1. Chapter Ten
Harmonic Analysis

2. Chapter Overview
In this chapter, performing harmonic analyses in Simulation will be covered:
It is assumed that the user has already covered Chapter 4 Linear Static Structural Analysis and Chapter 5 Free Vibration Analysis prior to this chapter.
The following will be covered in this chapter:
Setting Up Harmonic Analyses
Harmonic Solution Methods
Damping
Reviewing Results
The capabilities described in this section are generally applicable to ANSYS Professional licenses and above.
Exceptions will be noted accordingly
March 29, 2005
Inventory #002215
10-2

3. Background on Harmonic Analysis
A harmonic analysis is used to determine the response of the structure under a steady-state sinusoidal (harmonic) loading at a given frequency.
A harmonic, or frequency-response, analysis considers loading at one frequency only. Loads may be out-of-phase with one another, but the excitation is at a known frequency. This procedure is not used for an arbitrary transient load.
One should always run a free vibration analysis (Ch. 5) prior to a harmonic analysis to obtain an understanding of the dynamic characteristics of the model.
To better understand a harmonic analysis, the general equation of motion is provided first:
March 29, 2005
Inventory #002215
10-3

4. Background on Harmonic Analysis
In a harmonic analysis, the loading and response of the structure is assumed to be harmonic (cyclic):
The use of complex notation is an efficient representation of the response. Since ejA is simply (cos(A)+jsin(A)), this represents sinusoidal motion with a phase shift, which is present because of the imaginary (j=-1) term.
The excitation frequency W is the frequency at which the loading occurs. A force phase shift y may be present if different loads are excited at different phases, and a displacement phase shift f may exist if damping or a force phase shift is present.
March 29, 2005
Inventory #002215
10-4

5. Background on Harmonic Analysis
For example, consider the case on right where two forces are acting on the structure
Both forces are excited at the same frequency W, but “Force 2” lags “Force 1” by 45 degrees. This is a force phase shift y of 45 degrees.
The way in which this is represented is via complex notation. This, however, can be rewritten as: In this way, a real component F1 and an imaginary component F2 are used.
The response {x} is analogous to {F}
March 29, 2005
Inventory #002215
10-5
Model shown is from a sample SolidWorks assembly.

6. Basics of Harmonic Analysis
For a harmonic analysis, the complex response {x1} and {x2} are solved for from the matrix equation: This results in the following assumptions:
[M], [C], and [K] are constant:
Linear elastic material behavior is assumed
Small deflection theory is used, and no nonlinearities included
Damping [C] should be included. Otherwise, if the excitation frequency W is the same as the natural frequency w of the structure, the response is infinite at resonance.
The loading {F} (and response {x}) is sinusoidal at a given frequency W, although a phase shift may be present
It is important to remember these assumptions related to performing harmonic analyses in Simulation.
March 29, 2005
Inventory #002215
10-6

7. A. Harmonic Analysis Procedure
The harmonic 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 harmonic analyses.
Attach Geometry
Assign Material Properties
Define Contact Regions (if applicable)
Define Mesh Controls (optional)
Include Loads and Supports
Request Harmonic Tool Results
Set Harmonic Analysis Options
Solve the Model
Review Results
March 29, 2005
Inventory #002215
10-7

8. … Geometry Any type of geometry may be present in a harmonic analysis
Solid bodies, surface bodies, line bodies, and any combination thereof may be used
Recall that, for line bodies, stresses and strains are not available as output
A Point Mass may be present, although only acceleration loads affect a Point Mass
March 29, 2005
Inventory #002215
10-8

9. … Material Properties
In a harmonic analysis, Young’s Modulus, Poisson’s Ratio, and Mass Density are required input
All other material properties can be specified but are not used in a harmonic analysis
As will be shown later, damping is not specified as a material property but as a global property
March 29, 2005
Inventory #002215
10-9

10. … 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:
The contact behavior is similar to free vibration analyses (Ch. 5), where nonlinear contact behavior will reduce to its linear counterparts since harmonic simulations are linear.
It is generally recommended, however, not to use a nonlinear contact type in a harmonic analysis
March 29, 2005
Inventory #002215
10-10

11. … Loads and Supports
Structural loads and supports may also be used in harmonic analyses with the following exceptions:
Thermal loads are not supported
Rotational Velocity is not supported
The Remote Force Load is not supported
The Pretension Bolt Load is nonlinear and cannot be used
The Compression Only Support is nonlinear and should not be used. If present, it behaves similar to a Frictionless Support
Remember that all structural loads will vary sinusoidally at the same excitation frequency
March 29, 2005
Inventory #002215
10-11

12. … Loads and Supports A list of supported loads are shown below:
The “Solution Method” will be discussed in the next section.
It is useful to note at this point that ANSYS Professional does not support “Full” solution method, so it does not support a Given Displacement Support in a harmonic analysis.
Not all available loads support phase input. Accelerations, Bearing Load, and Moment Load will have a phase angle of 0°.
If other loads are present, shift the phase angle of other loads, such that the Acceleration, Bearing, and Moment Loads will remain at a phase angle of 0°.
March 29, 2005
Inventory #002215
10-12

13. … Loads and Supports To add a harmonic load:
Add any of the supported loads as usual.
Under “Time Type,” change it from “Static” to “Harmonic”
Enter the magnitude (or components, if available)
Phase input, if available, can be input
If only real F1 and imaginary F2 components of the load are known, the magnitude and phase y can be calculated as follows:
March 29, 2005
Inventory #002215
10-13

14. … Loads and Supports
The loading for two cycles may be visualized by selecting the load, then clicking on the “Worksheet” tab
The magnitude and phase angle will be accounted for in this visual representation of the loading
March 29, 2005
Inventory #002215
10-14

15. B. Solving Harmonic Analyses
Prior to solving, request the Harmonic Tool:
Select the Solution branch and insert a Harmonic Tool from the Context toolbar
In the Details view of the Harmonic Tool, one can enter the Minimum and Maximum excitation frequency range and Solution Intervals
The frequency range fmax-fmin and number of intervals n determine the freq interval DW
Simulation will solve n frequencies, starting from W+DW.
In the example above, with a frequency range of 0 – 10,000 Hz at 10 intervals, this means that Simulation will solve for 10 excitation frequencies of 1000, 2000, 3000, 4000, 5000, 6000, 7000, 8000, 9000, and Hz.
March 29, 2005
Inventory #002215
10-15

16. … Solution Methods
There are two solution methods available in ANSYS Structural and above. Both methods have their advantages and shortcomings, so these will be discussed next:
The Mode Superposition method is the default solution option and is available for ANSYS Professional and above
The Full method is available for ANSYS Structural and above
Under the Details view of the Harmonic Tool, the “Solution Method” can be toggled between the two options (if available).
The Details view of the Solution branch should not be used, as it has no effect on the analysis.
March 29, 2005
Inventory #002215
10-16

17. … Mode Superposition Method
The Mode Superposition method solves the harmonic equation in modal coordinates
Recall that the equation for harmonic analysis is as follows:
For linear systems, one can express the displacements x as a linear combination of mode shapes fi : where yi are modal coordinates (coefficient) for this relation.
For example, one can perform a modal analysis to determine the natural frequencies wi and corresponding mode shapes fi.
One can see that as more modes n are included, the approximation for {x} becomes more accurate.
March 29, 2005
Inventory #002215
10-17

18. … Mode Superposition Method
The preceding discussion is meant to provide background information about the Mode Superposition method. From this, there are three important points to remember:
1. Because of the fact that modal coordinates are used, a harmonic solution using the Mode Superposition method will automatically perform a modal analysis first
Simulation will automatically determine the number of modes n necessary for an accurate solution
Although a free vibration analysis is performed first, the harmonic analysis portion is very quick and efficient. Hence, the Mode Superposition method is usually much faster overall than the Full method.
March 29, 2005
Inventory #002215
10-18

19. … Mode Superposition Method
Since a free vibration analysis is performed, Simulation will know what the natural frequencies of the structure are
In a harmonic analysis, the peak response will correspond with the natural frequencies of the structure. Since the natural frequencies are known, Simulation can cluster the results near the natural frequencies instead of using evenly spaced results.
In this example, the cluster option captures the peak response better than evenly-spaced intervals (4.51e-3 vs. 4.30e-3)
The Cluster Number determines how many results on either side of a natural frequency is solved.
March 29, 2005
Inventory #002215
10-19

20. … Mode Superposition Method
3. Due to the nature of the Mode Superposition method, Given Displacement Supports are not allowed
Nonzero prescribed displacements are not possible because the solution is done with modal coordinates
This was mentioned earlier during the discussion on loads and supports
March 29, 2005
Inventory #002215
10-20

21. … Full Method
The Full method is an alternate way of solving harmonic analyses
Recall the harmonic analysis equation:
In the Full method, this matrix equation is solved for directly in nodal coordinates, analogous to a linear static analysis except that complex numbers are used:
March 29, 2005
Inventory #002215
10-21

22. … Full Method
This results in several differences compared with the Mode Superposition method:
1. For each frequency, the Full method must factorize [Kc].
In the Mode Superposition method, a simpler set of uncoupled equations is solved for. In the Full method, a more complex, coupled matrix [KC] must be factorized.
Because of this, the Full method tends to be more computationally expensive than the Mode Superposition method
2. Given Displacement Support is available
Because {x} is solved for directly, imposed displacements are permitted. This allows for the use of Given Displacement Supports.
March 29, 2005
Inventory #002215
10-22

23. … Full Method 3. The Full method does not use modal information
Unlike the Mode Superposition method, the Full method does not rely on mode shapes and natural frequencies
No free vibration analysis is internally performed
The solution of {xC} is exact
No approximation of the response {x} to mode shapes is used
However, because modal information is not present to Simulation during a solution, no clustering of results is possible. Only evenly-spaced intervals is permitted.
March 29, 2005
Inventory #002215
10-23

24. C. Damping Input The harmonic equation has a damping matrix [C]
It was noted earlier that damping is specified as a global property
For ANSYS Professional license, only a constant damping ratio x is available for input
For ANSYS Structural licenses and above, either a constant damping ratio x or beta damping value can be input
Note that if both constant damping and beta damping are input, the effects will be cumulative
Either damping option can be used with either solution method (full or mode superposition)
March 29, 2005
Inventory #002215
10-24

25. … Background on Damping
Damping results in energy loss in a dynamic system.
The effect damping has on the response is to shift the natural frequencies and to lower the peak response
Damping is present in many forms in any structural system
Damping is a complex phenomena due to various effects. The mathematical representation of damping, however, is quite simple. Viscous damping will be considered here:
The viscous damping force Fdamp is proportional to velocity where c is the damping constant
There is a value of c called critical damping ccr where no oscillations will take place
The damping ratio x is the ratio of actual damping c over critical damping ccr.
March 29, 2005
Inventory #002215
10-25

26. … Constant Damping Ratio
The constant damping ratio input in Simulation means that the value of x will be constant over the entire frequency range.
The value of x will be used directly in Mode Superposition method
The constant damping ratio x is unitless
In the Full method, the damping ratio x is not directly used. This will be converted internally to an appropriate value for [C]
March 29, 2005
Inventory #002215
10-26

27. … Beta Damping
Another way to model damping is to assume that damping value c is proportional to the stiffness k by a constant b:
This is related back to the damping ratio x: One can see from this equation that, with beta damping, the effect of damping increases linearly with frequency
Unlike the constant damping ratio, beta damping increases with increasing frequency
Beta damping tends to damp out the effect of higher frequencies
Beta damping is in units of time
March 29, 2005
Inventory #002215
10-27

28. … Beta Damping There are two methods of input of beta damping:
Beta damping value can be directly input
A damping ratio and frequency can be input, and the corresponding beta damping value will be calculated by Simulation, per the equation on the previous slide
Although a frequency and damping ratio is input in this second case, remember that beta damping will linearly increase with frequency. This means that lower frequencies will have less damping and higher frequencies will experience more damping.
March 29, 2005
Inventory #002215
10-28

29. … Damping Relationships
There are some other measures of damping commonly used. Note that these are usually for single degree of freedom systems, so extrapolating it for use in multi-DOF systems (such as FEA) should be done with caution!
The quality factor Qi is 1/(2xi)
The loss factor hi is the inverse of Q or 2xi
The logarithmic decrement di can be approximated for light damping cases as 2pxi
The half-power bandwidth Dwi can be approximated for lightly damped structures as 2wixi
Remember that these measures of damping are simplified and for single DOF systems.
If the user understands the physical structure’s response over a frequency range as well as the difference between constant damping ratio and beta damping, then damping can be modeled appropriately in Simulation
March 29, 2005
Inventory #002215
10-29

30. D. Request Harmonic Tool Results
Results can then be requested from Harmonic Tool branch:
Three types of results are available:
Contour results of components of stresses, strains, or displacements for surfaces, parts, and/or assemblies at a specified frequency and phase angle
Frequency response plots of minimum, maximum, or average components of stresses, strains, displacements, or acceleration at selected vertices, edges, or surfaces.
Phase response plots of minimum, maximum, or average components of stresses, strains, or displacements at a specified frequency
Unlike a linear static analysis, results must be requested before initiating a solution. Otherwise, if other results are requested after a solution is completed, another solution must be re-run.
March 29, 2005
Inventory #002215
10-30

31. … Request Harmonic Tool Results
Request any of the available results under the Harmonic Tool branch
Be sure to scope results on entities of interest
For edges and surfaces, specify whether average, minimum, or maximum value will be reported
Enter any other applicable input
If results are requested between solved-for frequency ranges, linear interpolation will be used to calculate the response
For example, if Simulation solves frequencies from 100 to 1000 Hz at 100 Hz intervals, and the user requests a result for 333 Hz, this will be linearly interpolated from results at 300 and 400 Hz.
March 29, 2005
Inventory #002215
10-31

32. … Request Harmonic Tool Results
Simulation assumes that the response is harmonic (sinusoidal).
Derived quantities such as equivalent/principal stresses or total deformation may not be harmonic if the components are not in-phase, so these results are not available.
No Convergence is available on Harmonic results
Perform a modal analysis and perform convergence on mode shapes which will reflect response. This will help to ensure that the mesh is fine enough to capture the dynamic response in a subsequent harmonic analysis.
March 29, 2005
Inventory #002215
10-32

33. … Solving the Model
The Details view of the Solution branch is not used in a Harmonic analysis.
Only informative status of the type of analysis to be solved will be displayed
After Harmonic Analysis options have been set and results have been requested, the solution can be solved as usual with the Solve button
March 29, 2005
Inventory #002215
10-33

34. … Contour Results
Contour results of components of stress, strain, or displacement are available at a given frequency and phase angle
March 29, 2005
Inventory #002215
10-34

35. … Contour Animations
These results can be animated. Animations will use the actual harmonic response (real and imaginary results)
March 29, 2005
Inventory #002215
10-35

36. … Frequency Response Plots
XY Plots of components of stress, strain, displacement, or acceleration can be requested
For scoped results, average, minimum, or maximum values can be requested.
Bode plots (shown on right) is the default display method. However, real and imaginary results can also be plotted.
The Ctrl-left mouse button allows the user to query results on the graph.
Results can also be exported to Excel by right-clicking on the branch
Left-click on the graphics window to change the Graph Properties
March 29, 2005
Inventory #002215
10-36

37. … Phase Response Plots
Comparison of phase of components of stress, strain, or displacement with input forces can be plotted at a given frequency
The average, minimum, or maximum value of the scoped results can be used to track the phase relationship with all of the input forces.
In this example, the response is lagging the input forces, as expected, and the user can visually examine this phase difference.
Left-click on the graphics window to change the Graph Properties
March 29, 2005
Inventory #002215
10-37

38. … Requesting Results
A harmonic solution usually requires multiple solutions:
A free vibration analysis using the Frequency Finder should always be performed first to determine the natural frequencies and mode shapes
Although a free vibration analysis is internally performed with the Mode Superposition method, the mode shapes are not available to the user to review. Hence, a separate Environment branch must be inserted or duplicated to add the Frequency Finder tool.
Oftentimes, two harmonic solutions may need to be run:
A harmonic sweep of the frequency range can be performed initially, where displacements, stresses, etc. can be requested. This allows the user to see the results over the entire frequency range of interest.
After the frequencies and phases at which the peak response(s) occur are determined, contour results can be requested to see the overall response of the structure at these frequencies.
March 29, 2005
Inventory #002215
10-38

39. E. Workshop 10 Workshop 10 – Harmonic Analysis Goal:
Explore the harmonic response of the machine frame (Frame.x_t) shown here. The frequency response as well as stress and deformation at a specific frequency will be determined.
March 29, 2005
Inventory #002215
10-39