SOLID92 Element Description

SOLID92 has a quadratic displacement behavior and is well suited to model irregular meshes (such as produced from various CAD/CAM systems).

The element is defined by ten nodes having three degrees of freedom at each node: translations in the nodal x, y, and z directions. The element also has plasticity, creep, swelling, stress stiffening, large deflection, and large strain capabilities.

Figure 92.1: SOLID92 Geometry

SOLID92 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 92.1: SOLID92 Geometry.

Beside the nodes, the element input data includes the orthotropic material properties. Orthotropic material directions correspond to the element coordinate directions. The element coordinate system orientation is as described in Coordinate Systems.

Element loads are described in Element Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 92.1: SOLID92 Geometry. Positive pressures act into the element. Temperatures and fluences may be input as element body loads at the nodes. The node I temperature T(I) defaults to TUNIF. If all other temperatures are unspecified, they default to T(I). If all corner node temperatures are specified, each midside node temperature defaults to the average temperature of its adjacent corner nodes. For any other input temperature pattern, unspecified temperatures default to TUNIF. Similar defaults occurs for fluence except that zero is used instead of TUNIF.

You cannot set initial state conditions (INISTATE) using this element. You can set initial state conditions using current-technology elements only (such as LINK180,SHELL181). To continue using initial state conditions in future versions of Mechanical APDL, consider using a current element technology. For more information, see Legacy vs. Current Element Technologies in the Element Reference. For more information about setting initial state values, see INISTATE and Initial State Loading in the Basic Analysis Guide.

Pressure load stiffness effects are included in linear eigenvalue buckling automatically. If an unsymmetric matrix is needed for pressure load stiffness effects, use NROPT,UNSYM.

A summary of the element input is given in "SOLID92 Input Summary". A general description of element input is given in Element Input.

SOLID92 Output Data

The solution output associated with the element is in two forms:

Several items are illustrated in Figure 92.2: SOLID92 Stress Output. The element stress directions are parallel to the element coordinate system. The surface stress outputs are in the surface coordinate system and are available for any face (KEYOPT(6)). The coordinate system for face J-I-K is shown in Figure 92.2: SOLID92 Stress Output. The other surface coordinate systems follow similar orientations as indicated by the pressure face node description. Surface stress printout is valid only if the conditions described in Element Solution are met. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 92.2: SOLID92 Stress Output

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates that the item can be accessed by the Component Name method (ETABLE, ESOL). The O column indicates the availability of the items in the file jobname.out. The R column indicates the availability of the items in the results file.

In either the O or R columns, “Y” indicates that the item is always available, a letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 92.3: SOLID92 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) in the Basic Analysis Guide and The Item and Sequence Number Table in this manual for more information. The following notation is used in Table 92.3: SOLID92 Item and Sequence Numbers:

See Surface Solution for the item and sequence numbers for surface output for the ETABLE command.

SOLID92 Assumptions and Restrictions

SOLID92 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

Ansys Professional  —