Modal Analaysis

1. Modal Analysis
Module 7

2. Octo
ber
30,
2001
Inven
INTRODUCTIONTOANSYS6.0-INTRODUCTIONTOANSYS6.0-
Part2Part2
Training Manual
7. Modal Analysis
• Modal analysis is used to determine a structure’s vibration
characteristics — natural frequencies and mode shapes.
• It is the most fundamental of all dynamic analysis types and
is generally the starting point for other, more detailed
dynamic analyses.
• In this chapter, we will describe how to do a basic modal
analysis via the following topics:
A. Procedure
B. Workshop
For details, refer to your Structural Analysis Guide or
Dynamics Training Manual.

3. Octo
ber
30,
2001
Inven
INTRODUCTIONTOANSYS6.0-INTRODUCTIONTOANSYS6.0-
Part2Part2
Training Manual
Modal Analysis
A. Procedure
• The steps to do a modal analysis are as follows:
– Preprocessing
• Geometry
• Meshing
– Solution
• Analysis Type and Options
• Loading
• Solve
– Postprocessing
• Review results

4. Octo
ber
30,
2001
Inven
INTRODUCTIONTOANSYS6.0-INTRODUCTIONTOANSYS6.0-
Part2Part2
Training Manual
Modal Analysis
...Procedure
Geometry & Meshing
• Same considerations as a static analysis:
– Include as many details as necessary to sufficiently represent
model geometry.
– A fine mesh will be needed to resolve complex mode shapes.
• Both Young’s modulus and density are required.
– Specify mass density instead of weight density when using
British units.
• weight density (lb/in3
) ÷ g (in/sec2
) = mass density (lb-sec2
/in4
)
• For example, density of steel = 0.283/386 = 7.3E-04 lb-sec2
/in4
• Linear elements and material properties only. Nonlinearities
are ignored.

5. Octo
ber
30,
2001
Inven
INTRODUCTIONTOANSYS6.0-INTRODUCTIONTOANSYS6.0-
Part2Part2
Training Manual
Modal Analysis
...Procedure
Analysis Type
• The analysis type is modal.
– Solution > -Analysis Type- New Analysis
– Or issue ANTYPE,MODAL

6. Octo
ber
30,
2001
Inven
INTRODUCTIONTOANSYS6.0-INTRODUCTIONTOANSYS6.0-
Part2Part2
Training Manual
Modal Analysis
...Procedure
Analysis Options
• Mode extraction options
– MODOPT command or Solution >
Analysis Options...
– Method: Block Lanczos is generally
recommended.
– Number of modes: Specify the
number of modes you want to extract.
• Mode expansion options
– MXPAND command or Solution >
Analysis Options...
– Expanding modes allows you to view
them in the postprocessor.
– Number of modes is usually the same
as the number extracted.
• Prestress effects
– PSTRES command or Solution >
Analysis Options...
– calculate mode shapes of a
prestressed structure, such as a
spinning turbine blade.
Default settings are
usually sufficient

7. Octo
ber
30,
2001
Inven
INTRODUCTIONTOANSYS6.0-INTRODUCTIONTOANSYS6.0-
Part2Part2
Training Manual
Modal Analysis
...Procedure
Loading & Solve
• The only “loads” valid in a modal analysis are
displacement constraints:
– Solution > -Loads- Apply > Displacement >
– Or use the D family of commands: D, DK, DL, DA,
etc.
• If you don’t specify constraints, ANSYS will
calculate rigid body modes (zero frequency).
• After all constraints have been specified, obtain the solution:
– First save the database (SAVE command or Toolbar > SAVE_DB).
– Then issue SOLVE (or Solution > -Solve- Current LS).

8. Octo
ber
30,
2001
Inven
INTRODUCTIONTOANSYS6.0-INTRODUCTIONTOANSYS6.0-
Part2Part2
Training Manual
Modal Analysis
...Procedure
Review Results
• POST1 (the general postprocessor) is used to review modal analysis
results.
• Typically, the first step is to list the natural frequencies:
– General Postproc > Results Summary
– Or issue SET,LIST
– Note that each mode is stored in a separate substep.

9. Octo
ber
30,
2001
Inven
INTRODUCTIONTOANSYS6.0-INTRODUCTIONTOANSYS6.0-
Part2Part2
Training Manual
Modal Analysis
...Procedure
• To plot a mode shape:
– First read results for that substep
• General Postproc > Results Summary...
• Or use the SET command
– Then plot the deformed shape
• General Postproc > Plot Results >
Deformed Shape
• Or use the PLDISP command

10. Octo
ber
30,
2001
Inven
INTRODUCTIONTOANSYS6.0-INTRODUCTIONTOANSYS6.0-
Part2Part2
Training Manual
Modal Analysis
...Procedure
• You can also animate mode shapes:
– Utility Menu > PlotCtrls > Animate > Mode Shape
– Or use the ANMODE command
• Another option is to plot contours stresses and strains. Note,
however, that displacement and stress values are simply relative
numbers and have no real meaning.

11. Octo
ber
30,
2001
Inven
INTRODUCTIONTOANSYS6.0-INTRODUCTIONTOANSYS6.0-
Part2Part2
Training Manual
Modal Analysis
B. Workshop
• This workshop consists of the following problem:
W6. U-Bracket
Please refer to your Workshop Supplement for instructions.