PLANE42 Element Description

PLANE42 is used for 2D modeling of solid structures. The element can be used either as a plane element (plane stress or plane strain) or as an axisymmetric element. The element is defined by four nodes having two degrees of freedom at each node: translations in the nodal x and y directions. The element has plasticity, creep, swelling, stress stiffening, large deflection, and large strain capabilities.

An option is available to suppress the extra displacement shapes. See PLANE183 for a multi-node version of this element. See SOLID272 for an axisymmetric version that accepts nonaxisymmetric loading.

Figure 42.1: PLANE42 Geometry

PLANE42 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 42.1: PLANE42 Geometry. The element input data includes four nodes, a thickness (for the plane stress option only) and 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 42.1: PLANE42 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). For any other input pattern, unspecified temperatures default to TUNIF. Similar defaults occurs for fluence except that zero is used instead of TUNIF.

The nodal forces, if any, should be input per unit of depth for a plane analysis (except for KEYOPT(3) = 3) and on a full 360° basis for an axisymmetric analysis. KEYOPT(2) is used to include or suppress the extra displacement shapes.

KEYOPT(5) and KEYOPT(6) provide various element printout options. (See Element Solution.)

You cannot set initial state conditions (INISTATE) using this element. You can set initial state conditions using current-technology elements (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, issue NROPT,UNSYM.

A summary of the element input is given in "PLANE42 Input Summary". A general description of element input is given in Element Input. For axisymmetric applications see Harmonic Axisymmetric Elements.

PLANE42 Output Data

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

Several items are illustrated in Figure 42.2: PLANE42 Stress Output.

The element stress directions are parallel to the element coordinate system. Surface stresses are available on any face. Surface stresses on face IJ, for example, are defined parallel and perpendicular to the IJ line and along the Z axis for a plane analysis or in the hoop direction for an axisymmetric analysis. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 42.2: PLANE42 Stress Output

Stress directions shown are for KEYOPT(1) = 0

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 42.3: PLANE42 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 reference for more information. The following notation is used in Table 42.3: PLANE42 Item and Sequence Numbers:

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

PLANE42 Assumptions and Restrictions

PLANE42 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  —