Defining Hyperelastic Materials

Hyperelastic materials can undergo large elastic deformations under loading, returning to their original shape when the load is removed. In general, you can use hyperelastic models for elastomers (such as rubber) and other materials with similar properties.

Hyperelastic materials have a nonlinear stress-strain relationship that can vary significantly for different modes of deformation (compression, tension, and shear). For this reason, you generally require material test data that comprise all modes of deformation.

Simcenter STAR-CCM+ provides standard Neo-Hookean, Mooney-Rivlin, and Ogden models. These models provide stress-strain curves that are fitted to material test data using appropriate coefficients. To calculate the coefficients, you can use the material calibration curve-fitting tool provided in Simcenter STAR-CCM+.

All models are formulated in terms of the strain energy potential (see Hyperelastic Materials).

  1. To account for large deformations, activate the Nonlinear Geometry model in the solid stress continuum.
By default, Simcenter STAR-CCM+ treats solid materials as compressible. This approach is suitable for hyperelastic materials like highly compressible foams. However, materials like rubbers are nearly incompressible in most cases, as their volume does not change significantly with increasing stress.
  1. To model nearly incompressible materials, also activate the Nearly Incompressible Material model.
  2. Create a material law and assign it to the relevant solid materials, as explained in Defining the Solid Materials.
  3. Right-click the Material Laws > [Material Law 1] > Models node and choose Select models...
  4. In the Material Law 1 Model Selection dialog, activate the following models:
    Group box Model
    Material Stiffness Models Hyperelasticity
    Material Strain Measures Green-Lagrange (Large Strain)
    Hyperelastic Material Models Choose a model based on the available material test data:
    • If you have specific test data for the material, activate either the Mooney-Rivlin or the Ogden model. In general, the Ogden model is suitable for materials with larger strain levels.
    • If you do not have specific test data for the material and the strain is below 20%, activate the Neo-Hookean model.

    For more information on the models formulation, see Hyperelastic Materials.

    Optional Models To calculate the coefficients for the selected hyperelastic model in Simcenter STAR-CCM+, activate the Material Calibration model. This model is optional.


The Mooney-Rivlin and the Ogden models provide different levels of accuracy, allowing you to choose the number of terms that are included in the fitting curve (see Eqn. (4535) and Eqn. (4539)). Choose the level of accuracy based on the experimentally measured stress-strain curves. The number of terms should increase with the number of inflection points in the experimental stress-strain curves.
  1. To specify the number of terms:
    • If you activated the Mooney-Rivlin model, select the [Material Law] > Models > Mooney-Rivlin node and set Model Type to either 2-term, 5-term, or 9-term, as appropriate.

      For more information on these models, see Mooney-Rivlin Model.

    • If you activated the Ogden model, select the [Material Law] > Models > Ogden node and set Model Order to the desired number of terms. You can select a number between 1 and 6.

      For more information on these models, see Ogden Model.

For the Neo-Hookean model, you can define the material properties using either the Neo-Hookean Parameters (that is, bulk modulus and coefficient c10 in Eqn. (4533) and Eqn. (4534)) or Young's Modulus and Poisson's ratio. To choose the method for defining the material properties:
  1. Select the [Material Law] > Models > Neo-Hookean node and set Parameter Set to the desired option.
For each hyperelastic material in the simulation:
  1. Expand the Material Properties node.
    Simcenter STAR-CCM+ adds the relevant material properties under the Material Properties node, based on the specified model.

  2. Specify the material Density.
  3. Specify the remaining properties, which define the parameters for the selected hyperelastic model. For example, a two-term Mooney-Rivlin approach requires the specification of two fitting coefficients and the material bulk modulus. To define these properties, you can use one of the following methods:
    • Define the material properties manually by setting appropriate values on the relevant material property nodes. The properties available for each hyperelastic models are listed in the section Material Law Models Reference: Material Properties.
    • Calculate the values for the material properties in Simcenter STAR-CCM+ using the material calibration curve-fitting tool. This method requires experimental strain-stress measurements for known modes of deformation (uniaxial, biaxial, shear, and volumetric modes). Instructions for using the curve-fitting tool are provided below.
  4. If you define the Neo-Hookean material properties using either a constant value, or a field function dependent on other quantities such as temperature, make sure that:
    • Young's Modulus, Bulk Modulus, and Neo-Hookean Material Parameters (c10) are positive (> 0).
    • Poisson's ratio is between -1 and 0.5.

    If the Neo-Hookean material properties are invalid, the simulation stops.

To calculate hyperelastic model parameters using the curve-fitting tool:
  1. Prepare a .csv table file with two columns of experimental data. The calibration tool requires one of the following data pairs:
    • strain vs uniaxial stress
    • strain vs biaxial stress
    • shear strain vs shear stress
    • volume ratio vs volumetric stress
    In all cases, the first column contains the strain (or volume ratio) measurements, and the second column contains the corresponding stress measurements. For more information on the deformation modes, see Hyperelastic Material Calibration.
  2. In Simcenter STAR-CCM+, right-click the Tools > Tables node, select New Table > File Table, and import the .csv file containing the strain-stress data.
In the relevant physics continuum:
  1. Expand the Material Laws > [Material Law 1] > Models node and make sure that the Material Calibration model is active.
  2. Right-click the Material Calibration > Inputs node and select Add Input Table.
  3. Select the Inputs > [Input Table 1] node and set the following properties:
    Property Setting
    Active Activated
    Exponential Data This property has no effect on hyperelastic material calibration.
    Data Table Select the imported .csv table.
    Input Type Select the type of strain-stress measurements contained in the imported table.
  4. To launch the curve-fitting dialog, right-click the Material Calibration model and select Fitting Tool...
  5. In the Material Parameter Fitting dialog:
    1. For the parameters that you wish to calculate, activate the Active property and set appropriate minimum and maximum values.


    2. To calculate the parameters, select Execute Fit.
      Simcenter STAR-CCM+ fits the imported data and adds the calculated values to the dialog.

      If the tool fails to calculate parameters within the specified range, change the minimum and maximum values and repeat the fitting.

    3. To automatically set the material properties using the calculated values, select Save Parameters, then close the dialog.
    For more information on the functionality and properties available for material calibration, refer to Material Parameter Fitting Dialog, which describes parameter fitting in the context of viscous flow.
  6. If required, continue by defining any thermal properties. See Defining Thermal Properties.
    For more information, see Material Properties.