Modal Superposition
Analyzing forced dynamic response for large models can be very time-consuming. You can often improve the performance dramatically by using the modal superposition technique. The following requirements must be met for a modal solution to be possible:
•
The analysis is linear. It is possible, however, that the structure has been subjected to a preceding nonlinear history. The modal response can then be a linear perturbation around that state.
•
There are no nonzero prescribed displacements.
•
The important frequency content of the load is limited to a range that is small when compared to all the eigenfrequencies of the model, so that its response can be approximated with a small number of eigenmodes. In practice, this excludes wave and shock type problems.
•
If the modal solution is performed in the time domain, all loads must have the same dependency on the time.
When using the Structural Mechanics Module, there are four predefined study types for modal superposition:
•
Time Dependent, Modal
•
Frequency Domain, Modal
•
Time Dependent, Prestressed, Modal
•
Frequency Domain, Prestressed, Modal
The two first of these study types consist of two study steps: One step for computing the eigenfrequencies and one step for the modal response. The two latter have three study steps. Before the eigenfrequency step, you solve a static load case in order to get a prestress state used in the eigenfrequency computation.
In practice, you have often computed the eigenfrequencies already, and then want to use them in a modal superposition. In this case, start by adding an empty study, and then add a Time Dependent, Modal or Frequency Domain, Modal study step to it. After having added the study step this way, you must point the modal solver to the solution containing the eigenfrequencies and eigenmodes. You do this by first selecting Show default solver at the study level, and then selecting the eigenfrequency solution to be used in the Eigenpairs section of the generated modal solver.
In a modal superposition, the deformation of the structure is represented by a linear combination of its eigenmodes. The amplitudes of these modes are the degrees of freedom of the reduced problem. You must select which eigenmodes to include in the analysis. This choice is usually based on a comparison between the eigenfrequencies of the structure and the frequency content of the load. As a rule of thumb, select eigenmodes up to approximately twice the highest frequency of the excitation.
In the modal superposition formulation in COMSOL, the full model is projected onto the subspace spanned by the eigenmodes. A problem having the number of degrees equal to the number of included modes is then solved. Note that this differs from many implementations of modal superposition, where it often is assumed that the modal equations are totally decoupled.
An implication of this, is that it is not necessary to assume a certain structure of the damping matrix. Any type of damping which is allowable in the corresponding analysis of the full system can also be used in the modal based analysis.
For many common cases, the modal superposition analysis is not sensitive to whether the eigenmodes were computed using damping or not. The reason is that the eigenmodes of problems with Rayleigh damping and loss factor damping can be shown to be identical to those of the undamped problem, so that the projection to the subspace spanned by the eigenmodes is the same in both cases. For more general damping, it is however recommended that you suppress all contributions to the damping during the eigenfrequency step, and thus base the modal superposition on the solution to the undamped eigenfrequency problem.
Frequency Domain Analysis
All loads are assumed to have a harmonic variation. This is a perturbation type analysis, so only loads having the Harmonic perturbation property selected are then included in the analysis.
Time-Dependent Analysis
Only the factor of the load which is independent of time should be specified in the load features. The dependency on time is specified as Load factor under the Advanced section of the modal solver. This factor is then applied to all loads.
•
Modal Solver and Studies and Solvers in the COMSOL Multiphysics Reference Manual
•
Mechanical Damping and Losses
For an example showing how to perform modal superposition in time and frequency domain, see Various Analyses of an Elbow Bracket: Application Library path Structural_Mechanics_Module/Tutorials/elbow_bracket.