4-Node Thermal Shell

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | –

SHELL131 Element Description

SHELL131 is a 3-D layered shell element having in-plane and through-thickness thermal conduction capability. The element has four 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. SHELL131 generates temperatures that can be passed to structural shell elements in order to model thermal bending. See SHELL131 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 SHELL181 or SHELL281.

Figure 131.1:  SHELL131 Geometry

SHELL131 Geometry

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

x = element x-axis if ESYS is supplied.

SHELL131 Input Data

The geometry, node locations, and coordinates systems for this element are shown in Figure 131.1: SHELL131 Geometry. The element is defined by four 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 center of the element, which connects the midsides of edges LI and JK and is shown as xo in Figure 181.1:  SHELL181 Geometry. In the most general case, the axis can be defined as:


{x}I, {x}J, {x}K, {x}L = global nodal coordinates

If edges IJ and KL are parallel (rectangular or trapezoidal elements), the default orientation is the same as described in Coordinate Systems (the first surface direction is aligned with the IJ side). For elements with nonparallel edges IJ and JK, the default orientation represents the stress state better because the element uses a single point of quadrature (by default) in the element domain.

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.

You can also define element orientation via the ESYS command. See Coordinate Systems.

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 through-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 replaces 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:

- The element z-axis should be defined with the same care as for a structural shell element.
- If KEYOPT(6) = 1 (the paint option) is set, SECOFFSET,BOT should be input.

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 131.1: SHELL131 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 "SHELL131 Input Summary". A general description of element input is given in Element Input.

SHELL131 Input Summary


I, J, K, L

Degrees of Freedom

Quadratic (KEYOPT(3) = 0):

If KEYOPT(4) = 0 or 1: TBOT, TE2, TTOP
If KEYOPT(4) = 2: TBOT, TE2, TE3, TE4, TTOP
If KEYOPT(4) = 3: TBOT, TE2, TE3, TE4, TE5, TE6, TTOP
If KEYOPT(4) = 15: TBOT, TE2, TE3, TE4, TE5, TE6, TE7, TE8, TE9, TE10, TE11, TE12, TE13, TE14, TE15, TE16, TE17, TE18, TE19, TE20, TE21, TE22, TE23, TE24, TE25, TE26, TE27, TE28, TE29, TE30, TTOP

Linear (KEYOPT(3) = 1):

If KEYOPT(4) = 0 or 1: TBOT, TTOP
If KEYOPT(4) = 3: TBOT, TE2, TE3, TTOP
If KEYOPT(4) = 31: TBOT, TE2, TE3, TE4, TE5, TE6, TE7, TE8, TE9, TE10, TE11, TE12, TE13, TE14, TE15, TE16, TE17, TE18, TE19, TE20, TE21, TE22, TE23, TE24, TE25, TE26, TE27, TE28, TE29, TE30, TE31, TTOP

Constant (KEYOPT(3) = 2):

TEMP (one layer only)
Real Constants


Material Properties

MP command: KXX, KYY, KZZ, DENS, C, ENTH

Surface Loads
Convections  -- 
Face 1 (I-J-K-L) (bottom, -z side)
Face 2 (I-J-K-L) (top, +z side)
Face 3 (J-I), Face 4 (K-J), Face 5 (L-K), Face 6 (I-L)
Heat Fluxes  -- 
Face 1 (I-J-K-L) (bottom, -z side)
Face 2 (I-J-K-L) (top, +z side)
Face 3 (J-I), Face 4 (K-J), Face 5 (L-K), Face 6 (I-L)
Radiation  -- 
Face 1 (I-J-K-L) (bottom, -z side)
Face 2 (I-J-K-L) (top, +z side)
Body Loads
Heat Generations  -- 

HG(1), HG(2), HG(3), . . . ., HG(KEYOPT(4))

Special Features

Birth and death


Film coefficient evaluation (if any):

0 -- 

Evaluate at an average film temperature, (TS+TB)/2

1 -- 

Evaluate at element surface temperature, TS

2 -- 

Evaluate at fluid bulk temperature, TB

3 -- 

Evaluate at differential temperature, |TS-TB|


Temperature variation through layer:

0 -- 

Quadratic temperature variation through-layer (maximum number of layers = 15)

1 -- 

Linear temperature variation through-layer (maximum number of layers = 31)

2 -- 

No temperature variation through-layer (number of layers = 1)


Number of layers (input a value to match SECDATA commands, or leave blank to default). Maximum number of layers allowed depends on KEYOPT(3) setting (see above).



0 -- 

Thermal shell application

1 -- 

Paint application

SHELL131 Output Data

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

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

If the structural shell element uses two temperatures through the thickness, such as for SHELL181 (with only one layer) or SHELL281 (with only one layer), 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, such as for SHELL181 (with multiple layers), all temperatures are transferred over. In this case, the corner nodes of each SHELL131 element must have identical temperature degrees of freedom.

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 SHELL181 element using the same material and thickness for both layers can get its temperatures from a SHELL131 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 through the thickness for this element as well as all other thermal elements, use /GRAPHICS,POWER and /ESHAPE,1 followed by PLNSOL,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 131.1:  SHELL131 Element Output Definitions

ELElement NumberYY
NODESNodes - I, J, K, LYY
MATElement material number (from MAT command)YY
AREAArea of elementYY
XC, YC, ZCLocation where results are reportedY2
HGENHeat generations: HG(1), HG(2), HG(3), . . .Y-
TG:X, Y, ZThermal gradient components at midlayerYY
TF:X, Y, ZThermal flux components at midlayer YY
FACEFace label11
AREAFace area (same as element area)11
NODESFace nodes (same as element nodes)11
HFILMFace film coefficient11
TAVGAverage face temperature11
TBULKFluid bulk temperature1-
HEAT RATEHeat flow rate across face by convection11
HFAVGAverage film coefficient of the face-1
TBAVGAverage face bulk temperature-1
HFLXAVGHeat flow rate per unit area across face caused by input heat flux-1
HEAT RATE/AREAHeat flow rate per unit area across face by convection1-
HEAT FLUXHeat flux at each node of the face1-

  1. If a surface load is input.

  2. Available only at the centroid as a *GET item.

Table 131.2: SHELL131 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 131.2: SHELL131 Item and Sequence Numbers:


output quantity as defined in Table 131.1: SHELL131 Element Output Definitions


predetermined Item label for ETABLE command

Table 131.2:  SHELL131 Item and Sequence Numbers

Output Quantity NameItemFace 1Face 2IJKL
AREANMISC17-- -- -- --
HFAVGNMISC28-- -- -- --
TAVGNMISC39-- -- -- --
TBAVGNMISC410-- -- -- --
HEAT RATENMISC511-- -- -- --
HFLXAVGNMISC612-- -- -- --
THICKNESSNMISC-- -- 37383940

SHELL131 Assumptions and Restrictions

  • Zero area elements are not allowed. This occurs most frequently when the element is not numbered properly.

  • Zero thickness layers are not allowed.

  • A triangular element may be formed by defining duplicate K and L node numbers as described in Degenerated Shape Elements.

  • The cut boundary interpolation command (CBDOF) does not work with this element.

  • When using thermal contact, the TEMP degree of freedom must be present (KEYOPT(3) = 2 or KEYOPT(6) = 1).

  • There should not be a large variation in the ratio of through-thickness conductivity (KZZ) to layer thickness for all layers within the element. If the highest and lowest values for this ratio differ by a large factor (for example, 1e5), then the results for the element may be unreliable.

  • No check is made to ensure either that the number of layers between adjacent elements match or that the effective location of a degree of freedom (for example, TE7 from a 10 layer element) between elements sharing the same node is the same to a tolerance. If this is a concern, study the area using the /ESHAPE command. For cases where the layering intentionally changes, such as at a joint or at the runout of a tapered layer, use constraint equations (CE family of commands) with or without double nodes to connect the two sides.

  • The program removes all imposed degrees of freedom and nodal loads (i.e., internally issues DDELE,all,all and FDELE,all,all commands) when elements that use TTOP, TBOT, etc. as degrees of freedom:

    • are defined or redefined using the ET or KEYOPT commands.

    • are changed (or deleted) using the ET, ETCHG, or ETDELE commands to an element type that does not use these degrees of freedom.

      If your model contained SHELL131 elements with D and F loads, and you deleted these elements via ETDELE, the D and F loads will automatically be deleted and reapplied to the new DOF list. You do, however, need to check other loads and verify if they need to be deleted and reapplied.

  • When using the radiosity solver method, the Axis = ZEXT and CEXT extrusion options on the RSYMM command do not work with this element.

SHELL131 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 

  • Birth and death is not available.

ANSYS Mechanical Premium 

  • Birth and death is not available.

Release 18.2 - © ANSYS, Inc. All rights reserved.