SOLID45 Element Description

SOLID45 is used for the 3D modeling of solid structures. The element 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, creep, swelling, stress stiffening, large deflection, and large strain capabilities. A reduced integration option with hourglass control is available. A higher-order version of the SOLID45 element is SOLID186.

Figure 45.1: SOLID45 Geometry

SOLID45 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 45.1: SOLID45 Geometry. The element is defined by eight nodes and the orthotropic material properties. Orthotropic 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 45.1: SOLID45 Geometry. Positive pressures act into the element. Temperatures and fluences 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(1) is used to include or suppress the extra displacement shapes. KEYOPT(5) and KEYOPT(6) provide various element printout options (see Element Solution).

This element also supports uniform reduced (1 point) integration with hourglass control when KEYOPT(2) = 1. Using uniform reduced integration provides the following advantages when running a nonlinear analysis:

An analysis using uniform reduced integration can have the following disadvantages:

When the uniform reduced integration option is used (KEYOPT(2) = 1 - this option is the same as SOLID185 with KEYOPT(2) = 1), you can check the accuracy of the solution by comparing the total energy (SENE label in ETABLE) and the artificial energy (AENE label in ETABLE) introduced by hourglass control. If the ratio of artificial energy to total energy is less than 5%, the solution is generally acceptable. If the ratio exceeds 5%, refine the mesh. The total energy and artificial energy can also be monitored by using the OUTPR,VENG command in the solution phase. For more details, see Energies in the Mechanical APDL Theory Reference.

You cannot set initial state conditions (INISTATE) using this element. You can set initial state conditions using current-technology elements (such as LINK180,SHELL181). To continue using initial state conditions in future versions of Mechanical APDL, consider using a current element technology. For more information, see Legacy vs. Current Element Technologies in the Element Reference. For more information about setting initial state values, see the INISTATE command documentation and Initial State Loading in the Basic Analysis Guide.

Pressure load stiffness effects are included in linear eigenvalue buckling automatically. If an unsymmetric matrix is needed for pressure load stiffness effects, use NROPT,UNSYM.

A summary of the element input is given in "SOLID45 Input Summary". A general description of element input is given in Element Input.

SOLID45 Output Data

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

Several items are illustrated in Figure 45.2: SOLID45 Stress Output. The element stress directions are parallel to the element coordinate system. The surface stress outputs are in the surface coordinate systems and are available for any face (KEYOPT(6)). The coordinate systems for faces IJNM and KLPO are shown in Figure 45.1: SOLID45 Geometry. The other surface coordinate systems follow similar orientations as indicated by the pressure face node description. Surface stress printout is valid only if the conditions described in Element Solution are met. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

Figure 45.2: SOLID45 Stress Output

Stress directions shown are for KEYOPT(4) = 0

When KEYOPT(2) = 1 (the element is using uniform reduced integration), all the outputs for the element integration points are output in the same style as the full integration outputs. The number of points for full integration is used for consistency of output within the same element type.

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 45.3: SOLID45 Item and Sequence Numbers lists output available through 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 of this manual for more information. The following notation is used in Table 45.3: SOLID45 Item and Sequence Numbers:

See Surface Solution for the item and sequence numbers for surface output for the ETABLE command.

SOLID45 Assumptions and Restrictions

SOLID45 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 Professional  —