Fall 2002, METBD 440/451 - FEA Dynamics Applications

Prof. Dave Johnson, dhj1@psu.edu, Penn State - Erie, The Behrend College

MODAL Analysis Template

DEFINITIONS:

• MODE: a natural frequency of a system
• EIGENVALUE: a natural frequency of a system
• EIGENVECTOR:  the mode shape (shown by displacements of the structure)
• a vibration NODE: a location which does not move during vibratory motion

Reference:  ANSYS Structural Analysis Guide, Chapter 3: Modal Analysis

• Any nonlinearities, such as plasticity and contact (gap) elements, are ignored

• Any applied loads are ignored in a modal analysis, i.e., [K] - w²[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