1. Chapter Five
Modal Analysis

2. Chapter Overview
In this chapter, performing modal analyses in Design Simulation will be covered. In Design Simulation, performing a modal analysis is similar to a linear analysis.
It is assumed that the user has already covered Chapter 4 Linear Static Structural Analysis prior to this section.
The following will be covered:
Modal Analysis Procedure
Prestressed Modal Analysis Procedure
The capabilities described in this section are generally applicable to ANSYS DesignSpace Entra licenses and above.
Some options discussed in this chapter may require more advanced licenses, but these are noted accordingly.
Harmonic and nonlinear static structural analyses are not discussed here but in their respective chapters.
February 2, 2004
Inventory #002010
5-2

3. Basics of Modal Analysis
A modal analysis, or a free vibration analysis, is performed to obtain the natural frequencies and mode shapes of a structure
Modal analysis does not consider the response of the structure under dynamic loads but rather the natural frequencies. A modal analysis is usually the first step before solving more complicated dynamic problems.
A modal analysis is a subset of the general equation of motion:
February 2, 2004
Inventory #002010
5-3

4. Basics of Modal Analysis
In modal analysis, the structure is assumed to be linear, so the response is assumed to be harmonic:
where fi is the mode shape (eigenvector) and wi is the natural circular frequency for mode i.
By substituting this value in the earlier equation, the following is obtained:
Noting that the solution fi =0 is trivial, wi is solved for:
February 2, 2004
Inventory #002010
5-4

5. Basics of Modal Analysis
For a modal analysis, the natural circular frequencies wi and mode shapes fi are obtained from the matrix equation: This results in certain assumptions related to the analysis:
[K] and [M] are constant:
Linear elastic material behavior is assumed
Small deflection theory is used, and no nonlinearities included
[C] is not present, so damping is not included
{F} is not present, so no excitation of the structure is assumed
The structure can be unconstrained (rigid-body modes present) or partially/fully constrained, depending on the physical structure
It is important to remember these assumptions related to performing modal analyses in Design Simulation.
February 2, 2004
Inventory #002010
5-5

6. A. Modal Analysis Procedure
The modal analysis procedure is very similar to performing a linear static analysis, so not all steps will be covered in detail. The steps in yellow italics are specific to modal analyses.
Attach Geometry
Assign Material Properties
Define Contact Regions (if applicable)
Define Mesh Controls (optional)
Include Supports (if applicable)
Request Frequency Finder Results
Set Frequency Finder options
Solve the Model
Review Results
February 2, 2004
Inventory #002010
5-6

7. … Geometry and Material Properties
Similar to linear static analyses, any type of geometry supported by Design Simulation may be used:
Solid bodies
Surface bodies (with appropriate thickness defined)
Line bodies (with appropriate cross-sections defined)
For line bodies, only mode shapes and displacement results are available.
For material properties, Young’s Modulus, Poisson’s Ratio, and Mass Density are required
Since no loading is assumed, no other material properties will be used, if defined
February 2, 2004
Inventory #002010
5-7

8. … Contact Regions
Contact regions are available in modal analysis. However, since this is a purely linear analysis, contact behavior will differ for the nonlinear contact types, as shown below:
There are two important things to remember when using contact in a modal analysis:
The two nonlinear contact behaviors – rough and frictionless – will behave in a linear fashion, so they will internally behave as bonded or no separation instead.
If a gap is present, the nonlinear contact behaviors will be free (i.e., as if no contact is present). Bonded and no separation contact will depend on the pinball region size.
The pinball region is automatically determined by default
February 2, 2004
Inventory #002010
5-8

9. … Contact Regions
For ANSYS Professional licenses and above, additional contact options are present for use in modal analyses:
For rough and frictionless contact, the “Interface Treatment” can be changed to “Adjusted to Touch,” which will make the contact surfaces behave as bonded and no separation, respectively. (Even if a gap is present, the parts will behave as if they are initially touching if this option is set.)
The size of the “Pinball Region” may be changed as well as viewed to ensure that bonded and no separation contact is established, even if a gap is present.
Please refer to Chapters 3 and 4 for discussions on the pinball region and how to define its size
For ANSYS Structural licenses and above, frictional contact will behave similar to bonded contact if surfaces are touching but act as free (no contact) if contact is open.
It is not recommended to use frictional contact in a modal analysis since it is nonlinear.
February 2, 2004
Inventory #002010
5-9

10. … Loads and Supports
Structural and thermal loads not used in a modal analysis
See Section B later in this chapter for a discussion on prestressed modal analysis. In this situation, loads are considered but only for their prestress effects.
Supports can be used in modal analyses:
If no or partial supports are present, rigid-body modes can be detected and evaluated. These modes will be at 0 or near 0 Hz. Unlike static structural analyses, modal analyses do not require that rigid-body motion be prevented.
The boundary conditions are important, as they affect the mode shapes and frequencies of the part. Carefully consider how the model is constrained.
The compression only support is a nonlinear support and should not be used in the analysis.
If present, the compression only support will generally behave similar to a frictionless support.
February 2, 2004
Inventory #002010
5-10

11. … Requesting Results
Most of the options for modal analyses are similar to that of static analysis. However, Design Simulation knows to perform a modal analysis when the Frequency Finder tool is selected under the Solutions Branch
The Frequency Finder tool adds another branch to the Solutions branch
The Details View of the Frequency Finder allows the user to specify the “Max Modes to Find.” The default is 6 modes (max is 200). Increasing the number of modes to retrieve will increase the solution time.
The search may be limited to a specific frequency range of interest by selecting “Yes” on “Limit Search to Range.
By default, frequencies beginning from 0 Hz (rigid-body modes) will be calculated if a search range is not set.
The minimum and maximum range (in Hz) can be specified if “Limit Search to Range” is enabled. Note that this works in conjunction with “Max Modes to Find.” If not enough modes are requested, not all modes in the frequency range may be found.
February 2, 2004
Inventory #002010
5-11

12. … Requesting Results
Under the Frequency Finder branch are the requests requested
When toggling “Max Modes to Find” under the Frequency Finder branch, more mode shapes will automatically be added. The user does not need to request mode shapes from the Context toolbar.
If stress, strain, or directional displacements are to be requested, this can be done by adding the result from the Context toolbar.
For each stress, strain, or displacement result added, the user can specify which mode this corresponds to from the Details view, under “Mode.”
If stress or strain results are needed, be sure to add results under the Frequency Finder branch, not the Solution branch.
February 2, 2004
Inventory #002010
5-12

13. … Requesting Results
The corresponding ANSYS commands for the Frequency Finder branch is as follows:
If Frequency Finder branch is present, ANTYPE,MODAL is set
The number of modes is set with the nmodes argument, and the beginning and ending search frequencies are specified with freqb and freqe of the MODOPT,,nmodes,freqb,freqe command
All modes are expanded via the MXPAND command. To save disk space and calculation times, the element solution option of MXPAND is not turned on unless stress or strain results are requested.
February 2, 2004
Inventory #002010
5-13

14. … Solution Options
The solution branch provides details on the type of analysis being performed
For a modal analysis, none of the options in the Details view of the Solution branch usually need to be changed.
In the majority of cases, “Solver Type” should be left on the default option of “Program Controlled”.
If the model is a very large one of solid elements, and only a few modes are to be requested, the “Solver Type,” when changed to “Iterative,” may be more efficient.
The “Analysis Type” will display “Free Vibration” for the case of a modal analysis.
February 2, 2004
Inventory #002010
5-14

15. … Solution Options
For a regular modal analysis, none of the solution options except for “Solver Type” have much effect
“Large Deflection” and “Weak Springs” are meant for static analysis cases and should not be changed.
“Solver Type” can be set to “Direct” or “Iterative”
“Program Controlled” or “Direct” result in the Block Lanczos eigenvalue extraction method with the sparse direct equation solver (MODOPT,LANB and EQSLV,SPARSE). This is the most robust eigensolver, as it handles small & large models and beam, shell, or solid meshes, so it is the default option.
“Iterative” results in the PowerDynamics solution method, which is a combination of the subspace eigenvalue extraction method with the PCG equation solver (MODOPT,SUBSP and EQSLV,PCG). The PowerDynamics eigensolver can be efficient for large models of solid elements, when requesting only a few modes.
February 2, 2004
Inventory #002010
5-15

16. … Solving the Model
After setting up the model, one can solve the modal analysis just like any other analysis by selecting the Solve button.
A modal analysis is generally more computationally expensive than a static analysis on the same model because the equations solved for are different.
The Worksheet tab of the Solution branch provides detailed solution output, including the amount of memory being used and how many modes have been extracted already.
If stress or strain results or more frequencies/modes are requested after a solution is performed, a new solution is required.
February 2, 2004
Inventory #002010
5-16

17. … Reviewing Results After solution, mode shapes can be reviewed
Because there is no excitation applied to the structure, the mode shapes are relative values associated with free vibration
Mode shapes (displacements), stresses, and strains represent relative, not absolute quantities
The frequency is listed in the Details view of any result being viewed.
The animation button on the Results Context toolbar can be used to help visualize the mode shapes better.
February 2, 2004
Inventory #002010
5-17

18. … Reviewing Results
The Worksheet tab of the Frequency Finder branch summarizes all frequencies in tabular form
By reviewing the frequencies and mode shapes, one can get a better understanding of the possible dynamic response of the structure under different excitation directions
February 2, 2004
Inventory #002010
5-18

19. B. Prestressed Modal Analysis
In some cases, one may want to consider prestress effects when performing a modal analysis.
The stress state of a structure under constant (static) loads may affect its natural frequencies. This can be important, especially for structures thin in one or two dimensions.
Consider a guitar string being tuned – as the axial load is increased (from tightening), the lateral frequencies increase. This is an example of the stress stiffening effect.
February 2, 2004
Inventory #002010
5-19

20. … Prestressed Modal Analysis
The way in which prestressed modal analyses are solved for is that, internally, two iterations are automatically performed:
A linear static analysis is initially performed:
Based on the stress state from the static analysis, a stress stiffness matrix [S] is calculated:
The prestressed modal analysis is then solved for, including the [S] term
February 2, 2004
Inventory #002010
5-20

21. … Prestressed Modal Procedure
To perform a prestressed modal analysis (also known as a free vibration with prestress analysis), it is the same as running a regular free vibration analysis with the following exceptions:
A load (structural and/or thermal) must be applied to determine what the initial stress state of the structure is.
Results for the linear static structural analysis may also be requested under the Solution branch, not the Frequency Finder branch
A stress or strain result requested under the Frequency Finder branch will be relative stress/strain values for a particular mode
A stress or strain (or displacement) result requested under the Solution branch will be absolute stress/strain/displacement values for the statically applied load
February 2, 2004
Inventory #002010
5-21

22. … Prestressed Modal Example
Consider a simple comparison of a thin plate fixed at one end
Two analyses will be run – free vibration and free vibration with prestress effects – to compare the differences between the two.
Free Vibration
Free Vibration with Prestress
February 2, 2004
Inventory #002010
5-22

23. … Prestressed Modal Example
Notice that the only difference of running a modal analysis with or without prestress is the existence of a load
If a Frequency Finder tool is present and a load is present, Design Simulation knows that a “Free Vibration with Pre-Stress” analysis will be performed.
If results such as displacement, stress, or strains are requested directly underneath the Solution branch, the results from the linear static analysis can be reported.
February 2, 2004
Inventory #002010
5-23

24. … Prestressed Modal Example
In this example, with the applied force, a tensile stress state is produced, thus increasing the natural frequencies, as illustrated below
Free Vibration
1st mode frequency: 141 Hz
Free Vibration with Prestress
1st mode frequency: 184 Hz
February 2, 2004
Inventory #002010
5-24

25. … Prestressed Modal Analysis
For prestressed modal analysis, Design Simulation performs the two necessary iterations internally:
A linear static analysis with PSTRES,ON is run
A modal analysis is then run right afterwards with PSTRES,ON to consider prestress effects
Other items useful for ANSYS users to keep in mind:
No large-deflection prestress effects are currently supported in Design Simulation, so enabling the “Large Deflection: On” in the Solution branch is not permitted.
The equation solver for the static analysis and the eigensolver for the modal analysis currently cannot be independently set. Both will be affected by the “Solver Type” setting in the Solution branch.
February 2, 2004
Inventory #002010
5-25

26. C. Workshop 5 Workshop 5 – Modal Analysis Goal:
Investigate the vibration characteristics of two motor cover designs manufactured from 18 gage steel.
February 2, 2004
Inventory #002010
5-26