17.6.2.17. Temperature

This boundary condition simulates a uniform, time-dependent, or spatially varying temperature over the selected geometry.

A spatially varying load allows you to vary the magnitude of a temperature according to coordinates and/or time. in a single coordinate direction and as a function of time using the Tabular Data or Function features. For the specific steps to apply tabular data and function loads, see the Specifying Boundary Condition Magnitude section. Alternatively, you can specify multivariable time-dependent and spatially varying temperature loads using the Table feature. For the specific steps to apply table loads, see Specifying Loads With Tables.

Note:  For each load step, if an Imported Temperature load and a Temperature load are applied on common geometry selections, the Imported 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.

This page includes the following sections:

Analysis Types

Temperature is available for the following analysis types:
Dimensional Types

The supported dimensional types for the Temperature boundary condition include:

  • 3D Simulation

  • 2D Simulation: Supported for Plane Stress and Axisymmetric behaviors only.

Geometry Types

The supported geometry types for the Temperature boundary condition include:

  • Solid

  • Surface/Shell

  • Wire Body/Line Body/Beam

Topology Selection Options

The supported topology selection options for Temperature include:

  • Body. When scoping a load to a body, you need to specify whether the Temperature is applied to Exterior Faces Only or to the Entire Body using the Apply To option.

  • Face

  • Edge

  • Vertex

  • Nodes

  • Element Face

  • Element

Note:  The same temperature value is applied when multiple faces, edges, vertices, nodes, element faces, and elements are selected.

Define By Options

The Temperature boundary condition's loading is defined by Magnitude only.

Magnitude Options

The supported Magnitude options for Temperature include the following:

  • Constant

  • Tabular (Time Varying)

  • Tabular (Spatially Varying): Not supported for LS-DYNA analyses.

  • Function (Time Varying): Not supported for LS-DYNA analyses.

  • Function (Spatially Varying): Not supported for LS-DYNA analyses.

  • Table Name. Supported for the Mechanical APDL solver only. A multi-variable table of numeric values that defines the temperature distribution 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 Temperature Boundary Condition

To apply a Temperature:

  1. Select the Temperature option from the Environment Context tab. Alternatively, right-click the Environment tree object or in the Geometry window and select Insert>Temperature.

  2. Define the Scoping Method as either Geometry Selection or Named Selection and then specify the geometry.

  3. Specify the Magnitude of the Temperature.

  4. Depending on the type of Temperature load you selected for Magnitude, you may need to specify additional information under Spatial Coordinate System, Graph Controls, Tabular Data or Function.

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 is set to Geometry Selection. Displays the type of geometry (Body, Face, etc.) and the number of geometric entities (for example: 1 Body, 2 Edges) 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 is set to Named Selection. This field provides a drop-down list of available user-defined Named Selections.

Apply To (Body scoping only), options include:

  • Exterior Faces Only

  • Entire Body

Definition

Type: Read-only field that displays boundary condition type - Temperature.

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.

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.

Temperature 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 Temperature 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 D 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.

LS-DYNA References and Notes

The following LS-DYNA keywords and considerations are applicable for this boundary condition.

API Reference

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