Fall 2002, METBD 440/451 - FEA Dynamics Applications

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

MODAL Analysis Template


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

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

5b) choose Mode Extraction Method (SUBSPACE is an option)

SUBSPACE: for large symmetric problems, historically older method

5c) choose Mode Extraction Method (REDUCED is an option)

REDUCED (HOUSEHOLDER): faster  than SUBSPACE, can be less accurate

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