Abaqus/CAE allows you to evaluate hyperelastic material behavior by automatically creating response curves using selected strain energy potentials. When the curve fitting is complete, Abaqus/CAE opens the Visualization module and displays X–Y plots of the test results and a dialog box containing the stability limits for each strain energy potential. You can review the results and adjust the material as necessary. For more information, see “Evaluating hyperelastic and viscoelastic material behavior,” Section 12.4.7.
To display X–Y plots of hyperelastic material behavior:
From the main menu bar, select Material
Evaluatematerial name. The material that you select must include hyperelastic material data.
Tip: You can also select the name of the material in the Material Manager and then click Evaluate.
An Evaluate Material dialog box appears.
If you selected a hyperelastic material that also includes viscoelastic material data, toggle on Perform hyperelastic evaluation if it is not already selected.
If desired, you can also evaluate the viscoelastic behavior of the material. For more information, see “Displaying X–Y plots of viscoelastic material behavior,” Section 12.7.8.
In the Available Input Data field, do the following:
Select the Source option of your choice:
Select Test data if you want Abaqus to calculate the necessary strain energy potential coefficients from the experimental data specified in the material definition.
Select Coefficients if you want Abaqus to use the coefficients specified in the material definition.
If you selected Test data in the previous step, specify the test data type or types that you want Abaqus to use in calculating the strain energy potential coefficients. (Only data types for which you have specified data in the material definition appear in the list.)
If you intend to evaluate the Marlow strain energy potential, specify the test data type that Abaqus will use to define the deviatoric response. You can also specify whether compression, tension, or both types of test data should be used and whether volumetric test data should be used to define the volumetric response. (For more information, see “Marlow form” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.)
Note: If your hyperelastic material model includes lateral nominal strains, temperature-dependent data, or field variables, Marlow will be the only strain energy potential available for evaluation.
From the list of Standard Tests, select one or more tests for which you want response calculations using the data in the material definition.
For each test that you select, enter a minimum and maximum strain value that will be the upper and lower limits for the stress-strain response curves.
Click the Strain Energy Potentials tab, and do the following:
If you selected Test data as a data source, a list of all the available strain energy potentials appears. From the list, select one or more that you want Abaqus to apply to the experimental data. For more information on the strain energy potentials available in Abaqus see “Strain energy potentials” in “Hyperelastic behavior of rubberlike materials,” Section 22.5.1 of the Abaqus Analysis User's Guide.
If you selected Coefficients as a data source, the name of the strain energy potential specified in the material definition appears. You can simply review the information and move on to the next step.
If the material that you are evaluating also includes viscoelastic material properties, click the Viscoelastic tab; you can either toggle off Perform viscoelastic evaluation, or select viscoelastic evaluation options. For more information, see “Displaying X–Y plots of viscoelastic material behavior,” Section 12.7.8.
Click OK to begin the response calculations.
If the evaluation fails during the extraction of material coefficients due to problems with nonlinear curve-fitting, Abaqus/CAE displays a dialog box containing the name of the data (.dat) file; the path to the data file is printed in the message area. The data file provides detailed information on each problem encountered. (For more information on the data file, see “Output,” Section 4.1.1 of the Abaqus Analysis User's Guide.)
If Abaqus completes the tests successfully, Abaqus/CAE enters the Visualization module and displays X–Y plots of the test results in new viewports. (For information on X–Y plots, see Chapter 47, “X–Y plotting.”) The data objects appear in the X–Y Data Manager; you can copy them to an output database or perform any of the tasks that you can perform on other X–Y data in the Visualization module.
In addition, Abaqus/CAE displays an informational dialog box containing the stability limits and coefficients for each hyperelastic strain energy potential. The dialog box also displays the viscoelastic material parameters if a viscoelastic evaluation was performed. Abaqus/CAE displays in the message area the path to the data (.dat) file that contains all the material evaluation information.
If desired, return to the Property module to edit the material data or to evaluate other materials.
For example, if the Strain energy potential for the hyperelastic material was previously set to Unknown, you can use the evaluation results to complete the material definition using the optimal strain energy potential.
