SHELL229 Element Description

SHELL229 is a 3D layered shell element having in-plane thermal and electrical capabilities (membrane behavior), as well as structural capability (membrane and bending behavior). It supports the following physics combinations:

The element has four nodes with no limitation on the number of material layers (defined by the SECDATA command). It has up to 8 degrees of freedom at each node, including temperature and voltage in membrane format, as well as translation and rotation in 3D corresponding to structural analysis. The temperature generated by SHELL229 can be passed to structural shell elements (SHELL181 or SHELL281) in order to model thermal strain. See SHELL229 in the Mechanical APDL Theory Reference for more details about this element. For verification examples, see VM174, VM215, and VM223.

Figure 229.1: SHELL229 Geometry

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

x = element x-axis if ESYS is supplied.

SHELL229 Input Data

The geometry, node locations, and coordinates systems for this element are shown in Figure 229.1: SHELL229 Geometry. The element is defined by four nodes, one thickness per layer, a material angle for each layer, and the material properties.

The cross-sectional properties are input using the SECTYPE,,SHELL and SECDATA commands. These properties are the thickness, material number, and orientation of each layer. The number of integration points through the thickness is always 1, irrespective of the number entered in the SECDATA command. Real constants are not used for this element.

The default orientation for this element has the S1 (shell surface coordinate) axis aligned with the element's first parametric direction at its center.

The default first surface direction S1 can be reoriented in the element reference plane (as shown in Figure 229.1: SHELL229 Geometry) using 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.

KEYOPT(1) determines the element degree-of-freedom (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 229.1: SHELL229 Field Keys. For example, set KEYOPT(1) = 110 for a thermal-electric analysis (thermal field key + electric field key = 10 + 100). This activates a thermal-electric analysis with TEMP and VOLT as DOF labels and heat flow and electric current as reaction solutions.

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 table, material property requirements consist of those required for the individual fields (structural, thermal, and electric conduction) and those required for field coupling. Individual material properties are defined using the MP and MPDATA commands. Nonlinear and multiphysics material models are defined using the TB command.

The density, thermal conductivity, specific heat, and electrical resistivity can all be defined either with the MP command or the TB command.

The electrical resistivity can be defined as a function of primary variables by using tabular input on the MP command. For more information, see Defining Linear Material Properties Using Tabular Input in the Material Reference. Alternatively, TB,ELEC can be used to define electrical resistivity with TBOPT = RSV or electrical conductivity with TBOPT = COND. For more information, see Anisotropic Electrical Conductivity.

Nodal loads are defined with the D and F commands.

Element loads are described in Element Loading. Loads may be input on the element faces indicated by the circled numbers in Figure 229.1: SHELL229 Geometry using the SFE command. Body loads may be input at the element's material layers using the BFE commands.

SHELL229 surface and body loads are given in the following table. 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 Tabular Input in the Basic Analysis Guide and the individual surface or body load command description in the Command Reference.

The surface loads are input on a per-unit-area basis at all six faces including the shell edges:

This is in contrast to SHELL157 and SHELL181 where surface loads on shell edges (faces 3 to 6 above) are input on a per-unit-length basis.

The thermal surface loads, including radiation, convection, and heat flux can only be defined by the SFE command. Use the surface effect element SURF152 to generate film coefficients and bulk temperatures. SURF152 can also be used with FLUID116.

Element body loads may be input on a per layer basis. They can be defined with the BFE command only. One body load value is applied to the entire layer. If the first layer body load is input, and all others are unspecified, they default to the value specified for the first layer.

The body loads can be applied on material layers, where HG(1), HG(2), HG(3), . . . ., HG (number of material layers) can be defined with the BFE command only.

A summary of the element input is given in "SHELL229 Input Summary". A general description of element input is given in Element Input.

SHELL229 Output Data

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

Output temperatures may be read by structural shell elements SHELL181 and SHELL281 via the LDREAD,TEMP command.

Convection heat flux is positive out of the element. Applied heat flux is positive into the element.

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

A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

To see the distribution of element quantities through the thickness for this element, enter the POST1 postprocessor (/POST1), then issue /GRAPHICS,POWER and /ESHAPE,1 followed by PLESOL.

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 229.6: SHELL229 Element Output Definitions lists output available through the ETABLE command using NMISC item. See Element Table for Variables Identified By Sequence Number 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 229.7: SHELL229 Item and Sequence Numbers:

Table 229.8: SHELL229 SMISC Item and Sequence Numbers lists output available through the ETABLE command using SMISC item for all analyses with a structural field. See Creating an Element Table and The Item and Sequence Number Table in this reference for more information. The following notation is used:

SHELL229 Assumptions and Restrictions

SHELL229 Product Restrictions

There are no product-specific restrictions for this element.