Harmonic-2

1. Structural Harmonic Analysis

2. 7/22/2019 2
Introduction
• Harmonic response analysis is a technique used to determine the steady-state response
of a linear structure to loads that vary sinusoidal (harmonically) with time
• Any sustained cyclic load will produce a sustained cyclic response (a harmonic response)
in a structural system.
• Harmonic response analysis gives you the ability to predict the sustained dynamic
behaviour of your structures, thus enabling you to verify whether or not your designs will
successfully overcome resonance, fatigue, and other harmful effects of forced vibrations.

3. 7/22/2019 3
Harmonic Analysis Outcomes
• The idea is to calculate the structure's response at several frequencies and obtain a graph
of some response quantity (usually displacements) versus frequency.
• "Peak" responses are then identified on the graph and stresses reviewed at those peak
frequencies.
• This analysis technique calculates only the steady-state, forced vibrations of a structure.

4. 7/22/2019 4
• To completely specify a harmonic load, three pieces of information are usually required:
the amplitude, the phase angle, and the forcing frequency range
• The amplitude is the maximum value of the load, which you specify using the commands
• The phase angle is a measure of the time by which the load lags (or leads) a frame of
reference it is the angle measured from the real axis.
• The phase angle is required only if you have multiple loads that are out of phase with
each other
• Note: A harmonic analysis cannot calculate the response to multiple forcing functions
acting simultaneously with different frequencies (for example, two machines with
different rotating speeds running at the same time).
…General Terminology

5. 7/22/2019 5
General equation of motion:
Assume free vibrations and ignore damping:
Assume harmonic motion ( i.e.., The roots of this equation are i2, the eigenvalues, where
i ranges from 1 to number of DOF. Corresponding vectors are {x}i, the eigenvectors.
       02
 uMK 
       0 uKuM 
Governing Equation
)sin( tUu 
[M] = mass matrix;
[C] = damping matrix;
[K] = stiffness matrix;
{Ẍ} = nodal acceleration vector;
{Ẋ}= nodal velocity vector;
{X} = nodal displacement vector;
{F(t)} = load vector
[M]{Ẍ} + [C]{Ẋ} + [K]{X} = F(t)

6. 7/22/2019 6
Different forms of Governing Equation
1. [M]{Ẍ} + [C]{Ẋ} + [K]{X} = F(t)
Basic equation of motion
2. [M]{Ẍ} + [K]{X} = F(t)
Basic equation of motion without damping
3. [M]{Ẍ} + [K]{X} = 0
Basic equation of motion without damping and
initial conditions are zero

7. 7/22/2019 7
Solve the Equation of Motion
• Note that all vibrations problems have
similar equations of motion. Consequently,
we can just solve the equation once, record
the solution, and use it to solve any vibration
problem we might be interested in. The
procedure to solve any vibration problem is:
1. Derive the equation of motion, using
Newton’s laws (or sometimes you can use
energy methods)
2. Do some algebra to arrange the equation of
motion into a standard form
3. Look up the solution to this standard form
in a table of solutions to vibration
problems.

8. 7/22/2019 8
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
Geometry
Material
properties
Contacts
Meshing
Harmonic settings,
loads & supports
Solve the
model

9. 7/22/2019 9
… 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
Rotor-Shaft-Fan assembly of an EV-MOTOR

10. 7/22/2019 1010
… 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
• Damping is not specified as a
material property but as a global
property
Double click on
engineering materials to
define material & their
properties

11. 7/22/2019 11
… 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
type
• The contact behavior is similar to free vibration
analyses, 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 Friction
Bonded
No Separation
Rough
Frictionless
Types of Connections available and they are used as per the requirements

12. 7/22/2019 12
Analysis settings
In the harmonic analysis setting we define ,
• Frequency range (minimum & maximum )
• Solution intervals
• Mode superposition
• Modal frequency range( if required)
• Boundary conditions depending on the requirement
• Loads are applied sinusoidally in the tabular format at
one frequency only

13. 7/22/2019 13
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.
n
ff minmax
2

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 10000 Hz.

14. 7/22/2019 14
… 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.

15. 7/22/2019 15
… 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.
2. 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.

16. 7/22/2019 16
… Mode Superposition Method
3. Due to the nature of the Mode
Superposition method, Given
Displacement Supports are not
allowed
Non zero prescribed
displacements are not possible
because the solution is done
with modal coordinates
This was mentioned earlier
during the discussion on loads
and supports
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.

17. 7/22/2019 17
…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)

18. 7/22/2019 18
…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.
xcFdamp

crc
c
x
• 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 unit less
• In the Full method, the damping ratio x
is not directly used. This will be
converted internally to an appropriate
value for [C]

19. 7/22/2019 19
… 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
kc b
222
2 i
i
iicr
i
m
k
c
c b


b

b
x 
• 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
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.

20. 7/22/2019 20
… 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
sinusoidal at the same excitation frequency
A list of supported loads are shown below:
• 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°.
Type of Load Phase Input Solution Method
Acceleration Load No Full or Mode Superposition
Standard Earth Gravity Load No Full or Mode Superposition
Pressure Load No Full or Mode Superposition
Force Load No Full or Mode Superposition
Bearing Load No Full or Mode Superposition
Moment Load No Full or Mode Superposition
Given Displacement Support No Full Only

21. 7/22/2019 21
… 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

22. 7/22/2019 22
…Request Harmonic Tool Results
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.
• 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.

23. 7/22/2019 23
… 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.
The graphs the peaks correspond to the resonance conditions. The operating frequencies must be
well below the resonance conditions, hence resonance conditions can be easily avoided.

24. 7/22/2019 24
… Harmonic Tool Results
• 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.
Left-click on the graphics window to change the Graph Properties
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.
Amplitude Vs Frequency plots Amplitude Vs Frequency plots
Comparison of phase of components of stress, strain,
or displacement with input forces can be plotted at a
given frequency

25. 7/22/2019 25
…Other Solution
• 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.

26. Thank You
7/22/2019 26