PLANE182 Element Description

Use PLANE182 to model 2D solid structures. It can be used as either a plane element (plane stress, plane strain or generalized plane strain) or an axisymmetric element with or without torsion. In most cases, the element is defined by four nodes with two degrees of freedom at each node: translations in the nodal x and y directions. For the axisymmetric option with torsion, it is still defined by four nodes, but with 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, stress stiffening, large deflection, and large strain capabilities. It has a mixed-formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials.

See PLANE182 for more details about this element.

Figure 182.1: PLANE182 Geometry

PLANE182 Input Data

The geometry and node locations for this element are shown in Figure 182.1: PLANE182 Geometry. The element input data includes four nodes, a thickness (for the plane stress option only), and the orthotropic material properties. The default element coordinate system is along global directions. You can define an element coordinate system (ESYS), which forms the basis for orthotropic material directions.

Element loads are described in Element Loading. Pressures can be input as surface loads on the element faces as shown by the circled numbers on Figure 182.1: PLANE182 Geometry. Positive pressures act into the element. Temperatures can 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.

Input the nodal forces (if any) 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 more information about 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 strain/stress output. Use RSYS 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.

"PLANE182 Input Summary" contains a summary of the element input. For a general description of element input, see Element Input. For axisymmetric applications see Harmonic Axisymmetric Elements.

PLANE182 Output Data

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

Several items are illustrated in Figure 182.2: PLANE182 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 182.2: PLANE182 Stress Output

Stress directions are shown for Global.

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.

PLANE182 Assumptions and Restrictions

PLANE182 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  —