Loading...

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

The Adobe Flash plugin is needed to view this content

Harmonic Analysis

- Chapter Ten

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

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

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.

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.

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.

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

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

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

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

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

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.

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

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

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.

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.

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.

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)

Mode Superposition Method

- Cluster example

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

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.

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)

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.

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

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

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

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

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

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.

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

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

Contour Results

- Contour results of components of stress, strain,

or displacement are available at a given

frequency and phase angle

Contour Animations

- These results can be animated. Animations will

use the actual harmonic response (real and

imaginary results)

Frequency Response Plots

- XY Plots of components of stress, strain,

displacement, or acceleration can be requested

Phase Response Plots

- Comparison of phase of components of stress,

strain, or displacement with input forces can be

plotted at a given frequency

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.

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.

(No Transcript)