Use the Damping subnode to add several types of damping to the material model. Damping can be used in Time Dependent, Eigenfrequency, and Frequency Domain studies; for other study types the settings in the Damping subnode are ignored.

You can add the Damping subnode to the Linear Elastic Material, the Nonlinear Elastic Material, and the Hyperelastic Material.

The available damping models differs between various COMSOL products (see http://www.comsol.com/products/specifications/).

The applicability of the different types of damping are summarized in Table 4-4.

Select a Damping type, and enter settings depending on the type.

In this damping model, the damping parameter ξ is expressed in terms of the mass m and the stiffness k as

That is, Rayleigh damping is proportional to a linear combination of the stiffness and mass; there is no direct physical interpretation of the mass damping parameter αdM and the stiffness damping parameter βdM.

Select Input parameters — Alpha and beta — to enter the damping parameters explicitly, or Damping ratios to derive the damping parameters from the damping ratio at two frequencies.

When Alpha and beta is selected, the Mass damping parameter αdM and the Stiffness damping parameter βdK.

When Damping ratios is selected, enter two pairs of frequencies, f1 and f2, and the corresponding damping ratios ζ1 and ζ2 at these frequencies. The Rayleigh damping parameters are computed as

The isotropic loss factor damping is described by the single isotropic loss factor ηs, which acts on all entries in the elastic constitutive matrix. It can be used for isotropic, orthotropic, and anisotropic materials.

When Isotropic loss factor is selected, use the Isotropic structural loss factor list to select the way to enter ηs. The default is to take the value From material. For User defined, enter another value or expression.

An elastic material is in general described by a symmetric 6-by-6 elasticity matrix D. The loss can be isotropic or anisotropic, and is described by either the isotropic loss factor ηs or by a symmetric anisotropic 6-by-6 loss factor matrix ηD or ηDVo. The orientations are the same as in the parent node.

When Anisotropic loss factor is selected, use the Loss factor for elasticity matrix D list to select the way to enter ηD or ηDVo. The default is to take the values From material. For User defined enter the components of ηD or ηDVo in the upper-triangular part of a symmetric 6-by-6 matrix.

An orthotropic material is described by three Young’s modulus components (Ex, Ey, and Ez) and three shear modulus components (Gxy, Gyz, and Gxz). For an orthotropic material, loss factors can be specified in three different ways:

When Orthotropic loss factor is selected, use the Loss factor for orthotropic Young’s modulus list to select the way to enter ηE. The default is to take the values From material. For User defined enter other values or expressions.

Use the Loss factor for orthotropic shear modulus list to select the way to enter ηG or ηGVo. The default is to take the values From material. For User defined, enter other values or expressions.

With viscous damping, the material will get additional stresses proportional to the strain rate. Enter Bulk viscosity ηb and Shear viscosity ηv to model damping caused by volume change and deformation, respectively.

Enter the Loss factor for stiffness matrix DA, ηDA; Loss factor for stiffness matrix DB, ηDB; Loss factor for stiffness matrix DD, ηDD; and Loss factor for stiffness matrix DAs, ηDAs.

The default for all section properties is to take the values From material. Any one of the loss matrices can also be User defined. In that case, selecting Isotropic input is identical to selecting Diagonal input and entering the same value in all three diagonal components. In most cases, the Symmetric input option is the most relevant, since that is the only one in which a loss factor can be assigned to all elements in the section stiffness matrices.

Physics tab with Linear Elastic Material, Layered Linear Elastic Material, Hyperelastic Material, or Nonlinear Elastic Material node selected in the model tree: