The Linear Elastic Material node adds the equations for a linear elastic solid and an interface for defining the elastic material properties.

By adding the following subnodes to the Linear 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/). Also, the available options depend on the physics interface in which the Linear Elastic Material is used.

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.

Define the Solid model and the linear elastic material properties.

Select a linear elastic Solid model: Isotropic, Orthotropic, or Anisotropic. Select:

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

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 an Isotropic Solid model, from the Specify list select a pair of elastic properties for an isotropic material — Young’s modulus and Poisson’s ratio, Young’s modulus and shear modulus, Bulk modulus and shear modulus, Lamé parameters, or Pressure-wave and shear-wave speeds. For each pair of properties, select from the applicable list to use the value From material or enter a User defined value or expression.

Each of these pairs define the elastic properties and it is possible to convert from one set of properties to another according to Table 4-1.

When Orthotropic is selected from the Solid model list, the material properties vary in orthogonal directions only. The Material data ordering can be specified in either Standard or Voigt notation. When User defined is selected in 3D, enter three values in the fields for Young’s modulus E, Poisson’s ratio ν, and the Shear modulus G. This defines the relationship between engineering shear strain and shear stress. It is applicable only to an orthotropic material and follows the equation

When Anisotropic is selected from the Solid model list, the material properties vary in all directions, and the stiffness comes from the symmetric Elasticity matrix, D. The Material data ordering can be specified in either Standard or Voigt notation. When User defined is selected, a 6-by-6 symmetric matrix is displayed.

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. For details, see the Mixed Formulation section in the Structural Mechanics Theory chapter.

From the Use mixed formulation list, select None, Pressure formulation, or Strain formulation.

If a study step is geometrically nonlinear, the default behavior is to use a large strain formulation in all domains. Select the Geometrically linear formulation check box to always use a small strain formulation, irrespective of the setting in the study step.

When a geometrically nonlinear formulation is used, the elastic deformations used for computing the stresses can be obtained in two different ways if inelastic deformations are present: additive decomposition and multiplicative decomposition. The default is to use multiplicative decomposition. Select Additive strain decomposition to change to an assumption of additivity.

Note: This section is only available with COMSOL products that support geometrically nonlinear analysis (see https://www.comsol.com/products/specifications/).

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 Layered Shell selected:

Physics tab with Multibody Dynamics selected: