Temperature

You can use the Temperature command to specify a temperature to apply to selected geometry or nodes. The options available for defining that temperature load depend on your current solver environment.

Defining a temperature in the Simcenter Nastran and Simcenter 3D Multiphysics environments

In the Simcenter Nastran, MSC Nastran, and Simcenter 3D Multiphysics environments, you can use the Temperature command to define thermal loads on a structure to:

• Perform stress analysis.

• Determine thermal expansion.

The options in the Temperature dialog box correspond to one of several different bulk data entries depending on the option you select from the Type list:

Type	Description	Corresponding bulk data entry
Temperature****Node ID Table	Defines the temperature at selected nodes to determine thermal loading, temperature-dependent material properties, or stress recovery.	TEMP
Temperature - External Time Unassigned	Applies a constant temperature load by importing an existing results file. Results can be imported from Nastran, Simcenter 3D Thermal, Abaqus, or ANSYS.	TEMP
**Through Thickness (Temperature and Gradient)**Through Thickness (Top and Bottom)	Defines the temperature and gradient in the thickness direction for certain types of 2D elements.	TEMPP1
On 1D elements	Defines temperature loads for CBAR, CBEAM, CBEND, CROD, CTUBE, and CONROD elements.	TEMPRB

For more information on specifying temperatures for Nastran analyses, see Modeling thermal strain in a Nastran analysis.

Note:

You cannot add a temperature directly to the load container of a Simcenter Nastran, MSC Nastran, or Simcenter 3D Multiphysics solution or subcase; instead, a load set must be used.

Defining a temperature in the Simcenter 3D Multiphysics environment

In the Simcenter 3D Multiphysics environment, you can also create temperatures with time assigned values. You cannot place time assigned and time unassigned temperatures in the same temperature set.

You can choose these additional selections from the Type list of the Temperature dialog box:

Type	Description	Corresponding bulk data entry
Temperature - Time Assigned	Defines a temperature with a time dependent field.	DTEMP
Temperature - External Time Assigned	Applies a time dependent temperature by importing a Binary Universal (.bun) file.	DTEMPEX

For more information on specifying temperatures for Multiphysics analyses, see Modeling thermal strain.

Defining a temperature load in the Abaqus environment

In the Abaqus environment, the options in the Temperature Load dialog box correspond to the *TEMPERATURE keyword. You can use the Temperature Load command to define create an Abaqus predefined temperature field.

In a structural analysis, the temperature difference between a predefined temperature field and any initial temperatures creates thermal strains if you specify a thermal expansion coefficient for the assigned material. The specified Temperature Load also affects any temperature-dependent material properties.

For more information, see:

• *TEMPERATURE in the Abaqus Analysis Keywords Reference Guide.

• Predefined fields in the Abaqus Analysis User’s Guide.

Defining a temperature load in the ANSYS environment

In the ANSYS environment, the options in the Temperature Load dialog box correspond to the BF command. You can use the Temperature Load command to define a body force temperature load on selected nodes.

For more information, see BF in the ANSYS Commands Reference manual.

Applying temperature loads from previous analyses

You can apply temperature results from a previous analysis as a load in the current solution using the Temperature Load command. Using the Temperature – External Time Unassigned and Temperature – External Time Assigned options, you can import temperature pre-loads from Nastran (OP2), Abaqus (FIL), ANSYS (RTH), or Simcenter 3D Thermal (BUN) files. For Abaqus, you can also use the Temperature – External option to import either FIL or ODB files and set parameters for how the software extracts the values from the results files.

In addition, in the Abaqus and ANSYS environments, you can use the Temperature Pre-Load options in the Solution Step dialog box to import pre-loads.

Where do I find it?

Application	Pre/Post
Prerequisite	A Simulation file as the work part and displayed part Simcenter Nastran, MSC Nastran, Simcenter 3D Multiphysics, Abaqus, or ANSYS as the specified solver Structural as the specified analysis type
Command Finder	Temperature
Simulation Navigator	Right-click Load Container→New Load→Temperature

How do I

Define a temperature load

Define a temperature load using a node ID table

Define a spatial temperature load

Define a temperature load from an external file

Learn more

Defining temperature loads on Nastran 1D elements

Defining temperature loads on Nastran 2D elements

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Temperature, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });