Calibrating data for isotropic elastic-plastic material behavior

The isotropic elastic-plastic calibration behavior enables you to derive isotropic elastic and plastic material behaviors.

Related Topics
Creating a linear elastic material model
Defining classical metal plasticity

  1. From the Model Tree, expand the Calibrations container and double-click Behaviors.

    The Create Calibration Behavior dialog box appears.

  2. Enter a name for the material calibration behavior, select Elastic Plastic Isotropic, and click Continue.

    The Edit Behavior dialog box appears.

  3. From the Elastic-Plastic Data options, do the following:

    1. Expand the Data set list and select the data from which you want to calculate the first set of calibration values.
    2. 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.

    3. 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.

    4. 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.

      Abaqus/CAE adds plastic data points to the table in the dialog box. You can edit any of these data if you want to customize further the plastic data.

  4. From the Poisson's Ratio Data options, do the following:

    1. From the Data set list, select the data from which you want to calculate Poisson's ratio.
    2. 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.

  5. 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.

  6. 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.