CPT213 Element Description

CPT213 is a higher-order 2D eight-node coupled physics solid element capable of modeling coupled physics phenomena such as structural-pore-fluid-diffusion-thermal analysis and structural implicit gradient regularization using a nonlocal field. The element has quadratic displacement behavior and is well suited to modeling curved boundaries.

The element is defined by eight nodes and can have the following degrees of freedom at each corner node:

and two degrees of freedom at midside nodes:

CPT213 can be used as a plane strain or axisymmetric element. The element has stress stiffening, large deflection, and large strain capabilities. Various printout options are also available. See CPT213 for more details about this element.

Figure 213.1: CPT213 Geometry

A higher-order version of this element is CPT217.

CPT213 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 213.1: CPT213 Geometry.

A degenerated triangular-shaped element can be formed by defining the same node number for nodes K, L and O. In addition to the nodes, In addition to the nodes, for structural-pore-fluid-diffusion-thermal analysis, the element input data includes 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. Loads can be input (SF and SFE) on the element faces indicated by the circled numbers in Figure 213.1: CPT213 Geometry. Positive pressures act into the element. Positive pressures act into the element. Body loads may be input (BF and BFE) at the element nodes or as a single element value. Nodal forces can be applied to the nodes directly (F).

CPT213 surface, body, and nodal-force loads are given in Table 213.1: CPT213 Surface, Body, and nodal-force loads. Also see Loading Types in the Coupled-Field Analysis Guide.

Most loads can be defined as a function of primary variables by using tabular input. For more information, see Applying Loads Using Tabular Input in the Basic Analysis Guide and the descriptions of individual loading commands in the Command Reference.

For problems that do not consider the optional temperature degrees of freedom, 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). 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 and on a full 360° basis for an axisymmetric analysis.

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

The element generally produces an unsymmetric matrix. To avoid convergence difficulty, use the unsymmetric solver (NROPT,UNSYM).

The following table summarizes the element input. Element Input gives a general description of element input.

CPT213 Output Data

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

By default, the integration point results are copied to the nodes (ERESX).

As illustrated in Figure 213.2: CPT213 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 213.2: CPT213 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 number refers to a table footnote that describes when the item is conditionally available, and - indicates that the item is not available. All output is available only if calculated (based on input values).

For axisymmetric solutions, the X, Y, XY, and Z stress and strain outputs correspond to the radial, axial, in-plane shear, and hoop stresses and strains.

Table 213.3: CPT213 Item and Sequence Numbers lists output available via 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 document for more information. The following notation is used in Table 213.3: CPT213 Item and Sequence Numbers:

CPT213 Assumptions and Restrictions

CPT213 Product Restrictions

There are no product-specific restrictions for this element.