Assigning Elements
Nonlinear Structural Analysis and Thermal Analysis provide a library of elements that can be assigned to the parts in your model. When you create a Nonlinear Structural Analysis case or a Thermal Analysis case, Nonlinear Structural Analysis or Thermal Analysis, repectively, assigns a default element type to each mesh part in your model. When you are working in the Nonlinear Structural Analysis workbench, you can modify the default element assignment that is applied to all parts. In addition, you can modify the element assignment to a selected part or to a selected region within a part. You cannot change the element assignments from their default values in the Thermal Analysis workbench.
The following topics are discussed in this section:
Default Element Assignments
Nonlinear Structural Analysis and Thermal Analysis assign a default element type to each mesh part in your model based on the dimensionality of the mesh part (solid, two-dimensional, or beam), the order of the element (linear or parabolic), and the case (structural or thermal). Table 5–1 and Table 5–2 describe the default element type assignment for a Nonlinear Structural and Thermal case, respectively. (See Creating Mesh Parts for information on creating mesh parts.)
Table 5–1 Default element types for a Structural case.
| Mesh Part | Element | Description |
|---|---|---|
| Beam Linear | B31 | 2-node linear beam in space |
| Beam Parabolic | B32 | 3-node quadratic beam in space |
| Solid Linear | C3D4 | 4-node linear tetrahedron |
| Solid Linear | C3D6 | 6-node linear triangular prism |
| Solid Linear, Extruded | C3D8 | 8-node linear hexahedron |
| Solid Parabolic, Modified | C3D10M* | 10-node modified tetrahedron, with hourglass control |
| Solid Parabolic | C3D15 | 15-node quadratic triangular prism |
| Solid Parabolic, Extruded | C3D20 | 20-node quadratic hexahedron |
| 2D Linear | S3 | 3-node triangular general-purpose shell, finite membrane strains (identical to element S3R) |
| 2D Linear | S4 | 4-node doubly curved general-purpose shell, finite membrane strains |
| 2D Parabolic | STRI65 | 6-node triangular thin shell, using five degrees of freedom per node |
| * When modeling contact using the surface-to-surface formulation, C3D10 elements are preferred over C3D10M. | ||
Table 5–2 Default element types for a Thermal case.
| Mesh Part | Element | Description |
|---|---|---|
| Solid Linear | DC3D4 | 4-node linear heat transfer tetrahedron |
| Solid Linear | DC3D6 | 6-node linear heat transfer triangular prism |
| Solid Linear | DC3D8 | 8-node linear heat transfer hexahedron |
| Solid Parabolic | DC3D10 | 10-node quadratic heat transfer tetrahedron |
| Solid Parabolic | DC3D15 | 15-node quadratic heat transfer triangular prism |
| Solid Parabolic | DC3D20 | 20-node quadratic heat transfer hexahedron |
| 2D Linear | DS3 | 3-node heat transfer triangular shell |
| 2D Linear | DS4 | 4-node heat transfer quadrilateral shell |
| 2D Parabolic | DS6 | 6-node heat transfer triangular shell |
| 2D Parabolic | DS8 | 8-node heat transfer quadrilateral shell |
Additional Element Formulations
An element's formulation refers to the mathematical theory used to define the element's behavior. To accommodate different types of behavior, some element families include elements with several different formulations. You can choose additional formulations when you are modifying the global element assignment (every element of that type in the model) or the local element assignment (every element of that type in a selected part). The following additional element formulations are provided by Nonlinear Structural Analysis and Thermal Analysis:
Hybrid elements
Hybrid elements are intended primarily for use with incompressible and almost incompressible material behavior. When the material response is incompressible, the solution to a problem cannot be obtained in terms of the displacement history only, since a purely hydrostatic pressure can be added without changing the displacements. Hybrid elements have more internal variables than their nonhybrid counterparts and are slightly more expensive computationally.
Modified parabolic tetrahedral elements
Modified parabolic tetrahedral elements result in improved computational performance for components involved in contact interactions.
Reduced-integration elements
The solver uses numerical techniques to integrate various quantities over the volume of each element, thus allowing complete generality in material behavior. Using Gaussian quadrature for most elements, the solver evaluates the material response at each integration point in each element. Some elements can use full or reduced integration, a choice that can have a significant effect on the accuracy of the element for a given problem. Reduced integration uses a lower-order integration to form the element stiffness. The mass matrix and distributed loadings use full integration. Reduced integration reduces running time, especially in three dimensions.
Incompatible mode elements
Linear hexahedral elements with incompatible modes perform much better in pure bending applications than the standard linear hexahedron but with much less computational expense than parabolic elements.
Table 5–3 lists the additional element types that are available in Nonlinear Structural Analysis and Thermal Analysis.
Table 5–3 Additional supported element types.
| Mesh Part | Options | Element | Description |
|---|---|---|---|
| Solid Linear | Hybrid | C3D4H | 4-node linear tetrahedron, hybrid, constant pressure |
| Solid Linear | Hybrid | C3D6H | 6-node linear triangular wedge, hybrid, constant pressure |
| Solid Linear, Swept | Hybrid | C3D8H | 8-node linear hexahedron, hybrid, constant pressure |
| Solid Linear, Extruded | Reduced Integration | C3D8R | 8-node linear hexahedron, reduced integration, hourglass control |
| Solid Linear, Extruded | Incompatible Modes | C3D8I | 8-node linear hexahedron, incompatible modes |
| Solid Linear, Extruded | Hybrid & Reduced Integration | C3D8RH | 8-node linear hexahedron, hybrid, constant pressure, reduced integration, hourglass control |
| Solid Linear, Extruded | Hybrid & Incompatible Modes | C3D8IH | 8-node linear hexahedron, hybrid, constant pressure, incompatible modes |
| Solid Parabolic | None | C3D10 | 10-node quadratic tetrahedron |
| Solid Parabolic | Modified | C3D10M | 10-node modified tetrahedron, with hourglass control |
| Solid Parabolic | Hybrid | C3D10H | 10-node quadratic tetrahedron, hybrid, linear pressure |
| Solid Parabolic | Modified & Hybrid | C3D10MH | 10-node modified quadratic tetrahedron, hybrid, linear pressure |
| Solid Parabolic | Hybrid | C3D15H | 15-node modified quadratic triangular wedge, hybrid, linear pressure |
| Solid Parabolic, Extruded | Reduced Integration | C3D20R | 20-node quadratic hexahedron, reduced integration |
| Solid Parabolic, Extruded | Hybrid | C3D20H | 20-node quadratic hexahedron, hybrid, linear pressure |
| Solid Parabolic, Extruded | Hybrid & Reduced Integration | C3D20RH | 20-node quadratic hexahedron, hybrid, linear pressure, reduced integration |
| 2D Linear | Reduced Integration | S3R | 3-node triangular general-purpose shell, finite membrane strains (identical to element S3) |
| 2D Linear | Reduced Integration | S4R | 4-node doubly curved general-purpose shell, reduced integration, hourglass control, finite membrane strains |
Modifying Global Element
Assignments
When you create a nonlinear or thermal case, Nonlinear Structural Analysis or Thermal Analysis creates a Global Element Assignment object. The Global Element Assignment object for each case (Nonlinear Structural or Thermal) defines the default element formulation for each combination of element topology and order. The element type selected by Nonlinear Structural Analysis or Thermal Analysis depends on the dimensionality of the part and the meshing technique that you apply to it. For example, by default Nonlinear Structural Analysis or Thermal Analysis 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, shell, and beam element behaviors are available. You can use modified, hybrid, reduced-integration, and incompatible mode 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.
-
Double-click the Global Element Assignment object under the Nonlinear Structural 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 case. In a Thermal case the data presented are for information only.
-
Select an element from the list, and select any additional element formulations to apply: Modified Formulation, Reduced Integration, Hybrid Formulation, or Incompatible Modes. 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.
-
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.
Modifying Local Element
Assignments
When you are working in a Nonlinear Structural Analysis case, you can modify the element type assignments for a selected mesh part by selecting additional element formulation options. You can also modify the element type assignments for a selected region within a mesh part, such as a selected face of a shell part. Solid, shell, and beam element behaviors are available in Nonlinear Structural Analysis. You can use modified, hybrid, reduced-integration, and incompatible mode element controls to further change the selected element behaviors. See Default Element Assignments and Additional Element Formulations for more information.
This task shows you how to modify the local element
assignment for a selected mesh part or region.
-
Click the Local Element Assignment icon
.The Local Element Assignment dialog box appears, and a Local Element Assignment object appears in the specification tree under the Global Element Assignment feature.
-
From the window or the specification tree, select the mesh part or a region within a mesh part.
The Support field is updated to reflect your selection, and the Element Type field displays the element type assigned to the selected part.
-
Optionally, select the element controls to apply: Modified Formulation, Hybrid Formulation, Reduced Integration, or Incompatible Modes. 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.
-
Click OK in the Local Element Assignment dialog box.