SOLID226 Element Description

SOLID226 supports the following physics combinations:

The element has twenty nodes with up to six degrees of freedom per node.

Structural capabilities include elasticity, plasticity, hyperelasticity, viscoelasticity, viscoplasticity, creep, large strain, large deflection, and stress stiffening effects. It also has mixed formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials.

Piezoresistive capabilities include the piezoresistive effect. Piezoelectric capabilities include direct and converse piezoelectric effects. Electrostatic-structural capabilities include electrostatic force coupling. Thermoelectric capabilities include Seebeck, Peltier, and Thomson effects, as well as Joule heating. In addition to thermal expansion, structural-thermal capabilities include the piezocaloric effect in dynamic analyses. The Coriolis effect is available for analyses with structural degrees of freedom. The thermoplastic effect is available for analyses with structural and thermal degrees of freedom.

The diffusion expansion and hydrostatic stress-migration effects are available for analyses with structural and diffusion degrees of freedom. The thermo-migration effect (Soret effect) and the temperature-dependent saturated concentration effect are available for analyses with thermal and diffusion degrees of freedom. The electro-migration effect is available for analyses with electrical and diffusion degrees of freedom.

See SOLID226 in the Mechanical APDL Theory Reference for more details about this element.

Figure 226.1:  SOLID226 Geometry

SOLID226 Input Data

The geometry, node locations, and the coordinate system for this element are shown in Figure 226.1: SOLID226 Geometry. The element input data includes twenty nodes and structural, thermal, and electrical material properties. The type of units (MKS or user defined) is specified through the EMUNIT command. EMUNIT also determines the value of free-space permittivity EPZRO. The EMUNIT defaults are MKS units and EPZRO = 8.85e-12 Farads/meter.

KEYOPT(1) determines the element DOF set and the corresponding force labels and reaction solution. KEYOPT(1) is set equal to the sum of the field keys shown in Table 226.1: SOLID226 Field Keys. For example, KEYOPT(1) is set to 11 for a structural-thermal analysis (structural field key + thermal field key = 1 + 10). For a structural-thermal analysis, UX, UY, and TEMP are the DOF labels and force and heat flow are the reaction solution.

The coupled-field analysis KEYOPT(1) settings, DOF labels, force labels, reaction solutions, and analysis types are shown in the following table.

As shown in the following tables, material property requirements consist of those required for the individual fields (structural, thermal, electric conduction, electrostatic, or diffusion) and those required for field coupling. Individual material properties are defined via the MP and MPDATA commands. Nonlinear and multiphysics material models are defined via the TB command. (The nonlinear material models do not apply to piezoelectric analyses (TB,PIEZ) where KEYOPT(1) = 1001 or 1011).

Various combinations of nodal loading are available for this element (depending upon the KEYOPT(1) value). Nodal loads are defined with the D and the F commands.

Element loads are described in Nodal Loading. Loads may be input on the element faces indicated by the circled numbers in Figure 226.1: SOLID226 Geometry using the SF and SFE commands. Positive pressures act into the element. Body loads may be input at the element's nodes or as a single element value using the BF and BFE commands.

SOLID226 surface and body loads are given in the following table. CHRGS and CHRGD are interpreted as negative surface charge density and negative volume charge density, respectively.

Most surface and body loads can be defined as a function of primary variables by using tabular input. For more information, see Applying Loads Using TABLE Type Array Parameters in the Mechanical APDL Basic Analysis Guide and the individual surface or body load command description in the Command Reference.

Automatic element technology selections are given in the following table.

A summary of the element input is given in "SOLID226 Input Summary". A general description of element input is given in Element Input.

SOLID226 Output Data

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

The element output 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 number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 226.7: SOLID226 Element Output Definitions lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) of the Basic Analysis Guide and The Item and Sequence Number Table of this reference for more information. The following notation is used in Table 226.8: SOLID226 Item and Sequence Numbers:

SOLID226 Assumptions and Restrictions

SOLID226 Product Restrictions

There are no product-specific restrictions for this element.