Vibration Analysis

1
Vibration Analysis

• Chapter Five

2
Chapter Overview

• In this chapter, performing free vibration
  analyses in Simulation will be covered. In
  Simulation, performing a free vibration analysis
  is similar to a linear static analysis.
• It is assumed that the user has already covered
  Chapter 4 Linear Static Structural Analysis prior
  to this section.
• The following will be covered
• Free Vibration Analysis Procedure
• Free Vibration with Pre-Stress Analysis Procedure
• The capabilities described in this section are
  generally applicable to ANSYS DesignSpace Entra
  licenses and above.

3
Basics of Free Vibration Analysis

• For a free vibration analysis, the natural
  circular frequencies wi and mode shapes fi are
  calculated fromAssumptions
• K and M are constant
• Linear elastic material behavior is assumed
• Small deflection theory is used, and no
  nonlinearities included
• C is not present, so damping is not included
• F is not present, so no excitation of the
  structure is assumed
• The structure can be constrained or unconstrained
• Mode shapes f are relative values, not absolute

4
A. Free Vibration Analysis Procedure

• The free vibration 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 free
  vibration analyses.
• Attach Geometry
• Assign Material Properties
• Define Contact Regions (if applicable)
• Define Mesh Controls (optional)
• Include Supports (if applicable)
• Request Frequency Finder Results
• Set Frequency Finder Options
• Solve the Model
• Review Results

5
Geometry and Point Mass

• Similar to linear static analyses, any type of
  geometry supported by Simulation may be used
• Solid bodies, surface bodies and line bodies
• For line bodies, only mode shapes and
  displacement results are available.
• The Point Mass feature can be used
• The Point Mass adds mass only in a free vibration
  analysis. The effect is to add only mass (not
  stiffness) to a structure.
• Because of this, the Point Mass will decrease the
  natural frequency in free vibration analyses.

6
Material Properties

• For material properties, Youngs Modulus,
  Poissons Ratio, and Mass Density are required
• Since no loading is assumed, no other material
  properties will be used, if defined

7
Contact Regions

• Contact regions are available in free vibration
  analyses. However, since this is a purely linear
  analysis, contact behavior will differ for the
  nonlinear contact types
• Contact free vibration analyses
• Rough and frictionless
• will internally behave as bonded or no separation
• If a gap is present, the nonlinear contact
  behaviors will be free (i.e., as if no contact is
  present)
• Bonded and no separation contact status will
  depend on the pinball region size

8
Contact Regions

• Contact options (ANSYS Professional )
• Rough and frictionless
• Interface Treatment can be changed to Adjusted
  to Touch, which will make the contact surfaces
  behave as bonded and no separation
• The size of the Pinball Region may be changed
  to ensure that bonded and no separation contact
  is established even where a gap exists
• For ANSYS Structural licenses and above,
  frictional contact will behave similar to bonded
  contact if surfaces are touching but act as free
  (no contact) if contact is open.
• It is not recommended to use frictional contact
  in a free vibration analysis since it is
  nonlinear.

9
Loads and Supports

• Structural and thermal loads not used in free
  vibration
• Supports can be used in free vibration analyses
• If no or partial supports are present, rigid-body
  modes can be detected and evaluated. These modes
  will be at or near 0 Hz.
• The boundary conditions affect the mode shapes
  and frequencies of the part. Carefully consider
  how the model is constrained.
• The compression only support is a nonlinear
  support and should not be used in the analysis.
• If present, the compression only support will
  generally behave similar to a frictionless
  support.

10
Requesting Results

• Simulation triggers a free vibration analysis
  when the Frequency Finder tool is selected under
  the Solutions Branch
• The Details View of the Frequency Finder allows
  the user to specify the Max Modes to Find. The
  default is 6 modes (max is 200). Increasing the
  number of modes to retrieve will increase the
  solution time.
• The search may be limited to a specific frequency
  range of interest by selecting Yes on Limit
  Search to Range.
• By default, frequencies beginning from 0 Hz
  (rigid-body modes) will be calculated if a search
  range is not set.

11
Requesting Results

• For each requested mode an additional result
  object will be automatically added below the
  Frequency Finder
• If stress, strain, or directional displacements
  are to be requested, this can be done by adding
  the result from the Context toolbar.
• For each stress, strain, or displacement result
  added, the user can specify which mode this
  corresponds to from the Details view, under
  Mode.

If relative stress or strain results are needed,
be sure to add results under the Frequency Finder
branch, not the Solution branch. Recall that mode
shapes are relative values since no excitation is
present. Hence, stresses and strains are also
relative.
12
Solution Options

• For a free vibration analysis, typically none of
  the options in the Details view of the Solution
  branch need to be changed
• In the majority of cases, Solver Type should be
  left on the default option of Program
  Controlled
• The Analysis Type will display Free Vibration

13
Solving the Model

• Solve a free vibration analysis just like any
  other analysis by selecting the Solve button.
• A free vibration analysis is generally more
  computationally expensive than a static analysis
• If a Solution Information branchis requested
  detailed solution output
  will be available
• If stress or strain results or morefrequencies/mo
  des are requestedafter a solution is performed,
  a newsolution is required.

14
Reviewing Results

• Mode shapes
• Because there is no excitation applied to the
  structure, the mode shapes are relative values
  associated with free vibration
• Mode shapes (displacements), stresses, and
  strains represent relative, not absolute
  quantities
• The frequency is listed in the Details view of
  any result being viewed
• The animation tab below the graphics window can
  be used to help visualize the mode shapes

15
Reviewing Results

• The Worksheet tab of the Frequency Finder branch
  summarizes all frequencies in tabular form
• By reviewing the frequencies and mode shapes, one
  can geta better understanding of the possible
  dynamic response ofthe structure under different
  excitation directions

16
B. Workshop 5.1 Free Vibration

• Workshop 5.1 Free Vibration Analysis
• Goal
• Investigate the vibration characteristics of two
  motor cover designs manufactured from 18 gauge
  steel.

17
C. Free Vibration with Pre-Stress

• In some cases, one may want to consider prestress
  effects when performing a free vibration
  analysis.
• The stress state of a structure under constant
  (static) loads may affect its natural frequencies
• Consider a guitar string being tuned as the
  axial load is increased (from tightening), the
  lateral frequencies increase
• This is an example of the stress stiffening effect

18
Free Vibration with Pre-Stress

• In free vibration with pre-stress analyses,
  internally, two iterations are automatically
  performed
• A linear static analysis is initially performed
• Based on the stress state from the static
  analysis, a stress stiffness matrix S is
  calculated
• The free vibration with pre-stress analysis is
  then solved, including the S term

19
Procedure w/ Pre-Stress Effects

• A prestressed modal analysis is the same as
  running a regular free vibration analysis with
  the following exceptions
• A load (structural and/or thermal) must be
  applied to determine what the initial stress
  state of the structure is
• Results for the linear static structural analysis
  may also be requested under the Solution branch
  (not the Frequency Finder branch)
• A stress or strain result requested under the
  Frequency Finder branch will be relative
  stress/strain values for a particular mode
• A stress or strain (or displacement) result
  requested under the Solution branch will be
  absolute stress/strain/displacement values for
  the statically applied load

20
Example w/ Pre-Stress Effects

• Consider a simple comparison of a thin plate
  fixed at one end
• Two analyses will be run free vibration and
  free vibration with pre-stress effects to
  compare the differences between the two.

21
Example w/ Pre-Stress Effects

• Notice that the only difference in running a free
  vibration analysis with or without pre-stress is
  the existence of a load
• If a Frequency Finder tool is present and a load
  is present, Simulation knows that a Free
  Vibration with Pre-Stress analysis will be
  performed.
• If results such as displacement, stress, or
  strains are requested directly underneath the
  Solution branch, the results from the linear
  static analysis are reported

22
Example w/ Pre-Stress Effects

• In this example, with the applied force, a
  tensile stress state is produced, thus increasing
  the natural frequencies, as illustrated below

23
D. Workshop 5.2 Prestressed Modal

• Workshop 5.2 Prestressed Modal Analysis
• Goal simulate the modal response of the tension
  link (shown below) in both a stressed and
  unstressed state.

24
(No Transcript)