Modeling thermal strain

You can model thermal strain by defining an initial set of stress free temperatures and applying additional temperature loads.

Defining initial temperatures

The software automatically creates a Temperature Set of type Initial/Stress Free Temperature when you create a Multiphysics Structural or Coupled solution, or a Simcenter Nastran SOL 401 or SOL 402.

Double-click the Initial/Stress Free Temperature temperature set to change the default temperature. Use the Temperature command to define additional, initial temperatures for your solution. The software uses the temperature set's default temperature for all nodes that do not have a defined temperature load in the initial temperature set.

Note:

The software creates the initial temperature set with a default temperature of 20° C or 68° F.

Defining temperature loading

You use a Temperature Set of type Temperature Load to define the load temperatures for the solution.

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.

Note:

If you create temperatures with time assigned values, you cannot place time assigned and time unassigned temperatures in the same temperature set.

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 Material, Orthotropic Material, 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°.

Corresponding Nastran Syntax

• The Initial/Stress Free Temperature set corresponds to the TEMPERATURE(INITIAL) case control command.

• The Temperature Load type of temperature set corresponds to the TEMPERATURE(LOAD) case control command.

• The Temperature command corresponds to the TEMP, DTEMP, or DTEMPEX bulk entries.

• The Default Temperature field in the Temperature Set dialog box corresponds to the TEMPD bulk entry.

Where do I find it?

Application	Pre/Post
Prerequisite	A Simulation file as the work part and the displayed partSimcenter Nastran or Simcenter 3D Multiphysics as the specified solverStructural or Coupled as the specified analysis typeSOL 401 Multi-Step Nonlinear (Simcenter Nastran), SOL 402 Multi-Step Nonlinear Kinematics (Simcenter Nastran), or Multi-Step Nonlinear (Multiphysics) as the specified solution
Simulation Navigator	Right-click the temperature set node→New→Temperature

Learn more

SOL 401 Multi-Step Nonlinear

SOL 401 Multi-Step Nonlinear workflow

SOL 402 Multi-Step Nonlinear Kinematics

SOL 402 Multi-Step Nonlinear Kinematics workflow

Controlling plasticity and creep effects

Controlling the sequence of bolt pre-loads (SOL 401)

Element Add/Remove (SOL 401)

Simcenter Nastran SOL 401 Co-simulation with Simcenter STAR-CCM+

Complex modes analysis (SOL 402)

Displaying graphs in the Solution Monitor using the Report simulation object

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Modeling thermal strain, 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 } });