1. Chapter Five
Vibration Analysis

2. Chapter Overview
In this chapter, performing free vibration analyses in Simulation will be covered. In Simulation, performing a free vibration analysis is similar to a linear static 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:
Free Vibration Analysis Procedure
Free Vibration with Pre-Stress 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.
March 29, 2005
Inventory #002215
5-2

3. Basics of Free Vibration Analysis
For a free vibration analysis, the natural circular frequencies wi and mode shapes fi are calculated from: 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
Mode shapes {f} are relative values, not absolute
It is important to remember these assumptions related to performing free vibration analyses in Simulation.
March 29, 2005
Inventory #002215
5-3

4. A. Free Vibration Analysis Procedure
The free vibration 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 free vibration 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
March 29, 2005
Inventory #002215
5-4

5. … Geometry and Point Mass
Similar to linear static analyses, any type of geometry supported by 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.
The Point Mass feature can be used:
Input for the Point Mass was described earlier in Chapter 4.
The Point Mass adds mass only in a free vibration analysis. It is connected to selected surfaces as if no stiffness is present, so the effect is to add only mass (not stiffness) to a structure.
Useful for including the effect of distributed weight on selected surfaces. Because of this, the Point Mass will decrease the natural frequency in free vibration analyses.
March 29, 2005
Inventory #002215
5-5

6. … Material Properties
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
March 29, 2005
Inventory #002215
5-6

7. … Contact Regions
Contact regions are available in free vibration analyses. However, since this is a purely linear analysis, contact behavior will differ for the nonlinear contact types:
There are two important things to remember when using contact in a free vibration 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
March 29, 2005
Inventory #002215
5-7

8. … Contact Regions
For ANSYS Professional licenses and above, additional contact options can be used in free vibration 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 free vibration analysis since it is nonlinear.
March 29, 2005
Inventory #002215
5-8

9. … Loads and Supports
Structural and thermal loads not used in free vibration
See Section B later in this chapter for a discussion on free vibration with pre-stress analysis. In this situation, loads are considered but only for their pre-stress effects.
Supports can be used in free vibration 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, free vibration 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.
March 29, 2005
Inventory #002215
5-9

10. … Requesting Results
Most of the options for free vibration analyses are similar to that of static analysis. However, Simulation knows to perform a free vibration 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.
March 29, 2005
Inventory #002215
5-10

11. … 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 relative stress or strain results are needed, be sure to add results under the Frequency Finder branch, not the Solution branch.
Recall that mode shapes are relative values since no excitation is present. Hence, stresses and strains are also relative.
March 29, 2005
Inventory #002215
5-11

12. … Solution Options
The solution branch provides details on the type of analysis being performed
For a free vibration 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.”
March 29, 2005
Inventory #002215
5-12

13. … Solving the Model
After setting up the model, one can solve the free vibration analysis just like any other analysis by selecting the Solve button.
A free vibration analysis is generally more computationally expensive than a static analysis on the same model because of the equations solved.
If a “Solution Information” branch is requested under the Solution branch, detailed solution output, including the amount of memory used and solution progress, will be available in the Worksheet tab.
If stress or strain results or more frequencies/modes are requested after a solution is performed, a new solution is required.
March 29, 2005
Inventory #002215
5-13

14. … 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.
March 29, 2005
Inventory #002215
5-14

15. … 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
March 29, 2005
Inventory #002215
5-15

16. B. Workshop 5.1 – Free Vibration
Workshop 5.1 – Free Vibration Analysis
Goal:
Investigate the vibration characteristics of two motor cover designs manufactured from 18 gauge steel.
March 29, 2005
Inventory #002215
5-16

17. C. Free Vibration with Pre-Stress
In some cases, one may want to consider prestress effects when performing a free vibration 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.
March 29, 2005
Inventory #002215
5-17

18. … Free Vibration with Pre-Stress
In free vibration with pre-stress analyses, 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 free vibration with pre-stress analysis is then solved, including the [S] term
March 29, 2005
Inventory #002215
5-18

19. … Procedure w/ Pre-Stress Effects
To perform a free vibration with pre-stress analysis (a.k.a. prestressed modal 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
March 29, 2005
Inventory #002215
5-19

20. … Example w/ Pre-Stress Effects
Consider a simple comparison of a thin plate fixed at one end
Two analyses will be run – free vibration and free vibration with pre-stress effects – to compare the differences between the two.
Free Vibration
Free Vibration with Pre-Stress
March 29, 2005
Inventory #002215
5-20

21. … Example w/ Pre-Stress Effects
Notice that the only difference of running a free vibration analysis with or without pre-stress is the existence of a load
If a Frequency Finder tool is present and a load is present, 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.
March 29, 2005
Inventory #002215
5-21

22. … Example w/ Pre-Stress Effects
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 Pre-Stress
1st mode frequency: 184 Hz
March 29, 2005
Inventory #002215
5-22

23. D. Workshop 5.2 – Prestressed Modal
Workshop 5.2 – Prestressed Modal Analysis
Goal: simulate the modal response of the tension link (shown below) in both a stressed and unstressed state.
March 29, 2005
Inventory #002215
5-23