Welcome to this Ansys How To Series video.
Harmonic Analysis is used to determine the steady-state response of any structure
subjected to loads that vary sinusoidally with time. Different from the transient
dynamic analysis, the harmonic analysis does not solve the time-history response of the structure.
It treats the structure’s dynamic behavior in the frequency domain instead of the time domain.
Therefore, the interpretation of harmonic analysis results becomes very different
from static and transient analysis. What engineers are most interested
in harmonic analysis is the resonance, where excessive motion, stress, noise,
and vibration occur at a certain frequency. To interpret the results correctly,
one needs to have a clear understanding of the objectives,
concepts, and assumptions of harmonic analysis. In this video, we will guide you to learn
how to interpret harmonic results and why it should be done this way.
By harmonic analysis, engineers can verify if the designs can successfully overcome resonance,
fatigue, and other harmful effects of the forced vibrations.
It is widely used in the fields of Aerospace, Machinery Parts, Electronic equipment, Bridges,
and Buildings, etc. We know that it can be computationally expensive to conduct
a time-history simulation of a structure under vibrating loads.
Harmonic analysis provides an alternative way to find the
peak response of the structure efficiently. However, the tradeoff of such computational
efficiency is that there are certain assumptions and restrictions.
First, we assume that all input loads vary sinusoidally at the same frequency.
Writing the loads in sinusoidal format, the subscript ‘i’ indicates different loads.
You will notice that amplitude Fmax and phase angle Theta can
be different for different loads, while frequency Omega always remains the same.
Here is an example of two loads, F1 and F2, plotted with time.
They have the same frequency, but the different amplitude and phase angle.
Here we are looking at two oscillating loads with the same phase angle, and then two loads
with different phase angles, we call this out of phase loads.
It is obvious that the structure will respond differently in these two cases.
Although harmonic analysis is a dynamic analysis, transient effects are not calculated.
It solves for the steady-state response of the structure after
the harmonic loads have been acting on the structure for a long period of time.
In other words, the start-up, or transient vibrations that usually
occur at the beginning of excitation cannot be considered with this method.
Now let’s have a look at the equation of motion solved by the finite element solver.
This equation is general for all kinds of dynamic analysis.
For harmonic analysis, since the input loads are all sinusoidal,
we assume that the output solutions of the structure are also sinusoidal with
the same frequency of the input loads. Note that we use Phi to denote the phase angle of
the solution so that to differentiate it from the input load phase angle Theta. The different
input and output phase angles can be caused by out-of-phase loads or damping added to the system.
We call the difference between Phi and Theta as the "Phase Shift”, showing how
much the input waveform is shifted compared with the response waveform of the structure.
To summarize, the input and the output of harmonic analysis are both sinusoidal acting at the same
excitation frequency. What we are trying to calculate is the amplitude of the response
and the phase angle. One thing to mention here is, although we say the solution of
harmonic analysis is sinusoidal, it only applies for the direct results, for example,
directional displacement, normal stress and strain, and shear stress and strain.
For total deformation, and other derived results, including principal strains
and stresses, equivalent strain, and stress, this is not the case.
For example, for total deformation, which is calculated as the square root of the sum of
squares, that is SRSS of ux, uy, and uz. Although on the right side of the equation, ux, uy, and uz
are all sinusoidal, the calculated value u_total might not be sinusoidal because there may be phase
difference in the displacement components, and taking SRSS will always yield a positive value,
which can be periodic but non-sinusoidal.
Similar reasoning applies to principal stress and strain and equivalent stress and strain.
Now, let’s move to a harmonic simulation and start to evaluate its results step by step.
We have here a model of a mounting bracket designed to support two masses that impose
sinusoidally oscillating loads at different locations and out of phase by 180 degrees.
We examine the results for a frequency sweep from zero to 60 Hz.
Our objective is to predict the location, frequency and phase angle
of the maximum response and the corresponding stresses.
We do all this with a mode superposition harmonic analysis.
For this case, the general workflow for the mode-sup harmonic analysis
was already set up and the solution has been run.
What remains in this exercise is to evaluate the results.
The modal analysis extracted all the modes from zero to 90 Hz.
We can see, by inspection of the completed modal results,
that the first two modes fall inside the range of frequencies under consideration.
The first mode is of particular interest as its mode shape is deflecting in the same direction
as the applied forces in plus and minus Y direction.
Under the Harmonic System, the two forces were strategically applied in Y direction
and out of phase with each other by 180 degrees. Under Analysis Settings, we have defined the
frequency sweep from zero to 60 Hz. Solution Intervals is set to 60,
which means a results set will be calculated at each Hz from zero to 60.
A damping ratio for the system is defined as 0.02.
It is important to understand that with a completed harmonic solution, we have result
sets over many frequencies and results at each frequency can change with respect to phase angle.
In reviewing harmonic results, then the first order of business is to ascertain
where in the structure is the largest response occurring and at what frequency and phase angle.
From there we can examine local results in more detail such as displacement,
stress and strain depending on the acceptance criteria we are trying to satisfy.
For this example, we begin by inserting a Frequency Response Plot,
also known as a Bode Plot, to ascertain the displacement, corresponding frequency,
and phase angle at the location of interest. This is usually the location of peak response.
Since in this application, the displacement in vertical Y direction is of greatest interest,
we scope deformation in vertical direction on entire geometry.
Notice how the peak displacement occurs at the first natural frequency of 37 Hz.
With Spatial Resolution set to 'Use Average',
this can sometimes give a low number whereas 'Use Maximum' might be more representative.
It is always best to review both average and maximum.
The ‘Use Minimum’ and ‘Use Maximum’ settings of the Spatial Resolution option are based on the
amplitude and thus are reported from the location with either the largest or the smallest value.
The ‘Use Average’ setting calculates the average from all the available components.
Next insert a Phase Response for same Y displacement component.
Define the frequency as 37 Hz.
From this graph, we can see that the maximum Y displacement will occur at 79.2 degrees.
We next want to determine where on the physical structure the peak response is occurring.
We can do this by simply right mouse button and insert displacement in Y direction.
Define frequency of 37 Hz and Sweep Phase of 79.2 degrees.
Notice how this corresponds closely with the first mode shape and corresponding
first natural frequency from the modal analysis. Also, the maximum value reported in this plot
corresponds to the peak value on the amplitude vs frequency plot.
We can obtain similar results for velocity and acceleration peak results.
Note that these results are 90 degrees out of phase with each other.
This makes sense given that these results are derived from first and second derivatives
of the displacement result which is a sinusoidal expression of phase angle.
By careful examination of the components of stress vs phase angle,
we can see that the Sz component of stress dominates all the others.
We can also see that it is maximum at 79.2 degrees phase angle.
Once we have established the frequency and phase angle of greatest interest,
we can focus our attention on critical derived quantities like, equivalent stress.
Insert a plot of maximum equivalent stress and set “By” to “Max Over Frequency”
and the sweeping phase angle to 79.2 degrees. We could arrive at the same result if we plotted
S-equivalent by “Maximum Over Phase” and set the frequency to 37 Hz.
This location represents the point of maximum bending.
Having created a named selection for this location of interest, it is possible to export this data
to a separate excel spreadsheet for further post processing.
Notice how, in this case, bending stress in Z direction dominates the overall stress state.
Notice also, that although each stress component has a sinusoidal characteristics,
derived quantities like equivalent stress are periodic, but not sinusoidal.
From this point, depending on the design objectives, these results can be compared
with critical design allowables to assess the integrity of the design.
To briefly summarize, harmonic analysis is a frequency-based analysis.
The input and the output of harmonic analysis are both sinusoidal
acting at the same excitation frequency.
What to be calculated is the amplitude of the response and the phase angle.
Because it’s a frequency-based analysis, the interpretation of results
takes a different route from what we do for static and time-history dynamic analysis.
By this video, we hope to help you build a general workflow for evaluating harmonic results.
Usually, we should look for frequency response first to find frequency and
phase angle where peak response occurs, then check the contour plots of interest.
We also need to pay special attention to the various options in the settings of
results, for example, the “Use Average”, “Use Minimum” and “Use Maximum” options
for extracting frequency response, to avoid misunderstanding of the results.
In general, we often need to evaluate multiple result items
to have a complete understanding of harmonic response of a structure. If you find this video
helpful, please like, comment, and subscribe. To find more information about harmonic analysis or
other topics, check our channel for more how to videos and visit ansys.com/courses today!