MET 425 Lecture Notes

Reference: ANSYS Help System > Mechanical APDL (formerly ANSYS) > Structural Analysis Guide > Chapters 3 (Modal), 4 (Harmonic), 5 (Transient) 

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

• [WB has Modal, Harmonic Response, Transient, Random Vibration, Response Spectrum, Rigid Dynamics & Explicit Dynamics  simulation choices]

Dynamic analyses are required when a useful answer cannot be determined by static analysis methods.

Additional data is required:

• models must have inertia (mass)

• Load steps, substeps, and equilibrium iterations may be important

• time integration may be needed - user guides solution accuracy (and success) by time step size selection (ITS)

Large amount of output data may be produced - control large file content/size and location

Time history postprocessing (in addition to general postproc.) may be useful

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
• In MODAL analysis the deflections are "normalized" - not real displacements.  Also, stresses and forces are NOT available
• Free vibration (no constraints) - is rigid body motion a problem ?

PROCEDURE (Workbench) 

1. Create a  Modal analysis object in the Project Schematic

2. Create or import a model for the analysis (must have stiffness & mass)

3.  Initial Conditions: None or a previous structural analysis ( if pre-stressed**)

4. Analysis Settings:

a.      No. of modes to find (default: 6)

b.      Search Range, if desired

5. Analysis Data Management: Where are the solution files written ? 

6. View vibration mode shape (and animation) using Total Deformation plot:

Click on upper-left corner of “Tabular Data,” right-mouse > “Create Mode Shape Results” to set up a total deformation plot for each mode.

PROCEDURE (ANSYS)

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)

Pre-stressed Modal Analysis

Used to calculate the frequencies and mode shapes of a prestressed structure, such as a spinning turbine blade. The procedure to do a prestressed modal analysis is essentially the same as a regular modal analysis, except that you first need to prestress the structure by doing a static structural analysis

PROCEDURE (Workbench) 

1.  Create a  Static Structural analysis object in the Project Schematic with proper constraint and loads to create the prestress condition.  Establish the solution and results for the static structural simulation, then:

2.  In the WB Project Schematic, drag and drop a Modal Analysis object onto the "Solution" line of the Static Structural analysis object.  This links the material, model, mesh, constraints, and the stress-state from the static structural to the new modal object.

The Modal "Initial Conditions" are then linked to reference the previous "Static Structural" analysis results
[WB uses the same model, materials, mesh, and constraints to solve the modal analysis and includes the stresses created by the static structural simulation]

PROCEDURE (ANSYS)

1. Create a static structural analysis with proper constraint and loads to create the prestress conditions
    
2. Solve the static analysis including a request to calculate prestress effects (command: PSTRES,ON)
    
3. Postprocess, as usual - do NOT delete any of the scratch files from the static structural analysis
   [specifically the files, jobname.emat and jobname.esav, are needed later]
    
4. Re-enter solution and set up a new, modal analysis, request prestress effects (command: PSTRES,ON)
    
5. Set modal analysis options (described above)
    
6. Use the same constraints as the static analysis model.
    
7. Solve and postrocess the prestressed modal analysis