Mechanical APDL Basic Analysis Guide - Ansys

Chapter 1: Getting Started with ANSYS
Note that if you needed to change any of the other material properties, you would double-click on
Linear Isotropic in the previous step. This would cause the dialog box associated with linear isotropic
properties to appear. You could then edit those properties.
Consider another case where you have the requirement for two material models, where the second model
is the same as the first except that it needs to include constants for one more temperature. To perform this
task:
1. In the Define Material Model Behavior dialog box, click on the following menu path: Edit> Copy,
then choose 1 for from Material number, and enter 2 for to Material number. Click on OK. The
Material Models Defined window now includes Material Model Number 2 in its list. If you doubleclick
on Material Model Number 2, the identical material properties appear below Material Model
Number 2 as those listed for Material Model Number 1.
2. Double-click on Nonlinear Isotropic under Material Model Number 2. The associated dialog box
appears.
3. Move the text cursor to the Temperature row in the column furthest to the right, and click on the
Add Temperature button. A T3 column appears.
4. In the new column, enter the new temperature and the four constants associated with this temperature.
5. Click on OK. The dialog box closes. If you double-click on Nonlinear Isotropic under Material Model
Number 2, the associated dialog box appears and reflects the new temperature data that you added
for Material Model Number 2.
1.1.4.4.7. Example: Defining a Material Model Combination
This example is intended to show you how to define a material based on a combination of two material
models. It steps you through a procedure that uses the material model interface to define a material for
simulating cyclic softening at one temperature. This is accomplished by using the Nonlinear Isotropic model
combined with the Chaboche model.
If you performed either of the previous examples in this section, start a new ANSYS session before beginning
the following example.
1. From the ANSYS Main Menu, click on the following menu path: Preprocessor> Material Props> Material
Models. The Define Material Model Behavior dialog box appears.
2. In the Material Models Available window, double-click on the following options: Structural, Linear,
Elastic, Isotropic. A dialog box appears.
3. Enter values for material properties, as required (EX for elastic modulus, and PRXY for Poisson's ratio).
Click on OK. Material Model Number 1 and Linear Isotropic appear in the Material Models Defined
window.
4. In the Material Models Available window, double-click on the following options: Nonlinear, Inelastic,
Rate Independent, Combined Kinematic and Isotropic Hardening Plasticity, von Mises Plasticity.
5. Double-click on Chaboche and Nonlinear Isotropic. A dialog box appears for defining the constants
for the Chaboche model.
6. Enter the first three constants associated with the Chaboche model (click on the Help button for information
on these constants).
7. The Chaboche model allows you to specify more constants. If you choose to specify more constants,
click on the Add Row button, and enter the next constant.
8. Repeat the previous step for all the remaining Chaboche constants that you want to define.
14
Release 13.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.