Harmonic Analysis - PowerPoint PPT Presentation

Loading...

PPT – Harmonic Analysis PowerPoint presentation | free to download - id: 79a7c0-ODJjM



Loading


The Adobe Flash plugin is needed to view this content

Get the plugin now

View by Category
About This Presentation
Title:

Harmonic Analysis

Description:

Chapter Ten Harmonic Analysis Chapter Overview In this chapter, performing harmonic analyses in Simulation will be covered: It is assumed that the user has already ... – PowerPoint PPT presentation

Number of Views:36
Avg rating:3.0/5.0
Slides: 39
Provided by: Sheld50
Learn more at: http://www-eng.lbl.gov
Category:

less

Write a Comment
User Comments (0)
Transcript and Presenter's Notes

Title: 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 as In 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
    equation 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
  • 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
    Harmonic Tool 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 and beta damping are
    input, the effects will be cumulative
  • Either damping option can be used with either
    solution method (full or mode superposition)

23
Background on Damping
  • Damping can be caused by various effects.
  • Viscous damping is 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.

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 whether average,
    minimum, or maximum value will 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 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

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)
About PowerShow.com