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 www.comsol.com/products/specifications/)

The Global coordinate system is selected by default. The Coordinate system list contains all applicable coordinate systems in the component. The coordinate system is used for interpreting directions of orthotropic and anisotropic material data and 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 an 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 checkbox 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 these are known a priori. The Load Reversal Points section enables to set the load reversal points manually based on user defined expressions.

From the list select how to specify the load reversal points — Automatic, None, or User defined. For User defined enter a Boolean expression to fulfill the reversal point for each component of the strain tensor.

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, 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.

When From study step is selected, a total Lagrangian formulation for large strains is used when the Include geometric nonlinearity checkbox is selected in the study step. If the checkbox is not selected, the formulation is geometrically linear, with a small strain formulation.

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 checkbox in all study steps.

Select a Strain decomposition — Automatic, Additive, Logarithmic, 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 the deformation gradient.

Only the additive decomposition of strains is available for the Small-Strain Overlay model.

Select how to compute the energy dissipated by Creep, Plasticity, Viscoplasticity, or other dissipative processes.

Select how to Store dissipation — From physics interface, Individual contributions, Total, Domain ODEs (legacy), or Off.

Use From physics interface to treat the dissipative processes as specified in the settings of the physics interface, see for instance Energy Dissipation in the Solid Mechanics interface.

Use Individual contributions to treat each dissipative process independently. Selecting this option gives a more flexible implementation for problems where dissipation occurs at different time scales, and you want to distinguish each phenomenon separately.

Use Total to accumulate all the dissipative processes into one common variable.

Use Domain ODEs to accumulate the dissipative processes into ODE variables instead of internal state variables.

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 checkbox to reduce the number of integration points used for the weak contribution in the material. Reduced integration give faster computations at the element level and help mitigate locking issues. However, reduced integration may also introduce numerical instabilities, which then require an additional stabilization term.

By default, the Reduced integration checkbox is cleared, except in interfaces designed for explicit dynamic analysis, where it is always selected.

Select a method for Hourglass stabilization — Automatic, Energy sampling, Hessian, Flanagan–Belytschko, Manual, or None to be used in combination with the reduced integration scheme.

The Automatic option selects the stabilization method and its properties based on the physics interface, space dimension, shape function type and order of the displacement field, and the study type.

For the Energy sampling, Hessian, and Flanagan–Belytschko methods, the hourglass stiffness can be scaled by specifying a stiffness multiplier fstb. This multiplier can be an expression of any parameter or variable in the model. This multiplier can be expressed as any parameter or variable in the model. However, to maintain computational efficiency, avoid expensive definitions such as nonlocal coupling operators.

For the hourglass stabilization methods, the stiffness is automatically adjusted during the solution process using an internal multiplier. This accounts for the effect of inelastic deformations, such as damage and plasticity. This correction can be disabled by setting Inelastic deformations to Ignore. Ignoring inelastic deformations may be necessary for scenarios like cyclic loading, where the hourglass stiffness could become too small during unloading. Alternatively, adjust the value for the Minimum stiffness multiplier., which acts as a lower bound for the hourglass stiffness, which is applied in addition to any expression entered for fstb.

For the Energy sampling method, the default stabilization uses an isotropic linear elastic potential. Set the Energy Sampling Potential to Hyperelastic for large deformations. When selected, a neo-Hookean potential is used for nonlinear strains, while linear strains use the linear elastic potential.

The Hessian method evaluates a weak contribution using the reduced integration order. For hexahedral mesh elements, this approach may not suppress all hourglass modes. In most cases, non-stabilized modes are suppressed by constraints adjacent to the domain, but if they are not, select Use full integration to increase the integration order of the stabilization equations to suppress all modes. The higher integration order will increase the computational cost of the stabilization method.

Physics tab with Solid Mechanics selected:

Physics tab with Membrane selected: