SOLID186 Element Description

SOLID186 is a higher order 3D 20-node solid element that exhibits quadratic displacement behavior. The element is defined by 20 nodes having three degrees of freedom per node: translations in the nodal x, y, and z directions. The element supports 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.

SOLID186 is available in two forms:

A lower-order version of the SOLID186 element is SOLID185.

SOLID186 Homogeneous Structural Solid Element Description

SOLID186 Homogeneous Structural Solid is well suited to modeling irregular meshes (such as those produced by various CAD/CAM systems). The element may have any spatial orientation.

Various printout options are available. See SOLID186 for more details.

Figure 186.1: SOLID186 Homogeneous Structural Solid Geometry

SOLID186 Homogeneous Structural Solid Input Data

The geometry, node locations, and the element coordinate system for this element are shown in Figure 186.1: SOLID186 Homogeneous Structural Solid Geometry. A prism-shaped element may be formed by defining the same node numbers for nodes K, L, and S; nodes A and B; and nodes O, P, and W. A tetrahedral-shaped element and a pyramid-shaped element may also be formed as shown in Figure 186.1: SOLID186 Homogeneous Structural Solid Geometry. SOLID187 is a similar, but 10-node tetrahedron element.

In addition to the nodes, the element input data includes the anisotropic material properties. Anisotropic material directions correspond to the element coordinate directions. The element coordinate system orientation is as 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 on Figure 186.1: SOLID186 Homogeneous Structural Solid 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 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.

KEYOPT(16) = 1 activates steady-state analysis (defined via SSTATE). For more information, see Steady-State Rolling in the Theory Reference. For a steady-state analysis, elements must be numbered as shown in Figure 186.1: SOLID186 Homogeneous Structural Solid Geometry.

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

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

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

SOLID186 Homogeneous Structural Solid Output Data

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

Figure 186.2: SOLID186 Homogeneous Structural Solid 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.

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.

Table 186.2: SOLID186 Homogeneous Structural Solid Item and Sequence Numbers lists output available through ETABLE using the Sequence Number method. See The General Postprocessor (POST1) and The Item and Sequence Number Table in this document for more information. The following notation is used in Table 186.2: SOLID186 Homogeneous Structural Solid Item and Sequence Numbers:

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

SOLID186 Homogeneous Structural Solid Assumptions and Restrictions

This element has a layered option (KEYOPT(3) = 1). See "SOLID186 Layered Structural Solid Assumptions and Restrictions" for additional information.

SOLID186 Layered Structural Solid Element Description

Use SOLID186 Layered Structural Solid to model layered thick shells or solids. The layered section definition is specified via section (SECxxx) commands. A prism degeneration option is also available.

Figure 186.3: SOLID186 Layered Structural Solid Geometry

x_o = Element x-axis if ESYS is not supplied.

x = Element x-axis if ESYS is supplied.

SOLID186 Layered Structural Solid Input Data

The geometry, node locations, and the element coordinate system for this element are shown in Figure 186.3: SOLID186 Layered Structural Solid Geometry. A prism-shaped element may be formed by defining the same node numbers for nodes K, L, and S; nodes A and B; and nodes O, P, and W.

In addition to the nodes, the element input data includes the anisotropic material properties. Anisotropic material directions correspond to the layer coordinate directions which are based on the element coordinate system. The element coordinate system follows the shell convention where the z axis is normal to the surface of the shell. The nodal ordering must follow the convention that I-J-K-L and M-N-O-P element faces represent the bottom and top shell surfaces, respectively. You can change the orientation within the plane of the layers via the ESYS command in the same way that you would for shell elements (as described in Coordinate Systems). To achieve the correct nodal ordering for a volume mapped (hexahedron) mesh, you can use the VEORIENT command to specify the desired volume orientation before executing the VMESH command. Alternatively, you can use the EORIENT command after automatic meshing to reorient the elements to be in line with the orientation of another element, or to be as parallel as possible to a defined ESYS axis.

Layered Section Definition Using Section Commands

You can associate SOLID186 Layered Structural Solid with a shell section (SECTYPE). The layered composite specifications (including layer thickness, material, orientation, and number of integration points through the thickness of the layer) are specified via shell section (SECxxx) commands. You can use the shell section commands even with a single-layered element. Mechanical APDL obtains the actual layer thicknesses used for element calculations by scaling the input layer thickness so that they are consistent with the thickness between the nodes.

You can designate the number of integration points (1, 3, 5, 7, or 9) located through the thickness of each layer. Two points are located on the top and bottom surfaces respectively and the remaining points are distributed equal distance between the two points. The element requires at least two points through the entire thickness. When no shell section definition is provided, the element is treated as single-layered and uses two integration points through the thickness.

SOLID186 Layered Structural Solid does not support real constant input for defining layer sections.

Other Input

The default orientation for this element has the S1 (shell surface coordinate) axis aligned with the first parametric direction of the element at the center of the element and is shown as x_o in Figure 186.3: SOLID186 Layered Structural Solid Geometry.

The default first surface direction S1 can be reoriented in the element reference plane (as shown in Figure 186.3: SOLID186 Layered Structural Solid Geometry) via the ESYS command. You can further rotate S1 by angle THETA (in degrees) for each layer via the SECDATA command to create layer-wise coordinate systems. See Coordinate Systems for details.

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 186.3: SOLID186 Layered Structural Solid Geometry. Positive pressures act into the element.

If you specify no element body load for defining temperatures--that is, if you define temperatures with commands other than BFE--SOLID186 Layered Structural Solid adopts an element-wise temperature pattern and requires only eight temperatures for the eight element corner 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 nodal temperatures default to TUNIF. Mechanical APDL calculates all layer interface temperatures by interpolating nodal temperatures.

Alternatively, you can input temperatures as element body loads at the corners of the outside faces of the element and at the corners of the interfaces between layers. In such a case, the element uses a layer-wise pattern. Temperatures T1, T2, T3, T4 are used for the bottom of layer 1, temperatures T5, T6, T7, T8 are used for interface corners between layers 1 and 2, and so on between successive layers, ending with temperatures at the top layer NLayer. If you input exactly NLayer+1 temperatures, one temperature is used for the four bottom corners of each layer, and the last temperature is used for the four top corner temperatures of the top layer. The first corner temperature T1 defaults to TUNIF. If all other corner temperatures are unspecified, they default to T1. For any other input pattern, unspecified temperatures default to TUNIF.

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.

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

KEYOPT(16) = 1 activates steady-state analysis (defined via SSTATE). For more information, see Steady-State Rolling in the Theory Reference. For a steady-state analysis, elements must be numbered as shown in Figure 186.3: SOLID186 Layered Structural Solid Geometry.

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

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

SOLID186 Layered Structural Solid Output Data

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

Figure 186.4: SOLID186 Layered Structural Solid Stress Output

The element stress directions are parallel to the layer coordinate system.

KEYOPT(8) controls the amount of data output to the results file for processing with the LAYER command. Interlaminar shear stress is available as SYZ and SXZ evaluated at the layer interfaces. KEYOPT(8) must be set to 1 to output these stresses in POST1. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

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.

Table 186.4: SOLID186 Layered Structural Solid Item and Sequence Numbers lists output available via ETABLE using the Sequence Number method. See The General Postprocessor (POST1) and The Item and Sequence Number Table in this document for more information. The following notation is used in Table 186.4: SOLID186 Layered Structural Solid Item and Sequence Numbers:

SOLID186 Layered Structural Solid Assumptions and Restrictions

SOLID186 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  —