SOLID272 Element Description

Use SOLID272 to model axisymmetric solid structures. It is defined by four nodes on the master plane, and nodes created automatically in the circumferential direction based on the four master plane nodes. The total number of nodes depends on the number of nodal planes (KEYOPT(2)). Each node has three degrees of freedom: translations in the nodal x, y and z directions. The element allows a triangle as the degenerated shape on the base plane to simulate irregular areas. The element has plasticity, hyperelasticity, stress stiffening, large deflection, and large strain capabilities. It also has mixed-formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and nearly and fully incompressible hyperelastic materials.

For more details about this element, see SOLID272 in the Mechanical APDL Theory Reference, and General Axisymmetric Elements in this document.

Figure 272.1:  SOLID272 Geometry (KEYOPT(2) = 3)

SOLID272 Input Data

The geometry and node locations for this element (when KEYOPT(2) = 3) are shown in Figure 272.1: SOLID272 Geometry (KEYOPT(2) = 3). The element input data includes nodes and the orthotropic material properties. The total number of nodes is the four base nodes times the number of nodal planes. (For information about how Fourier nodes are generated, see the NAXIS command documentation.) The default element coordinate system is the cylindrical coordinate system with the z axis as the axisymmetric axis (defined via the SECDATA command) and the circumferential direction as θ. (See General Axisymmetric Elements for details.) Use the ESYS command to define an element coordinate system, which forms the basis for orthotropic material directions.

Element loads are described in Nodal Loading. Pressures must be input as element surface loads on the element edges of the nodal planes as shown by the circled numbers in Figure 272.1: SOLID272 Geometry (KEYOPT(2) = 3). Positive pressures act into the element and the maximum face edge is 4n, where n is the number of nodal planes. If pressure is applied on the element edge with face numbers less than or equal to 4 and no load on other edges, the pressure loads are the same on the 360 degrees of circumferential surfaces. (If pressure is applied on a single element edge with a face number greater than 4, the pressure is ignored.) If pressure is applied on the element edges with faces p and 4q+p (where q = 1 . . . n-1), the pressure changes linearly with respect to θ within the part of the surface bounded by the edges p and 4q+p; on the rest of the surface, the pressure is zero.

Temperatures may be input as element body loads at the nodes. For the four nodes on the master plane, the node I1 temperature T(I₁) defaults to TUNIF. If all other temperatures are unspecified, they default to T(I₁). For any other input pattern, unspecified temperatures default to TUNIF. For the nodes generated in the circumferential direction based on the master node, they default to the value of their base nodes (T(I₁), T(J₁), T(K₁) or T(L₁), depending on their location) if all other temperatures are unspecified. For any other input pattern, unspecified temperatures default to TUNIF.

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 in this document.

As described in Coordinate Systems, you can use the ESYS command to orient the material properties and strain/stress output. Use RSYS to choose 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, issue a NROPT,UNSYM command. For a geometric nonlinear analysis when convergence is an issue, use an unsymmetric matrix.

"SOLID272 Input Summary" contains a summary of the element input. See Element Input in this document for a general description of element input.

SOLID272 Output Data

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

As shown in Figure 272.2: SOLID272 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.

To view 3-D mode shapes for a modal or eigenvalue buckling analysis, expand the modes with element results calculation active (via the MXPAND command's Elcalc = YES option).

Figure 272.2:  SOLID272 Stress Output

Element stress directions SX, SY, and SZ shown in the global coordinate system.

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.

Table 272.2: SOLID272 Item and Sequence Numbers lists output available through ETABLE using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this document for more information. The following notation is used in the output table:

SOLID272 Assumptions and Restrictions

SOLID272 Product Restrictions

There are no product-specific restrictions for this element.