Harmonic Analysis

1
Harmonic Analysis

• Chapter Ten

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

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

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.

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 asIn this way, a real component
  F1 and an imaginary component F2 are used.
• The response x is analogous to F

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
  equationThis 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.

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

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

9
Material Properties

• In a harmonic analysis, Youngs Modulus,
  Poissons 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

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

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

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.

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

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

15
B. Solving Harmonic Analyses

• Prior to solving, request the Harmonic Tool
• Select the Solution branch and insert a
  HarmonicTool from the Context toolbar
• In the Details view of the Harmonic Tool, onecan
  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 WDW.

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.
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 branchshould
  not be used, as it has no effecton the analysis.

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.

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.

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.

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

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

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.

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.

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 andbeta
  damping are input, the effects willbe cumulative
• Either damping option can be used witheither
  solution method (full or modesuperposition)

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 velocitywhere 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.

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

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
  xOne 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

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

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 structures
  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

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.

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 whetheraverage,
  minimum, or maximum valuewill 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.

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.

33
Solving the Model

• The Details view of the Solution branch is not
  used in a Harmonic analysis.
• Only informative status of the type ofanalysis
  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

34
Contour Results

• Contour results of components of stress, strain,
  or displacement are available at a given
  frequency and phase angle

35
Contour Animations

• These results can be animated. Animations will
  use the actual harmonic response (real and
  imaginary results)

36
Frequency Response Plots

• XY Plots of components of stress, strain,
  displacement, or acceleration can be requested

37
Phase Response Plots

• Comparison of phase of components of stress,
  strain, or displacement with input forces can be
  plotted at a given frequency

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.

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.

40
(No Transcript)