4 elements for shells that have been meshed with linear quadrilateral elements. You can select additional element behaviors and controls that modify the default element assignments. Solid, continuum shell, gasket, shell, membrane, and beam element behaviors are available inAbaqus for CATIA V5. You can use modified, hybrid, reduced-integration, incompatible mode, and thickness behavior element controls to further change the selected element behaviors. See Default Element Assignments and Additional Element Formulations for more information.

You can override the default global element assignment for a selected part or region using the local element assignment tool described in Modifying Local Element Assignments.

This task shows you how to modify the global element assignment.

  1. Double-click the Global Element Assignment object under the Nonlinear Structural case, Explicit Dynamics case, or Thermal case feature in the specification tree.

    The Global Element Assignment dialog box appears. The dialog box displays a list of the element topology and order and the corresponding element type. The contents of the dialog box depend on the type of case you are in. However, you can modify the default element type assignments only in a Nonlinear Structural or Explicit Dynamics case. In a Thermal case the data presented are for information only.

  2. Select an element from the list, and select any additional element formulations to apply: Modified Formulation, Reduced Integration, Hybrid Formulation, Incompatible Modes, Thickness behavior only (for gasket elements, used to ignore shear and membrane gasket material properties), or Section Controls (for an Explicit Dynamics case). Only the element controls applicable to the current element type are available.

    If necessary, the element name in the Element Type column changes to reflect your selection.

  3. If you selected the linear hexahedral or wedge element formulations, you can choose between Solid, Continuum Shell, and Gasket elements. See Assigning Continuum Shell Properties to Solids and Assigning Gasket Properties to Solids for more information.

  4. If parabolic hexahedral or wedge elements are assigned to the part, you can choose between Solid and Gasket elements. See Assigning Gasket Properties to Solids for more information.

  5. If you selected the linear triangle, linear quadrilateral, or parabolic quadrilateral element formulations, you can choose between Shell and Membrane elements. See Assigning Membrane Properties to Surfaces for more information.

  6. If you selected Section Controls, click to open the Section Controls dialog box. You can edit one or more of the following controls, depending on the current element type:

    1. Toggle on Yes for Second-order accuracy if the analysis includes components undergoing more than five revolutions.

    2. Toggle on Yes for Distortion control, and change the Length ratio to change the distortion control behavior for solid elements.

      Toggle on No to turn off distortion control.

      By default, distortion control is activated only for elements with hyperelastic or hyperfoam materials.

    3. Toggle on Enhanced, Relax stiffness, Stiffness, Viscous, or Combined to change the Hourglass control. If the selected method calls for it, you may change the Stiffness-viscous scaling factor and/or the Displacement hourglass scaling factor.

    See Section Controls for more information.

  7. Click OK in the Global Element Assignment dialog box.

    All elements in the model with the selected topology and order will use the specified element type, unless a local element assignment is applied to some elements.