METBD 450 Lecture Notes

Text: Building Better Products with FEA,
by V. Adams & A. Askenazi, (Read pp. 72-87)

Reference:  ANSYS Structural Analysis Guide

Chapter 3: Modal Analysis

DYNAMIC FEA SIMULATION

• MODAL (free vibration) to find the natural frequencies of a system

• HARMONIC (forced - sinusoidal) to determine a system's response to an oscillating input

• TRANSIENT (general) to determine a system's response to general forcing functions, impact, including nonlinear behaviors

Modal Analysis Definitions:

• MODE: a natural frequency of a system.  
  • Natural Frequency: a system will prefer to vibrate at certain frequencies due ONLY to stiffness and mass characteristics of the system
  • Theoretical systems (single DOF) help us understand vibration
  •        Units:  w_n (rad/sec),  f_n (Hz or cycles/sec)
  • Real systems have an infinite number of modes, but we are usually concerned with the first bunch which:
    • may coincide with an operating frequency of the machinery (RESONANCE), and
    • often have the largest (more destructive) amplitude response
• EIGENVALUE: a natural frequency of a system
• EIGENVECTOR: the mode shape (shown by displacements of the FEA model) shows the shape of the structure when it is vibrating at a given natural frequency
• a vibration NODE: a location which does not move during vibratory motion
• Note:
  • 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
• PERIOD: time required for one vibration cycle, T = 1/f_n (in sec/cycle)
• DAMPING: absorbs energy during dynamic simulation
  • causes vibrations to die out if energy is not added to sustain the motion
  • normally, NOT considered in modal analysis

PROCEDURE

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..'

• choose Mode Extraction Method (since 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.

6) Define any constraints on the system (forces are not used in modal analysis)