SHELL132 Element Description

SHELL132 is a 3-D layered shell element having in-plane and through-thickness thermal conduction capability. The element has eight nodes with up to 32 temperature degrees of freedom at each node. The conducting shell element is applicable to a 3-D, steady-state or transient thermal analysis. SHELL132 generates temperatures that can be passed to structural shell elements in order to model thermal bending. See SHELL132 in the Mechanical APDL Theory Reference for more details about this element.

If the model containing the conducting shell element is to be analyzed structurally, use an equivalent structural shell element instead, such as SHELL281.

Figure 132.1:  SHELL132 Geometry

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

x = element x-axis if ESYS is supplied.

SHELL132 Input Data

The geometry, node locations, and coordinates systems for this element are shown in Figure 132.1: SHELL132 Geometry. The element is defined by four/eight nodes, one thickness per layer, a material angle for each layer, and the material properties. If the material is uniform and the analysis has no transient effects, only one layer is needed with a linear temperature variation through the thickness.

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. Tapered thicknesses may be input using the SECFUNCTION command. The number of integration points from the SECDATA command is not used; rather it is determined for all layers with KEYOPT(3). In the GUI, the ShellTool provides a convenient way to define section data for this element (see Shell Analysis and Cross Sections in the Structural Analysis Guide). Real constants are not used for this element.

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 four in-plane integration points:

Where element geometry {x} is given as follows:

(s,r) = two isoparametric element coordinates

hI (s,r) = shape functions associated with eight element nodes.

{x}i = global coordinates of eight element nodes

The first surface direction S₁ can be rotated by angle θ (in degrees) for the layer via the SECDATA command. For an element, you can specify a single value of orientation in the plane of the element. Layer-wise orientation is supported.

Generally, the quadratic variation in temperature through each layer (KEYOPT(3) = 0) is used for transient analysis or for strongly temperature dependent materials, and the linear variation in temperature through each layer (KEYOPT(3) = 1) is used for steady state analysis with materials that are either not temperature dependent or weakly temperature dependent. Layers may be used to model the physical changes of properties through the thickness or the effect of a thru-thickness transient in greater detail.

KEYOPT(4) duplicates the number of layers input on the SECDATA commands. If KEYOPT(4) is 0 or blank, the program will query each element during definition in PREP7 as to which section information is being used, and then reassign the element to a different type. More element types are created as needed. The result can be seen using ETLIST and ELIST after all elements are defined. To ensure that the program can do this redefinition, you must define the section information before the element is defined.

If KEYOPT(6) (also referred to as the paint option) is used, TBOT is replaced with TEMP, allowing the element to be directly attached to an underlying solid to avoid the use of constraint equations. When this option is used, surface loads cannot be applied to face 1.

As this is a thermal shell element, the direction of the element z-axis and the presence of the SECOFFSET command have no effect on the solution. However, to get correct plots when using the /ESHAPE command:

Element loads are described in Nodal Loading. Convection or heat flux (but not both) and radiation (using the RDSF surface load label) may be input as surface loads at the element faces as shown by the circled numbers on Figure 132.1: SHELL132 Geometry. Because shell edge convection and flux loads are input on a per-unit-length basis, per-unit-area quantities must be multiplied by the total shell thickness. Radiation is not available on the edges. You can also generate film coefficients and bulk temperatures using the surface effect element SURF152. SURF152 can also be used with FLUID116.

Heat generation rates may be input as element body loads on a per layer basis. One heat generation value is applied to the entire layer. If the first layer heat generation rate HG(1) is input, and all others are unspecified, they default to HG(1). Nodal values are averaged over the entire element.

A summary of the element input is given in "SHELL132 Input Summary". A general description of element input is given in  Element Input.

SHELL132 Output Data

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

Output nodal temperatures may be read by structural shell elements (such as SHELL281) using the LDREAD,TEMP capability. If the structural shell element uses two temperatures through the thickness, only TBOT and TTOP are used, and any internal temperatures such as TE2 are ignored. If the structural shell element uses more than two temperatures through the thickness, all temperatures are transferred over. In this case, the corner nodes of each SHELL132 element must have identical temperature degrees of freedom. Also, the number of temperature points at a node generated in the thermal shell must match the number of temperature points at a node needed by the structural shell. For example, a two layer shell element using the same material and thickness for both layers can get its temperatures from a SHELL132 element using either two layers with KEYOPT(3) = 1 (linear variation) or one layer with KEYOPT(3) = 0 (quadratic variation). Temperatures passed from this element to the stress analysis via LDREAD,TEMP can be viewed using BFELIST, as opposed to the usual BFLIST.

Heat flowing out of the element is considered to be positive. Heat flows are labeled HBOT, HE2, . . . HTOP, similar to the temperature labels. Gradient and flux information is provided at the midthickness of each layer. 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.

To see the temperature distribution thru the thickness for this element as well as all other thermal elements, use /GRAPHICS,POWER and /ESHAPE,1 followed by PLNSOLL,TEMP.

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 132.2: SHELL132 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 in this reference for more information. The following notation is used in Table 132.2: SHELL132 Item and Sequence Numbers:

SHELL132 Assumptions and Restrictions

SHELL132 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