This section describes how to extract material behavior constants from calibration data sets. You can define calibration behaviors for the following material models:
Isotropic elastic
Isotropic elastic-plastic
You can also add support for custom calibration behaviors, which appear as new options in the Calibration Behavior dialog box. For more information, see "Creating custom material calibration plug-ins in Abaqus/CAE" in the Dassault Systèmes DSX.ECO Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com.
The isotropic elastic calibration behavior enables you to derive isotropic elastic data (Young's modulus and Poisson's ratio) from calibration data sets and to apply these material constants to the elastic material properties of a material definition in your model. For more information about elastic material properties in Abaqus/CAE, see “Creating a linear elastic material model” in “Defining elasticity,” Section 12.9.1.
To calibrate data for isotropic elastic material behavior:
From the Model Tree, expand the Calibrations container and double-click Behaviors.
The Create Calibration Behavior dialog box appears.
Enter a name for the material calibration behavior, select Elastic Isotropic, and click Continue.
The Edit Behavior dialog box appears.
From the Parameter Set 1 options, do the following to calculate a value for Young's modulus:
From the Data set list, select the data from which you want to calculate Young's modulus.
Click 
.
Abaqus/CAE computes Young's modulus and displays its value to the right of the Young's modulus label.
From the Parameter Set 2 options, do the following to calculate a value for Poisson's ratio:
From the Data set list, select the data from which you want to calculate Poisson's ratio.
Click .
Abaqus/CAE computes Poisson's ratio and displays its value to the right of the Poisson's ratio label.
From the Material list, select the material definition to which you want to apply this calibration behavior; or click 
to create a new material definition for this calibration behavior. For more information about defining a new material model, see “Creating or editing a material,” Section 12.7.1.
Click OK to save the isotropic elastic behaviors to the selected material model.
Abaqus/CAE adds the new behavior to the model tree and adds the specified Young's modulus and Poisson's ratio to the Elastic material properties for the specified material.
The isotropic elastic-plastic calibration behavior enables you to derive isotropic elastic and plastic material behaviors. For more information about elastic material properties in Abaqus/CAE, see “Creating a linear elastic material model” in “Defining elasticity,” Section 12.9.1; for more information about plastic material properties in Abaqus/CAE, see “Defining classical metal plasticity” in “Defining plasticity,” Section 12.9.2
To calibrate data for isotropic elastic-plastic material behavior:
From the Model Tree, expand the Calibrations container and double-click Behaviors.
The Create Calibration Behavior dialog box appears.
Enter a name for the material calibration behavior, select Elastic Plastic Isotropic, and click Continue.
The Edit Behavior dialog box appears.
From the Elastic-Plastic Data options, do the following:
Expand the Data set list and select the data from which you want to calculate the first set of calibration values.
From the Ultimate point options, either click to calculate the ultimate point automatically or click 
and select the ultimate point from the viewport.
Abaqus/CAE plots the ultimate point in the viewport and displays its coordinates in the dialog box.
From the Yield point options, click and pick the yield point from the viewport.
Abaqus/CAE plots a line between the origin and the yield point in the viewport, displays the coordinates for the yield point in the dialog box, and calculates the Young's modulus and displays its value to the right of the Young's modulus label.
Select the plastic points for this material calibration by doing either of the following:
Drag the Plastic points slider to the right to calculate a greater number of plastic points or drag the slider to the left to calculate fewer plastic points.
Click to pick plastic points from the viewport.
From the Poisson's Ratio Data options, do the following:
From the Data set list, select the data from which you want to calculate Poisson's ratio.
Click .
Abaqus/CAE computes the Poisson's ratio, displays its value in the Poisson's ratio field, and plots it in the viewport. If desired, you can adjust the calculated value of Poisson's ratio by changing the value in the field.
From the Material list, select the material definition to which you want to apply this calibration behavior; or click to create a new material definition for this calibration behavior. For more information about defining a new material model, see “Creating or editing a material,” Section 12.7.1.
Click OK.
Abaqus/CAE updates the new calibration behavior. If you specified a material definition, Abaqus/CAE maps the isotropic elastic-plastic calibration behavior parameters to the Elastic and Plastic material behaviors of that material definition.
Note: Any elastic or plastic material behaviors in the selected material are overwritten when you map data from a calibration behavior to the material definition.