Prestressed Structures
You can analyze eigenfrequency or frequency domain problems where the dynamic properties of the structure are affected by a preload, such as a tensioned string.
Usually, a study of a prestressed problem includes using study steps. The first step is a Stationary step in which the static preload is applied. The effects of the preload can be computed with or without taking geometric nonlinearity into account. In the second study step, where the you compute the eigenfrequency or the frequency response, it is necessary to take geometric nonlinearity into account. Even if the displacements and strains are small, this is what gives the prestress contribution to the equations.
The same principles apply also to a linear buckling analysis, except that both study steps should be geometrically linear. The nonlinear contribution is included in the formulation of the buckling eigenvalue itself.
Follower Loads
Loads which change orientation with deformation, such as a pressure, actually contribute not only to the load, but also to the stiffness. This is a physical effect, and not just a numerical artifact. Whether such loads are included or not in an Eigenfrequency study step will affect the computed eigenfrequencies. If you for some reason do not want this effect, you must suppress the load in the Physics and Variables section of the Eigenfrequency node.
If you use a local coordinate system for describing a load, you must in case of geometric nonlinearity pay attention to whether that coordinate system has constant axis orientations or not. As an example, the default boundary system has Frame set to Deformed Configuration, so that a load represented in that system will behave as a follower load. Change to Reference Configuration if the load should act in fixed directions.
Contact and Frequency Domain Analysis
If a contact is included in the prestress load case, you can perform a subsequent frequency domain analysis in which then the linearization will be made around the computed contact state. It is however not possible perform an eigenvalue analysis based on a contact solution.
Inelastic Stresses and Strains
When inelastic stresses and strains are part of the problem description, you need to make some extra considerations. Such contributions are formally part of the constitutive model, but generate load vector contributions.
There are three Preset study types which can be used to set up these two study steps: Prestressed Analysis, Eigenfrequency; Prestressed Analysis, Frequency Domain; and Linear Buckling.
If you want to explicitly prescribe the stress field for a prestressed analysis rather than solving for it, you should not use the two study step procedure.
In such a case, prescribe the stress field using an Initial Stress and Strain or External Stress node. Then add a separate Eigenfrequency study and select Include Geometric Nonlinearity in the settings for the study step.
Prestressed Analysis, Eigenfrequency, Prestressed Analysis, Frequency Domain, and Linear Buckling in the COMSOL Multiphysics Reference Manual
•
For an example of a general prestressed eigenfrequency analysis see Bracket—Eigenfrequency Analysis: Application Library path Structural_Mechanics_Module/Tutorials/bracket_eigenfrequency.
•
For an example of an analysis where the stress state is explicitly prescribed, see Vibrating Membrane: Application Library path Structural_Mechanics_Module/Verification_Examples/vibrating_membrane.