AWS90_Ch10_Harmonic.ppt

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-2
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

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-3
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:
          
F
x
K
x
C
x
M 

 



ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-4
• 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.
   
    t
j
j
t
j
j
e
e
x
x
e
e
F
F
W
W


f
y
max
max

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-5
• 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}
-1
-0.75
-0.5
-0.25
0
0.25
0.5
0.75
1
0 45 90 135 180 225 270 315 360 405 450 495 540 585 630 675 720
Angle (Degrees)
Force
Value
Force 1
Force 2
Model shown is from a sample SolidWorks assembly.
   
 
  t
j
t
j
t
j
j
e
jF
F
e
jF
F
e
e
F
F
W
W
W





2
1
max
max
max
sin
cos y
y
y

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-6
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.
     
    
2
1
2
1
2
jF
F
jx
x
K
C
j
M 



W

W


ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-7
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

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-8
… 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
ANSYS License Availability
DesignSpace Entra
DesignSpace
Professional x
Structural x
Mechanical/Multiphysics x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-9
… 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
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-10
… 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
DesignSpace Entra
DesignSpace
Professional x
Structural x
Initially Touching Inside Pinball Region Outside Pinball Region
Bonded Bonded Bonded Bonded Free
No Separation No Separation No Separation No Separation Free
Rough Rough Bonded Free Free
Frictionless Frictionless No Separation Free Free
Contact Type Static Analysis
Harmonic Analysis

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
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
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-12
• 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°.
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 Yes Full or Mode Superposition
Force Load Yes Full or Mode Superposition
Bearing Load No Full or Mode Superposition
Moment Load No Full or Mode Superposition
Given Displacement Support Yes Full Only
DesignSpace Entra
DesignSpace
Professional /
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-13
• 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:
DesignSpace Entra
DesignSpace
Professional x
Structural x












1
2
1
2
2
2
1
tan
F
F
F
F
magnitude
y

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-14
• 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
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-15
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.
n
f
f min
max
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.
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-16
… 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.
DesignSpace Entra
DesignSpace
Professional /
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-17
… 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.
DesignSpace Entra
DesignSpace
Professional x
Structural x
     
    
2
1
2
1
2
jF
F
jx
x
K
C
j
M 



W

W

   



n
i
i
i
y
x
1
f

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-18
• 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.
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-19
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.
DesignSpace Entra
DesignSpace
Professional x
Structural x
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.

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-20
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
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-21
… 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:
     
    
2
1
2
1
2
jF
F
jx
x
K
C
j
M 



W

W

DesignSpace Entra
DesignSpace
Professional
Structural x
       
 
   
   
    
C
C
C
C
C
C
F
x
K
jF
F
F
jx
x
x
K
C
j
M
K






W

W


2
1
2
1
2

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-22
… 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.
DesignSpace Entra
DesignSpace
Professional
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-23
… 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.
DesignSpace Entra
DesignSpace
Professional
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-24
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)
DesignSpace Entra
DesignSpace
Professional /
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-25
… 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.
x
c
Fdamp


cr
c
c

x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-26
… 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]
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-27
… 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
DesignSpace Entra
DesignSpace
Professional
Structural x
k
c b

2
2
2
2 i
i
i
i
cr
i
m
k
c
c bw
w
w
b
w
b
x 




ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-28
… 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
DesignSpace Entra
DesignSpace
Professional
Structural x
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.

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-29
… 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 2xi
– 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

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-30
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.
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-31
… 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.
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-32
… 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.
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-33
… 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
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-34
… Contour Results
• Contour results of components of stress, strain, or
displacement are available at a given frequency and phase
angle
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-35
… Contour Animations
• These results can be animated. Animations will use the
actual harmonic response (real and imaginary results)
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-36
… Frequency Response Plots
• XY Plots of components of stress, strain, displacement, or
acceleration can be requested
DesignSpace Entra
DesignSpace
Professional x
Structural x
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

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-37
… Phase Response Plots
• Comparison of phase of components of stress, strain, or
displacement with input forces can be plotted at a given
frequency
DesignSpace Entra
DesignSpace
Professional x
Structural x
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

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-38
… 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.
DesignSpace Entra
DesignSpace
Professional x
Structural x

ANSYS
Workbench
–
Simulation
Training Manual
Harmonic Analysis
March 29, 2005
Inventory #002215
10-39
• 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.
E. Workshop 10

AWS90_Ch10_Harmonic.ppt

Recommended

Recommended

More Related Content

Similar to AWS90_Ch10_Harmonic.ppt

Similar to AWS90_Ch10_Harmonic.ppt (20)

Recently uploaded

Recently uploaded (20)

AWS90_Ch10_Harmonic.ppt