SOLID187 Element Description

SOLID187 element is a higher order 3-D, 10-node element. SOLID187 has a quadratic displacement behavior and is well suited to modeling irregular meshes (such as those produced from various CAD/CAM systems).

The element is defined by 10 nodes having three degrees of freedom at each node: translations in the nodal x, y, and z directions. 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. See SOLID187 in the Mechanical APDL Theory Reference for more details about this element.

Figure 187.1:  SOLID187 Geometry

SOLID187 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 187.1: SOLID187 Geometry.

In addition to the nodes, the element input data includes the orthotropic or anisotropic material properties. Orthotropic and anisotropic material directions correspond to the element coordinate directions. The element coordinate system orientation is as described in the Material Reference.

Element loads are described in Nodal Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 187.1: SOLID187 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.

As described in Coordinate Systems, you can use ESYS 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.

KEYOPT(6) = 1 or 2 sets the element for using mixed formulation. For details on the use of mixed formulation, see .

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

KEYOPT(16) = 1 activates steady state analysis (defined via the SSTATE command). For more information, see Steady State Rolling in the Mechanical APDL Theory Reference.

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

You can apply an initial stress state to this element via the INISTATE command. For more information, see the INISTATE command, and also Initial Stress Loading.

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.

SOLID187 Output Data

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

Several items are illustrated in Figure 187.2: SOLID187 Stress Output. The element stress directions are parallel to the element coordinate system. A general description of solution output is given in The Item and Sequence Number Table. See the Basic Analysis Guide for ways to view results.

Figure 187.2:  SOLID187 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.

Table 187.2: SOLID187 Item and Sequence Numbers lists output available through ETABLE 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 187.2: SOLID187 Item and Sequence Numbers:

See Surface Solution for the item and sequence numbers for surface output (KEYOPT(17) = 4) for the ETABLE command

SOLID187 Assumptions and Restrictions

SOLID187 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