17.6.2.16. Thermal Condition

You can insert a known temperature (not from data transfer) boundary condition in an analysis by inserting a Thermal Condition object. Specify the value of the temperature in the Details pane under the Magnitude property. If the load is applied to a surface body, by default the temperature is applied to both the top and bottom surface body faces. You can optionally apply different temperatures to the top and bottom faces by adjusting the Shell Face entry in the Details pane. When you apply a Thermal Condition load to a solid body, the Shell Face property is not available in the Details pane. You can add the Thermal Condition load as time-dependent or spatially varying.

Note:

  • When a Thermal Condition is specified on the Top or Bottom shell face of a surface body, the opposite face defaults to the environment temperature unless it is otherwise specified from another load object.

  • For an assembly of bodies with different topologies (solid body, line, shell, beam), you must define a separate Thermal Condition load for each topology, that is, you must define one load scoped to line bodies, define a second load scoped to surface bodies, and so on.

  • For each load step, if an Imported Body temperature load and a Thermal Condition load are applied on common geometry selections, the Imported Body temperature load takes precedence. For additional rules when multiple load objects of the same type exist on common geometry selections, see Activating and Deactivating Loads.

  • If the Thermal Condition is applied to a shell face that has a Layered Section applied to it, you must set Shell Face to Both in order to solve the analysis.

This page includes the following sections:

Analysis Types

Thermal Condition is available for the following analysis types:
Dimensional Types

The supported dimensional types for the Thermal Condition boundary condition include:

  • 3D Simulation

  • 2D Simulation

Geometry Types

The supported geometry types for the Thermal Condition boundary condition include:

  • Solid

  • Surface/Shell

  • Wire Body/Line Body/Beam

Topology Selection Options

The supported topology selection options for Thermal Condition include:

  • Body. Thermal Condition is a body-based boundary condition.

  • Element

Define By Options

The Thermal Condition boundary condition’s loading is defined by Magnitude only.

Magnitude Options

The supported Magnitude options for Thermal Condition include the following:

  • Constant. This is the only option for Eigenvalue Buckling analyses.

  • Tabular (Time Varying)

  • Tabular (Step Varying): Supported for Static Structural analysis only.

  • Tabular (Spatially Varying)

  • Function (Time Varying)

  • Function (Spatially Varying)

  • Table Name. Supported for the Mechanical APDL solver only. A multi-variable table of numeric values that defines the temperature for the selection. The Magnitude field automatically lists the names of all tables that contain temperature as dependent variables.

  • New Table. Supported for the Mechanical APDL solver only. Select this option to create a new multivariable table of temperature values. You can then assign this table as the Magnitude.

Applying a Thermal Condition Boundary Condition

To apply a Thermal Condition:

  1. On the Environment Context tab, open the Loads drop-down menu and select Thermal Condition. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert>Thermal Condition.

  2. Define the Scoping Method. This property has two options: Geometry Selection and Named Selection. For either scoping type, the application supports only solid bodies, surface bodies (2D), line bodies, or elements.

    For surface bodies, in the Details pane, the Shell Face property provides a drop-down list. Select Top, Bottom, or Both (default) to apply the thermal boundary condition to the selected face. For bodies that have one or more layered section objects, you need to specify Both for Shell Face or the Thermal Condition will be under-defined and an error message will be generated.

  3. Specify the Magnitude of the temperature.

  4. Depending on the load type you selected for Magnitude, you may need to specify additional information under Tabular Data, Function, or Graphics Controls.

Details Pane Properties

The selections available in the Details pane are described below.

CategoryProperty/Options/Description
Scope

Scoping Method: Options include:

  • Geometry Selection: Default setting, indicating that the boundary condition is applied to a geometry or geometries, which are chosen using a graphical selection tool.

  • Geometry: Visible when the Scoping Method property is set to Geometry Selection. Displays the type of geometry (Body or Element) and the number of geometric entities (for example: 1 Body, 2 Elements) to which the boundary has been applied using the selection tools.

  • Named Selection: Indicates that the geometry selection is defined by a Named Selection.

  • Named Selection: Visible when the Scoping Method property is set to Named Selection. This field provides a drop-down list of available user-defined Named Selections. Named Selections must be either body- or element-based.

Definition

Type: Read-only field that displays the boundary condition type: Thermal Condition.

Magnitude: Temperature load. Select one of the following:

  • Import

  • Export

  • Constant. The default is 22 degrees Celsius.

  • Tabular

  • Function

  • Table Name. (Mechanical APDL solver only)

  • New Table.(Mechanical APDL solver only).

Suppressed: Include (No - default) or exclude (Yes) the boundary condition.

Load Vector Controls (Substructure Generation Analysis only)

Load Vector Assignment: Options include Program Controlled (default) and Manual. When set to Manual, the Load Vector Number property displays.

Load Vector Number: Specify a Load Vector Number using any value greater than 1. A setting of 1 is reserved for a pre-stress Substructure Generation analysis. If multiple loads have the same Load Vector Number, the application groups these loads during the solution process to generate a single load vector that is the combined effect of all grouped loads.

Function

This category displays when you set the Magnitude to Function. For additional information, see Spatial Load and Displacement Function Data.

Tabular Data

This category displays when you set the Magnitude to Tabular. For additional information, see Spatial Load Tabular Data.

Graph Controls

This category displays based upon the specifications made in the Function or Tabular categories. For additional information, see Spatial Load and Displacement Function Data or Spatial Load Tabular Data.

Thermal Condition Table Options (Mechanical APDL solver only)

If you selected the name of a table under Magnitude to define the temperature load on the boundary, the following options are available.

  • Parameterization: Check the box next to Magnitude to parameterize the table.

  • Spatial Coordinate System (read only)

  • Graphics Controls appears when you select a table that contains time as an independent variable.

For additional information, see Specify Thermal Condition Loads with Tables

Mechanical APDL References and Notes

The following Mechanical APDL commands, element types, and considerations are applicable for this boundary condition.

  • Temperatures are applied using the BF command. For surface bodies, with Top or Bottom Shell Face selection, temperatures are applied using the BFE command.

  • Magnitude (constant, tabular, and function) is always represented as a table in the input file.

  • A table is a special type of numeric array that enables the Mechanical APDL solver to calculate (through linear interpolation) the values between entries in a multi-dimensional table of numeric data. The solver applies these interpolated values across the selected geometry when it computes the solution. See the discussion in Array Parameters.

API Reference

For specific scripting information, see the Thermal Condition section of the ACT API Reference Guide.