Define a material with stress-strain data

Video: Create a new nonlinear material based on a library material

The following example shows how to define material plasticity conditions for a nonlinear analysis. In this example, you will edit an isotropic material to have the correct material properties for this type of analysis.

This is also an example of how you can use a table field to define varying material properties and then plot the table field.

In Simcenter Nastran or MSC Nastran, these stress-dependent material properties are exported to a MATS1 bulk data entry. For more information, see MATS1 bulk data entry export.

1. Ensure that the FEM is the work or displayed part.

2. Choose Menu→Tools→Materials→Assign Materials or Manage Materials.

3. In the Material List, select Library Materials.

4. From the Materials list, select Steel, which is an isotropic material in the Default Material Library.

5. Right-click the selected material and choose Copy .The new copy of the material opens in the Isotropic Material dialog box.

6. Select the Mechanical page.

7. Next to the Young's Modulus box, click , and choose Make Formula.

8. In the entry box, replace the formula with a constant value of 26.9e6 in units of lbf/in^2 (psi).

9. Select the Strength page.

10. Next to the Yield Strength box, click , and choose Make Formula, and then replace the formula with a constant value of 34970 in units of lbf/in^2 (psi).

11. Select the Mechanical page.

12. Expand the Stress-Strain Related Properties group.

13. In the list next to Stress-Strain, click , and choose New Field→Table.The Table Field dialog box appears.

14. From the Independent variable list, choose Strain.

15. As described in Defining tabular data, enter strain-stress data points as shown in the following table. Note that the strain value is in the first column. Click OK when finished.000.0013349700.00540000.0143750.015462500.02500000.03525000.0455000In a strain-stress table, the first point is always located at 0,0, and the second must equal (Ys/E, Ys). This results in a slope of E in the elastic data region where Ys is the Yield Strength value and E is the Young's Modulus value. If this point does not match the Yield Strength and Young's Modulus values, the software will correct it when you solve in Nastran. You can also enter additional points to define the data where the strain is greater than Ys/E.

16. You can plot the material properties by clicking , choosing Plot(XY), and selecting an existing viewport with the cursor in the Viewport dialog box.

17. Choose Results tab→Context group→Change Window Drop-down→Return to Model to close the graph.

18. Click OK on the Isotropic Material dialog box.

19. Close the Manage Materials dialog box.

How do I

Model temperature-dependent stress-strain behavior of materials

Learn more

Specifying stress-strain data for nonlinear materials

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Define a material with stress-strain data, 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 } });