Linear Elastic Material
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.
Shell Properties
This section is only present in the Layered Shell interface, where it is described in the documentation for the Linear Elastic Material node. The way the Linear Elastic Material node interacts with material definitions differ significantly between the Layered Shell interface and the other physics interfaces.
Coordinate System Selection
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.
Linear Elastic Material
Define the Material symmetry and the linear elastic material properties.
Material Symmetry
Select the Material symmetryIsotropic, Orthotropic, Anisotropic, or Crystal. Select:
Isotropic for a material that has the same properties in all directions.
Orthotropic for a material that has different material properties in orthogonal directions. It is also possible to define Transversely isotropic material properties.
Anisotropic for a material that has different material properties in different directions.
Crystal for a material that has certain crystal symmetry.
Note: The Orthotropic, Anisotropic, and Crystal options are only available with certain COMSOL products (see https://www.comsol.com/products/specifications/)
In the Layered Shell interface, the chosen material symmetry applies to all selected layers, irrespective of whether the material data is entered explicitly as User defined in the Linear Elastic Material node, or is obtained from a Layered Material node using the default From material option.
Density
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.
Default Model Inputs and Model Input in the COMSOL Multiphysics Reference Manual.
Specification of Elastic Properties for Isotropic Materials
For an Isotropic material, 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.
  D(E,ν)
D(E,G)
  D(K,G)
  D(λ,μ)
E =
ν =
K =
G =
μ
λ =
μ =
cp =
cs =
The individual property parameters are:
Young’s modulus (elastic modulus) E.
Lamé parameter λ and Lamé parameter μ.
Pressure-wave speed (longitudinal wave speed) cp.
Shear-wave speed (transverse wave speed) cs. This is the wave speed for a solid continuum. In plane stress, for example, the actual speed with which a longitudinal wave travels is lower than the value given.
Specification of Elastic Properties for Orthotropic Materials
When Orthotropic is selected from the Material symmetry list, the material properties are different in orthogonal directions (principal directions) given by the axes of the selected coordinate system. The Material data ordering can be specified in either Standard or Voigt notation. When User defined is selected, enter three values in the fields for Young’s modulus E, Poisson’s ratio ν, and the Shear modulus G. The latter defines the relationship between engineering shear strain and shear stress. It is applicable only to an orthotropic material and follows the equation
The Poisson’s ratio νij are defined differently depending on the application field. It is easy to transform among definitions, check which one the reference material uses.
You can set an orthotropic material to be Transversely isotropic. Then, one principal direction in the material is different from two others that are equivalent. This special direction is assumed to be the first axis of the selected coordinate system. Because of the symmetry, the following relations hold:
Thus, only five elasticity moduli need to be entered when the User defined option is selected.
Specification of Elastic Properties for Anisotropic Materials
When Anisotropic is selected from the Material symmetry list, the material properties vary in all directions. They can be specified using either the Elasticity matrix, D or the Compliance matrix, D-1. Both matrices are symmetric. 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.
In 1D and 1D axisymmetry, the elasticity matrix is assumed to represent either isotropic or orthotropic material. Entering components in the elasticity matrix that couple extension and shear, for instance, should be avoided.
Specification of Elastic Properties for Crystals
Because of the material symmetry, only certain components of the elasticity matrix need to be specified. The actual components to enter depend on the selected Crystal systemCubic (3 constants), Hexagonal (5 constants), Trigonal (6 constants), Trigonal (7 constants), Tetragonal (6 constants), Tetragonal (7 constants), or Orthorhombic (9 constants).
Mixed Formulation
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. It is also possible to select an Implicit formulation when an assumption of plane stress is used.
Geometric Nonlinearity
The settings in this section control the overall kinematics, the definition of the strain decomposition, and the behavior of inelastic contributions, for the material.
Select a FormulationFrom 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.
With the default From study step, a total Lagrangian formulation for large strains is used when the Include geometric nonlinearity check box is selected in the study step. If the check box 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 check box in all study steps.
When inelastic deformations are present, such as for plasticity, the elastic deformation can be obtained in two different ways: using additive decomposition of strains or using multiplicative decomposition of deformation gradients.
Select a Strain decompositionAutomatic (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.
When Automatic is selected, a multiplicative or additive decomposition is used with a total Lagrangian formulation, depending on the Include geometric nonlinearity check box status in the study step.
Select Additive to force an additive decomposition of strains.
Select Multiplicative to force a multiplicative decomposition of deformation gradients. This option is only visible if Formulation is set to Total Lagrangian.
The Strain decomposition input is only visible for material models that support both additive and multiplicative decomposition of deformation gradients.
See Lagrangian Formulation, Deformation Measures, and Inelastic Strain Contributions in the Structural Mechanics Theory chapter.
See Modeling Geometric Nonlinearity in the Structural Mechanics Modeling chapter.
See Study Settings in the COMSOL Multiphysics Reference Manual.
This section is only available with COMSOL products that support geometrically nonlinear analysis (see https://www.comsol.com/products/specifications/).
Energy Dissipation
You can select to compute and store various energy dissipation variables in a time-dependent analysis. Doing so will add extra degrees of freedom to the model.
Select the Calculate dissipated energy check box as needed to compute the energy dissipated by for example creep, plasticity, viscoplasticity, viscoelasticity, or damping.
To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box.
Discretization
If Pressure formulation is used, select the discretization for the Auxiliary pressureAutomatic, Discontinuous Lagrange, Continuous, Linear, or Constant. If Strain formulation is used, select the discretization for the Auxiliary volumetric strainAutomatic, Discontinuous Lagrange, Continuous, Linear, or Constant.
The Discretization section is available when Pressure formulation or Strain formulation is selected from the Use mixed formulation list. To display the section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box.
Quadrature Settings
Select the Reduced integration check box to reduce the integration points for the weak contribution of the feature. Select a method for Hourglass stabilizationAutomatic, 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.
Location in User Interface
Context Menus
Ribbon
Physics tab with Solid Mechanics selected:
Physics tab with Layered Shell selected:
Physics tab with Multibody Dynamics selected: