Modeling thermal strain in a Nastran analysis

For Nastran models, there are a number of different ways to define temperature properties for an analysis.

Defining temperature loading

In Nastran, you use the TEMPERATURE(LOAD) case control command combined with the either the TEMP/TEMPP1/TEMPRB and, optionally, the DLOAD/TLOAD1/TABLED1 bulk data entries to define a temperature load.

In Pre/Post, you can:

• Use the Temperature command to apply a temperature load to your model. To apply temperature results from a previous analysis as a load in the current solution, set Type to Temperature - External Time Unassigned.

• Use the Temperature Set command to add your temperature loads to your solution.

When you export or solve a solution that contains a Temperature Set of type Temperature Load, the software writes out a TEMPERATURE(LOAD) case control command and either:

• TEMP/TEMPP1/TEMPRB bulk data entries, if you specified a constant temperature load.

• TEMP/TEMPP1/TEMPRB and DLOAD/TLOAD1/TABLED1 bulk data entries, if you used a field to define varying temperature values.

Defining a default temperature for all other nodes in a solution

In Nastran, if you use a TEMP bulk data entry to specify a temperature value for selected nodes in your model, you must specify a default temperature for all other nodes. In Nastran, you use the TEMPD bulk data entry to define that default temperature.

In Pre/Post, use the Default Temperature field in the Temperature Set dialog box to define the default temperatures for the analysis.

When you export or solve your solution, the software uses the specified default values to write out a TEMPD bulk data entry for all nodes that do not have a defined temperature load for that temperature set.

Defining an initial temperature

In Nastran, you use the TEMPERATURE(INITIAL) case control command combined with the TEMP bulk data entry to define the initial temperature distribution for a solution.

In Pre/Post, you use a Temperature Set of type Initial/Stress Free Temperature to define the initial temperatures for the solution.

Solution Sequence	Role of the TEMPERATURE(INITIAL) command
SOL 101	Defines the strain free temperature used when computing the thermal strain.
Nastran SOL 106 and Simcenter Nastran SOL 601, 106 and SOL 701	Defines the strain free temperature used when computing the thermal strain.It is also used to evaluate temperature dependent material properties when TEMPERATURE(LOAD) is undefined.
Nastran SOL 153	Calculates conduction material properties and provides starting values for the iteration.

When you export or solve a solution that contains a Temperature Set of type Initial/Stress Free Temperature, the software writes out:

• A TEMPERATURE(INITIAL) case control command.

• A TEMP/TEMPP1/TEMPRB bulk data entry.

• A TEMPD bulk data entry for all nodes that do not have a defined temperature load in that temperature set.

Note:

• You cannot include both a TEMPERATURE(INITIAL) and a TEMPERATURE(MATERIAL) case control command in a Nastran input file. If your solution includes a temperature set of either type Initial/Stress Free Temperature or type Material Temperature, the only type of additional temperature sets you can add is Temperature Load.

• If you select the Ignore Material Temperature Dependence option in the Solution dialog box in a nonlinear or advanced nonlinear analysis (SOL 106 Nonlinear Statics, SOL 601, SOL 701), the software also does not export the TEMPERATURE (INITIAL) case control command.

Defining temperature-dependent materials

In Pre/Post, you can use fields to define certain material properties as temperature dependent. If you create an Isotropic material, you can define properties such as the Young's Modulus or Thermal Expansion Coefficient as varying with temperature.

If you define any of a material's properties as being temperature dependent, when you export or solve your model, the software writes out the MATi entry along with the appropriate MATTi and TABLEMi entries. For example, in a structural analysis, if you create an Orthotropic material with temperature-dependent properties, the software writes out the MAT8, MATT8, and TABLEM1/TABLEM2/TABLEM3 entries to your Nastran input file.

Ignoring temperature dependence of materials in selected solutions

If your model includes temperature dependent materials, you can choose not to include the temperature dependence in certain solutions. Use the Ignore Material Temperature Dependence option in the Create Solution dialog box to ignore the temperature-dependent properties during a solution. With this option, you do not have to make any modifications to the material itself.

When you select Ignore Material Temperature Dependence, the software does not write out the MATTi or TABLEM1/TABLEM2/TABLEM3 entries to export the temperature dependence. Instead, it evaluates the material's properties at the material's specified reference temperature, which you define with the Temperature (TREF) option on the Thermal tab of the isotropic, orthotropic, or anisotropic material dialog box. If you do not specify a value for the Temperature (TREF) option, the software exports the material with a reference temperature of 0°.

Learn more

Simcenter Nastran and MSC Nastran environments

Previewing Nastran solver syntax

Controlling the Nastran iterative solver

Allocating DBset size

Printing bulk data in your results file

Customizing a Nastran input file with user defined text

Look up more details

Simcenter Nastran and MSC Nastran boundary conditions

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Modeling thermal strain in a Nastran analysis, 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 } });