Eigenfrequency Analysis
An eigenfrequency study solves for the eigenfrequencies (natural frequencies) and the shapes of the corresponding eigenmodes.
When performing an eigenfrequency analysis, you can specify whether to look at the mathematically more fundamental eigenvalue, λ, or the eigenfrequency, f, which is more commonly used in a structural mechanics context. The relation between the two is
where i is the imaginary unit.
The undamped eigenvalue problem is commonly written as
where K is the stiffness matrix, M is the mass matrix, u is the eigenmode displacement vector, and ω = 2πf is the angular frequency. In case of damping, the eigenvalue equation is expanded to
(2-1)
where C is the viscous damping matrix, and K may be complex valued.
Because only the shape and not the size of the modes (eigenvectors) have physical significance, the computed modes can be scaled arbitrarily. You can select the method for scaling in the Eigenvalue Solver node of the solver sequence. If Scaling of eigenvectors is set to Mass matrix, the eigenmodes u are orthogonalized with respect to the mass matrix M so that
(2-2)
This is a common choice for the scaling of eigenvectors within the structural mechanics field. The choice of eigenvector scaling does not affect for example the results of a subsequent mode superposition analysis, but it will affect the interpretation of an exported modal representation of the system.
Modal Participation Factors
Modal (or ‘mass’) participation factors are useful tools when working with the modal representation of a structure. Through them, you can get the following information:
To compute modal participation factors, a Participation Factors node must be present under Definitions in the current component. When you add an Eigenfrequency study from the Add Study window, such a node is automatically created.
You can also add it manually under Definitions>Variable Utilities. If you do that after an eigenfrequency study has been run, you need to do an Update Solution in order to get access to the variables containing the participation factors.
The modal participation factors are available as global variables, and these can for example be displayed in a table using a Global Evaluation node under Derived Values in the Results branch. The participation factor results are available as predefined variables in the Definitions submenu for the component. In Table 2-1, the variables created from a Participation Factors node is listed (assuming the default tag mpf1).
The normalized participation factors are those which would be obtained if mass matrix scaled eigenmodes would have been used.
If a Participation Factors node is present in the model when an eigenfrequency study is run, an evaluation group named Participation Factors is automatically generated. It contains a table with the translational and rotational modal participation factors for all computed eigenfrequencies.
For an example showing how to compute modal participation factors and modal mass, see In-Plane Framework with Discrete Mass and Mass Moment of Inertia: Application Library path Structural_Mechanics_Module/Verification_Examples/inplane_framework_freq.
In the COMSOL Multiphysics Reference Manual:
In the theory chapter of the Structural Mechanics User’s Guide:
It is possible to compute eigenfrequencies for structures which are not fully constrained; this is sometimes referred to as free-free modes. For each possible rigid body mode, there is one eigenvalue which in theory is zero. The number of possible rigid body modes for different geometrical dimensions is shown in the table below.
The computed rigid body modes will in general not be recognizable as having pure translation or rotation. Rather, they will contain linear combinations of all the fundamental rigid body motions.
In a piezoelectric model, one more zero eigenfrequency could appear if you have not set a reference value for the electric potential.
In practice, the natural frequencies of the rigid body modes are not computed as exactly zero, but can appear as small numbers which can even be negative or complex. If rigid body modes are present in the model, then it is important to use a nonzero value in the Search for eigenfrequencies around text field in the settings for the Eigenfrequency study step. The value should reflect the order of magnitude of the first important nonzero eigenfrequency.
For an example showing an eigenfrequency computation in a model having a rigid body mode, see Eigenfrequency Analysis of a Free Cylinder: Application Library path Structural_Mechanics_Module/Verification_Examples/free_cylinder.
Damping
If any type of damping is included in the model, an eigenfrequency solution automatically returns the damped eigenvalues. The eigenfrequencies and, in general, also the mode shapes are complex in this case. A complex-valued eigenfrequency can be interpreted so that the real part represents the actual frequency, and the imaginary part represents the damping. The damping ratio of the corresponding eigenmode can be defined as
where the approximate expression is valid with high accuracy (within 2%) as long as long as the damping is less than 0.2.
In a complex mode shape there are phase shifts between different parts of the structure, so that not all points reach the maximum at the same time under free vibration.
Some damping types will still give real valued eigenmodes, this is the case for Rayleigh damping and loss factor damping.
Prestressed Analysis
In a loaded structure, the natural frequencies may be shifted due to stress stiffening.
To do a prestressed analysis, Include geometric nonlinearity must be selected in the Eigenfrequency study step. This is automatic when you add the Eigenfrequency, Prestressed study type.
The prestress loading can include a contact analysis, in which case the subsequent eigenfrequency analysis provide as linearization around the current contact state.
Frequency Dependent Material Properties
If the material data (stiffness or damping) is frequency dependent, the eigenvalue problem will become nonlinear. The most common case is when there are viscoelastic materials in the structure. In this case, the eigenvalue equation Equation 2-1 becomes
(2-3)
The eigenvalue solver as such assumes that the matrices involved are constant, so they must be evaluated at a certain frequency, the linearization point.
(2-4)
In order to get a correct solution to Equation 2-3, the linearization point ωL must be close to the actual eigenvalue ω. This is in general possible only for one single eigenfrequency at a time. You must solve this problem either by manual iteration, or by using some type of scripting, for example through a model method.
Eigenmodes of a Viscoelastic Structural Damper: Application Library path Structural_Mechanics_Module/Dynamics_and_Vibration/viscoelastic_damper_eigenmodes.