Chapter Five Vibration Analysis Vibration Analysis Chapter Overview

Chapter Five Vibration Analysis

Vibration Analysis Chapter Overview Training Manual – 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 Design. Space Entra licenses and above. ANSYS Workbench – Simulation • 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. August 26, 2005 Inventory #002265 5 -2

Vibration Analysis Basics of Free Vibration Analysis Training Manual Assumptions: – [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 ANSYS Workbench – Simulation • For a free vibration analysis, the natural circular frequencies wi and mode shapes fi are calculated from: August 26, 2005 Inventory #002265 5 -3

Vibration Analysis A. Free Vibration Analysis Procedure Training Manual – 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 ANSYS Workbench – Simulation • 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. – Review Results August 26, 2005 Inventory #002265 5 -4

Vibration Analysis … Geometry and Point Mass Training Manual – 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. ANSYS Workbench – Simulation • Similar to linear static analyses, any type of geometry supported by Simulation may be used: August 26, 2005 Inventory #002265 5 -5

Vibration Analysis … Material Properties Training Manual – Since no loading is assumed, no other material properties will be used, if defined ANSYS Workbench – Simulation • For material properties, Young’s Modulus, Poisson’s Ratio, and Mass Density are required August 26, 2005 Inventory #002265 5 -6

Vibration Analysis … Contact Regions Training Manual • 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 ANSYS Workbench – Simulation • 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: August 26, 2005 Inventory #002265 5 -7

Vibration Analysis … Contact Regions Training Manual – 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. ANSYS Workbench – Simulation • Contact options (ANSYS Professional +): August 26, 2005 Inventory #002265 5 -8

Vibration Analysis … Loads and Supports Training Manual • 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. ANSYS Workbench – Simulation • Structural and thermal loads not used in free vibration August 26, 2005 Inventory #002265 5 -9

Vibration Analysis … Requesting Results Training Manual – 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. The minimum and maximum range (in Hz) can be specified if “Limit Search to Range” is enabled. Note that this works in conjunction with “Max Modes to Find. ” If not enough modes are requested, not all modes in the frequency range may be found. ANSYS Workbench – Simulation • Simulation triggers a free vibration analysis when the Frequency Finder tool is selected under the Solutions Branch August 26, 2005 Inventory #002265 5 -10

Vibration Analysis … Requesting Results Training Manual – 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. ” ANSYS Workbench – Simulation – For each requested mode an additional result object will be automatically added below the Frequency Finder 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. August 26, 2005 Inventory #002265 5 -11

Vibration Analysis … Solution Options Training Manual • In the majority of cases, “Solver Type” should be left on the default option of “Program Controlled” – The “Analysis Type” will display “Free Vibration” ANSYS Workbench – Simulation – For a free vibration analysis, typically none of the options in the Details view of the Solution branch need to be changed August 26, 2005 Inventory #002265 5 -12

Vibration Analysis … Solving the Model Training Manual – A free vibration analysis is generally more computationally expensive than a static analysis – If a “Solution Information” branch is requested detailed solution output will be available – If stress or strain results or more frequencies/modes are requested after a solution is performed, a new solution is required. ANSYS Workbench – Simulation • Solve a free vibration analysis just like any other analysis by selecting the Solve button. August 26, 2005 Inventory #002265 5 -13

Vibration Analysis … Reviewing Results Training Manual – 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 ANSYS Workbench – Simulation • Mode shapes: August 26, 2005 Inventory #002265 5 -14

Vibration Analysis … Reviewing Results Training Manual – By reviewing the frequencies and mode shapes, one can get a better understanding of the possible dynamic response of the structure under different excitation directions ANSYS Workbench – Simulation • The Worksheet tab of the Frequency Finder branch summarizes all frequencies in tabular form August 26, 2005 Inventory #002265 5 -15

Vibration Analysis B. Workshop 5. 1 – Free Vibration Training Manual • Goal: – Investigate the vibration characteristics of two motor cover designs manufactured from 18 gauge steel. ANSYS Workbench – Simulation • Workshop 5. 1 – Free Vibration Analysis August 26, 2005 Inventory #002265 5 -16

Vibration Analysis C. Free Vibration with Pre-Stress Training Manual – 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 ANSYS Workbench – Simulation • In some cases, one may want to consider prestress effects when performing a free vibration analysis. August 26, 2005 Inventory #002265 5 -17

Vibration Analysis … Free Vibration with Pre-Stress Training Manual • 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 ANSYS Workbench – Simulation – In free vibration with pre-stress analyses, internally, two iterations are automatically performed: August 26, 2005 Inventory #002265 5 -18

Vibration Analysis … Procedure w/ Pre-Stress Effects Training Manual – 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 ANSYS Workbench – Simulation • A prestressed modal analysis is the same as running a regular free vibration analysis with the following exceptions: August 26, 2005 Inventory #002265 5 -19

Vibration Analysis … Example w/ Pre-Stress Effects Training Manual – Two analyses will be run – free vibration and free vibration with pre-stress effects – to compare the differences between the two. Free Vibration with Pre-Stress ANSYS Workbench – Simulation • Consider a simple comparison of a thin plate fixed at one end August 26, 2005 Inventory #002265 5 -20

Vibration Analysis … Example w/ Pre-Stress Effects – 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 ANSYS Workbench – Simulation • Notice that the only difference in running a free vibration analysis with or without pre-stress is the existence of a load: Training Manual August 26, 2005 Inventory #002265 5 -21

Vibration Analysis … Example w/ Pre-Stress Effects Training Manual Free Vibration with Pre-Stress 1 st mode frequency: 141 Hz 1 st mode frequency: 184 Hz ANSYS Workbench – Simulation • In this example, with the applied force, a tensile stress state is produced, thus increasing the natural frequencies, as illustrated below August 26, 2005 Inventory #002265 5 -22

Vibration Analysis D. Workshop 5. 2 – Prestressed Modal • Goal: simulate the modal response of the tension link (shown below) in both a stressed and unstressed state. ANSYS Workbench – Simulation • Workshop 5. 2 – Prestressed Modal Analysis Training Manual August 26, 2005 Inventory #002265 5 -23

August 26, 2005 Inventory #002265 5 -24