SOLID185 Element Description

SOLID185 is used for 3-D modeling of solid structures. It is defined by eight nodes having three degrees of freedom at each node: translations in the nodal x, y, and z directions. The element has plasticity, hyperelasticity, stress stiffening, creep, 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.

SOLID185 is available in two forms:

See SOLID185 for more details about this element.

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

SOLID185 Homogeneous Structural Solid Element Description

SOLID185 Structural Solid is suitable for modeling general 3-D solid structures. It allows for prism, tetrahedral, and pyramid degenerations when used in irregular regions. Various element technologies such as B-bar, uniformly reduced integration, and enhanced strains are supported.

Figure 185.1:  SOLID185 Homogeneous Structural Solid Geometry

SOLID185 Homogeneous Structural Solid Input Data

The geometry and node locations for this element are shown in Figure 185.1: SOLID185 Homogeneous Structural Solid Geometry. The element is defined by eight nodes and the orthotropic material properties. The default element coordinate system is along global directions. You may define an element coordinate system using ESYS, which forms the basis for orthotropic material directions.

Element loads are described in Nodal Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers in Figure 185.1: SOLID185 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). For any other input temperature pattern, unspecified temperatures default to TUNIF. Similar defaults occurs for fluence except that zero is used instead of 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.

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 Initial State in the Mechanical APDL Advanced Analysis Guide.

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.

The effects of pressure load stiffness are automatically included for this element. If an unsymmetrical matrix is needed for pressure load stiffness effects, use NROPT,UNSYM.

"SOLID185 Homogeneous Structural Solid Input Summary" contains a summary of element input. For a general description of element input, see Element Input.

SOLID185 Homogeneous Structural Solid Output Data

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

Several items are illustrated in Figure 185.2: SOLID185 Homogeneous Structural Solid Stress Output. See Element Table for Variables Identified By Sequence Number and The Item and Sequence Number Table in this document for more information.

Figure 185.2:  SOLID185 Homogeneous Structural Solid Stress Output

Stress directions shown are for global directions.

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 185.2: SOLID185 Homogeneous Structural Solid Item and Sequence Numbers lists output available via ETABLE using the Sequence Number method. See Element Table for Variables Identified By Sequence Number and The Item and Sequence Number Table in this document for more information. The following notation is used in Table 185.2: SOLID185 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

SOLID185 Homogeneous Structural Solid Assumptions and Restrictions

This element has a layered option (KEYOPT(3) = 1). See "SOLID185 Layered Structural Solid Assumptions and Restrictions" for additional information.

SOLID185 Layered Structural Solid Element Description

Use SOLID185 Layered Solid to model layered thick shells or solids. The layered section definition is given by ANSYS section (SECxxx) commands. A prism degeneration option is also available.

Figure 185.3:  SOLID185 Layered Structural Solid Geometry

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

x = Element x-axis if ESYS is supplied.

SOLID185 Layered Structural Solid Input Data

The geometry and node locations for this element are shown in Figure 185.3: SOLID185 Layered Structural Solid Geometry. The element is defined by eight nodes. A prism-shaped element may be formed by defining the same node numbers for nodes K and L, and O and P.

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 SOLID185 Layered 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. The program 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.

SOLID185 Layered 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 185.3: SOLID185 Layered Structural Solid Geometry.

The default first surface direction S1 can be reoriented in the element reference plane (as shown in Figure 185.3: SOLID185 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 Nodal Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers in Figure 185.3: SOLID185 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--SOLID185 Layered 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). `For any other input temperature pattern, unspecified nodal temperatures default to TUNIF. ANSYS computes 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.

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

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

The effects of pressure load stiffness are automatically included for this element. If an unsymmetrical 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.

SOLID185 Layered Structural Solid Output Data

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

Several items are illustrated in Figure 185.4: SOLID185 Layered Structural Solid Stress Output. See Filling the Element Table for Variables Identified By Sequence Number in the Mechanical APDL Basic Analysis Guide and The Item and Sequence Number Table in this document for more information.

Figure 185.4:  SOLID185 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 number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 185.4: SOLID185 Layered Structural Solid Item and Sequence Numbers lists output available via ETABLE using the Sequence Number method. See Element Table for Variables Identified By Sequence Number and The Item and Sequence Number Table in this document for more information. The following notation is used in Table 185.4: SOLID185 Layered Structural Solid Item and Sequence Numbers:

SOLID185 Layered Structural Solid Assumptions and Restrictions

SOLID185 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