DEFINITIONS:
Any nonlinearities, such as plasticity and contact (gap) elements, are ignored
Any applied loads are ignored in a modal analysis, i.e., [K] - w^{2}[M] = 0
1) Build the model (remember, you must have stiffness &
mass)
2) Enter the ANSYS Solution processor
3) (Optional) Use 'Reset Options..' if you have used this model for a previous analysis.
4) Pick 'New Analysis' - set it for 'Modal' Analysis
5) Pick 'Analysis Options..'
5a) choose Mode Extraction Method (ANSYS 6.1 DEFAULT method: Block Lanczos)
Block Lanczos: for large symmetric problems, has fast convergence, uses the SPARSE matrix solver
- Specify the Number of modes to extract
- Specify the Number of modes to expand
- usually take defaults on lumped mass (NO) and prestress options (NO)
- usually take the defaults for freq. range, normalization, etc.
5b) choose Mode Extraction Method (SUBSPACE is an option)
SUBSPACE: for large symmetric problems, historically older method
- Specify the Number of modes to extract
- Specify the Number of modes to expand
- usually take defaults on lumped mass (NO) and prestress options (NO)
- take the defaults for SUBSPACE Modal Analysis Options, unless you want a limited freq. range, printout of modes, or a different normalization
- SUBSPACE size, vectors, iterations can effect performance and accuracy
5c) choose Mode Extraction Method (REDUCED is an option)REDUCED (HOUSEHOLDER): faster than SUBSPACE, can be less accurate
- Specify the Number of modes to extract
- Specify the Number of modes to expand
- usually take defaults on lumped mass (NO) and prestress options (NO)
- take the defaults for REDUCED Modal Analysis Options, unless you want a limited freq. range, printout of modes, or a different normalization
- For the REDUCED Method, you must define Master DOF's - user selected for lumped masses, or if you know something about the system; Program Selected for the rest.
5d) choosing POWERDYNAMICS is a special setting which selects the SUBSPACE Iteration method along with the PCG solver
POWERDYNAMICS is often used for very large models (100,000+ DOFs)
5e) other choices for unsymmetric or damped modal analysis, as needed.
6) Define any constraints on the system (forces are not used in modal analysis)
7) Solve (watch for convergence and/or warnings in the Output Window)
8) Postprocessing (General Postproc>):
- Use 'Results Summary' to see what solutions are available.
- Use 'First Set' to look at the first mode shape (eigenvector)
- Use 'Next Set' to look at the next mode shape.
- Use 'PlotCtrls' -> Animante -> Mode Shape to see the vibration