The Nonlinear Elastic Material feature is used to model stress-strain relationships which are nonlinear even at infinitesimal strains. It is available in the Solid Mechanics and Membrane interfaces. This material model requires either the Nonlinear Structural Materials Module or the Geomechanics Module. Nonlinear Elastic Material is available for 3D, 2D, and 2D axisymmetry.

By adding the following subnodes to the Nonlinear Elastic Material node you can incorporate many other effects:

Note: Some options are only available with certain COMSOL products (see https://www.comsol.com/products/specifications/)

The Global coordinate system is selected by default. The Coordinate system list contains any additional coordinate systems that the model includes (except boundary coordinate systems). The coordinate system is used when stresses or strains are presented in a local system. The coordinate system must have orthonormal coordinate axes, and be defined in the material frame. Many of the possible subnodes inherit the coordinate system settings.

Nonlinear Structural Materials Module: Select a Material model: Ramberg–Osgood, Power law, Uniaxial data, Shear data, Bilinear elastic, or User defined.

Geomechanics Module: Select a Material model: Ramberg–Osgood, Hyperbolic law, Hardin–Drnevich, Duncan–Chang, Duncan–Selig, Small strain overlay, or User defined.

All nonlinear elastic material models have density as an input. The default Density ρ uses values From material. For User defined enter another value or expression.

If any material in the model has a temperature dependent mass density, and From material is selected, the Volume reference temperature list will appear in the Model Input section. As a default, the value of Tref is obtained from a Common model input. You can also select User defined to enter a value or expression for the reference temperature locally.

For a material with a very low compressibility, using only displacements as degrees of freedom may lead to a numerically ill-posed problem. You can then use a mixed formulation, which adds an extra dependent variable for either the pressure or for the volumetric strain, see the Mixed Formulation section in the Structural Mechanics Theory chapter.

From the Use mixed formulation list, select None, Pressure formulation, or Strain formulation. It is also possible to select an Implicit formulation when an assumption of plane stress is used.

Select from the applicable list to use the value From material or enter a User defined value or expression.

From the Specify list select a pair of elastic properties for an isotropic material — Young’s modulus and Poisson’s ratio (the default for Ramberg–Osgood, Power law, Duncan–Chang, and Duncan–Selig) or Bulk modulus and shear modulus (the default for Hyperbolic law and Hardin–Drnevich).

For Uniaxial data the Uniaxial stress function σax uses the value From material (if it exists) or User defined. If User defined is selected from the list, the default expression for σax is the linear function 210[GPa]*<physics>.eax, which corresponds to a linear elastic material with a Young’s modulus of 210 GPa. The variable <physics>.eax corresponds to the elastic uniaxial strain in pure axial loading, and is named using the scheme <physics>.eax, for example, solid.eax.

From the Specify list select how to specify the second elastic property for the material — Bulk modulus or Poisson’s ratio. Then, depending on the selection, enter a value or select from the applicable list to use the value From material or enter a User defined value or expression:

When you select Bulk modulus, the Young’s modulus is computed from the tensile part of the Uniaxial stress function σax. When you select Poisson’s ratio, you can either use the tensile part (default), or use the full tensile-compressive curve by selecting the check box Use nonsymmetric stress-strain data.

For Shear data the Shear stress function τ uses the value From material (if it exists) or User defined. If User defined is selected from the list, the default expression for τ is the linear function 80[GPa]*<physics>.esh, which corresponds to a linear elastic material with a shear modulus of 80 GPa. The variable <physics>.esh corresponds to the elastic shear strain in pure shear loading, and it is named using the scheme <physics>.esh, for example, solid.esh.

The default Bulk modulus K uses values From material. For User defined enter another value or expression.

For Bilinear elastic enter a value or select from the applicable list to use the value From material or enter a User defined value or expression.

In case of cyclic loading the load reversal points are automatically detected. But in many cases the load reversal points are known a priori. The Load Reversal Points section enables to set the load reversal points manually based on a loading parameter.

In the User defined material model, you specify the bulk modulus implicitly by entering the relation between pressure and volumetric elastic strain. Enter a value or select from the applicable list to use the value From material or enter a User defined value or expression.

Select a Formulation — From study step (default), Total Lagrangian, or Geometrically linear to set the kinematics of the deformation and the definition of strain. When From study step is selected, the study step controls the kinematics and the strain definition.

To have full control of the formulation, select either Total Lagrangian, or Geometrically linear. When Total Lagrangian is selected, the physics will force the Include geometric nonlinearity check box in all study steps.

Select a Strain decomposition — Automatic (default), Additive, or Multiplicative to decide how the inelastic deformations are treated. This option is not available when the formulation is set to Geometrically linear.

The Strain decomposition input is only visible for material models that support both additive and multiplicative decomposition of deformation gradients.

Select the Calculate dissipated energy check box as needed to compute the energy dissipated by Creep, Plasticity, Viscoplasticity, or Viscoelasticity.

To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box.

If Pressure formulation is used, select the discretization for the Auxiliary pressure — Automatic, Discontinuous Lagrange, Continuous, Linear, or Constant. If Strain formulation is used, select the discretization for the Auxiliary volumetric strain — Automatic, Discontinuous Lagrange, Continuous, Linear, or Constant.

Select the Reduced integration check box to reduce the integration points for the weak contribution of the feature. Select a method for Hourglass stabilization — Automatic, Manual, or None to use in combination with the reduced integration scheme. The default Automatic stabilization technique is based on the shape function and shape order of the displacement field.

Control the hourglass stabilization scheme by using the Manual option. Select Shear stabilization (default) or Volumetric stabilization.

When Shear stabilization is selected, enter a stabilization shear modulus, Gstb. The value should be in the order of magnitude of the equivalent shear modulus.

When Volumetric stabilization is selected, enter a stabilization bulk modulus, Kstb. The value should be in the order of magnitude of the equivalent bulk modulus.

Physics tab with Solid Mechanics selected:

Physics tab with Membrane selected: