Defining temperature loads on Nastran 2D elements

You can use the Through Thickness (Temperature and Gradient) and Through Thickness (Top and Bottom) options in the Temperature dialog box to define temperature loads for certain types of 2D elements.

• Use the Through Thickness (Temperature and Gradient) option to define the temperature and gradient in the thickness direction for the element.

• Use the Through Thickness (Top and Bottom) option to define temperatures for additional membrane stress calculation at the lower and upper surface of 2D elements.

Supported element types

You can use the Through Thickness (Temperature and Gradient) and Through Thickness (Top and Bottom) option to define temperatures on the following types of 2D elements:

• CQUAD4

• CQUAD8

• CTRIA3

• CTRIA6

• CQUADR

• CTRIAR

Specifying the temperature at the element’s reference plane

With the Through Thickness (Temperature and Gradient) option, you can use the Temperature at Element Reference Plane option to specify the temperature at the element’s reference plane.

• In Nastran, you use the ZOFFS field on the element’s bulk data entry (such as CQUAD4) to define the offset distance from the surface of the element’s nodes to the element’s reference plane.

• In Pre/Post, you use the Shell Offset option in the Mesh Associated Data dialog box to define this ZOFFS offset distance.

Specifying the temperatures at Z1 and Z2

With the Through Thickness (Top and Bottom) option, you can use the Temperature at Z1 and Temperature at Z2 options to define the temperatures for an additional membrane stress calculation at points Z1 and Z2.

• In Nastran, you use the Z1 and Z2 fields on the PSHELL bulk data entry to define the fiber distances that the software uses for these additional membrane stress calculations. By default, Z1 and Z2 are equal to one-half of the plate thickness. The positive direction is determined by the right-hand rule.

• In Pre/Post, you use the Fiber Distance, Z1 and Fiber Distance, Z2 options in the PSHELL physical property table dialog box to define the fiber distances.

Additional information

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

• Offsetting Shell Elements in the Simcenter Nastran Element Library Reference Manual

• TEMPRB in the Simcenter Nastran Quick Reference Guide

• PSHELL in the Simcenter Nastran Quick Reference Guide

Where do I find it?

Application	Pre/Post
Prerequisite	An active Simulation file with Simcenter Nastran or MSC Nastran as the specified solver and Structural as the specified analysis type
Command Finder	Temperature
Simulation Navigator	Under the appropriate solution containing a temperature set, right-click Temperature Set→New→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

Temperature

Defining temperature loads on Nastran 1D elements

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Defining temperature loads on Nastran 2D elements, 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 } });