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.
• 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 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
  equationAssumptions
• 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
• 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)
• Set Environment to Harmonic and apply 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
• 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
• Loads Not Supported
• Thermal loads
• Rotational Velocity
• Remote Force Load
• Pretension Bolt Load
• Compression Only Support (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
• Note 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 specify harmonic loads
• Flag the Environment as Harmonic
• Enter the magnitude (vector or component method)
• Enter an appropriate phase angle
• 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 (magnitude and phase angle) for two
  cycles may be visualized by selecting the load,
  then clicking on the Worksheet tab

15
B. Solving Harmonic Analyses

• Harmonic Setup
• Select the Solution branch and insert a
  HarmonicTool from the Context toolbar
• In the Details view 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 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
• 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
• Solution Method can be chosen in the Details
  view of the Harmonic Tool
• The Details view of the Solution branch has no
  effect on the analysis.

17
Mode Superposition Method

• The Mode Superposition method solves the harmonic
  equation in modal coordinates
• 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.
• As more modes n are included, the approximation
  for x becomes more accurate.

18
Mode Superposition Method

• Points to remember
• 1. 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
• The harmonic analysis portion is very quick and
  efficient, hence, the Mode Superposition method
  is usually much faster overall than the Full
  method
• Since a free vibration analysis is performed,
  Simulation knows what the natural frequencies of
  the structure are and can cluster the harmonic
  results near them (see next slide)

19
Mode Superposition Method

• Cluster example

20
Full Method

• The Full method is an alternate way of solving
  harmonic analyses
• 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

21
Full Method

• Points to remember
• 1. For each frequency, the Full method must
  factorize Kc.
• Because of this, the Full method tends to be more
  computationally expensive than the Mode
  Superposition method
• Given Displacement Support type is available
• The Full method does not calculate modes so no
  clustering of results is possible. Only
  evenly-spaced intervals is permitted.

22
C. Damping Input

• The harmonic equation has a damping matrix C
• For ANSYS Professional license only a constant
  damping ratio x is available
• For ANSYS Structural licenses and above, either a
  constant damping ratio x or beta damping value
  can be input
• If both constant damping andbeta damping are
  input, the effects willbe cumulative
• Either damping option can be used witheither
  solution method (full or modesuperposition)

23
Background on Damping

• Damping can be caused by various effects.
• Viscous damping is 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.

24
Constant Damping Ratio

• The constant damping ratio provides a value of x
  which is 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 and will be converted internally to
  an appropriate value for C

25
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 to the damping ratio x
• Beta damping increases with increasing frequency
  which tends to damp out the effect of higher
  frequencies
• Beta damping is in units of time

26
Beta Damping

• Beta damping can be input in two ways
• The damping value can be directly input
• A damping ratio and frequency can be input and
  the corresponding beta damping value will be
  calculated

27
Damping Relationships

• Common measures for damping
• 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

28
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 at a specified
  frequency and phase angle
• Frequency response plots of minimum, maximum, or
  average components of stresses, strains,
  displacements, or acceleration
• Phase response plots of minimum, maximum, or
  average components of stresses, strains, or
  displacements at a specified frequency
• Results must be requested before solving
• If other results are requested after a solution
  is completed another solution must be re-run

29
Request Harmonic Tool Results

• Result notes
• Scope results on entities of interest
• For edges and surfaces, specify whetheraverage,
  minimum, or maximum valuewill be reported
• 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.

30
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

31
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

32
Contour Results

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

33
Contour Animations

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

34
Frequency Response Plots

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

35
Phase Response Plots

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

36
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
• 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.

37
E. Workshop 10 Harmonic Analysis

• 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.

38
(No Transcript)