PLANE183 Element Description

PLANE183 is a higher order 2D, 8-node or 6-node element. PLANE183 has quadratic displacement behavior and is well suited to modeling irregular meshes (such as those produced by various CAD/CAM systems).

This element is defined by eight nodes or six nodes. It can be used as a plane element (plane stress, plane strain and generalized plane strain) or as an axisymmetric element (with or without torsion). In most cases, the element has two degrees of freedom at each node: translations in the nodal x and y directions. For the axisymmetric with torsion option, however, the element has three degrees of freedom at each node: translations in the nodal x and y directions and rotation in the nodal y direction.

The element has plasticity, hyperelasticity, creep, stress stiffening, large deflection, and large strain capabilities. It also has mixed formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials. Initial state is supported. Various printout options are also available. See PLANE183 for more details about this element.

Figure 183.1: PLANE183 Geometry

PLANE183 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 183.1: PLANE183 Geometry.

Although a degenerated triangular-shaped element may be formed by defining the same node number for nodes K, L and O when KEYOPT(1) = 1, it is better to use KEYOPT(1) = 1 for triangular shaped elements. In addition to the nodes, the element input data includes a thickness (TK) (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 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 in Figure 183.1: PLANE183 Geometry. Positive pressures act into the element. Temperatures 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.

The nodal forces, if any, should be input per unit of depth for a plane analysis (except for KEYOPT(3) = 3 or KEYOPT(3) = 5) and on a full 360° basis for an axisymmetric analysis. The input torque (if any) for an axisymmetric analysis with torsion is on a full 360° basis.

KEYOPT(3) = 3 enables you to define constant or varying thickness via the real constant input. To define varying thickness, input a table name (specified as %tablename% and created via *DIM). Tabular thickness can vary in terms of coordinates (X and Y) or node numbers. Supported primary variables for tabular thickness are X, Y, and NODES. (The Function Tool is a convenient way to define your thickness tables; you can use it to define thickness as a function of global/local coordinates.)

KEYOPT(3) = 5 enables generalized plane strain. (Surface output is suppressed.) For more information about the generalized plane strain option, see Generalized Plane Strain.

KEYOPT(6) = 1 sets the element for using mixed formulation. For details on the use of mixed formulation, see Applications of Mixed u-P Formulations .

KEYOPT(15) = 1 sets the element for perfectly matched layers (PML). For more information, see Perfectly Matched Layers (PML) in Elastic Media in the Theory Reference.

For extra surface output, KEYOPT(17) = 4 activates surface solution for faces with nonzero pressure. For more information, see Surface Solution.

You can apply an initial stress state to this element via the INISTATE command. For more information, see Initial State in the Advanced Analysis Guide.

As described in Coordinate Systems, you can use ESYS to orient the material properties and stress/strain output. Use ESYS to select output that follows the material coordinate system or the global coordinate system.

The effects of pressure load stiffness are automatically included for this element. If an unsymmetric matrix is needed for pressure load stiffness effects, use NROPT,UNSYM.

The next table summarizes the element input. Element Input gives a general description of element input. For axisymmetric applications see Harmonic Axisymmetric Elements.

PLANE183 Output Data

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

Several items are illustrated in Figure 183.2: PLANE183 Stress Output.

The element stress directions are parallel to the element coordinate system. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 183.2: PLANE183 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.

PLANE183 Assumptions and Restrictions

PLANE183 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 Mechanical Pro  —  

Ansys Mechanical Premium  —