ANSYS Mechanical Linear and Nonlinear ... - web page for staff

Customer Training Material 

LLecture t 2 

Modal Analysis y 

ANSYS Mechanical 

Linear and Nonlinear 

Dynamics 

ANSYS, Inc. Proprietary 

© 2011 ANSYS, Inc. All rights reserved. 

L02-1 

Release 13.0 

March 2011

ANSYS Mechanical Linear and Nonlinear Dynamics 

Modal Analysis 

Topics covered: 

A. Define modal analysis and its purpose. 


B. Discuss associated concepts, terminology, and mode extraction 

methods methods. 

C. Learn how to do a modal analysis in Workbench. 

D. Work on one or two modal analysis exercises. 



L02-2 

Release 13.0 

March 2011


Description & Purpose 


• A modal analysis is a technique used to determine the vibration 

characteristics of structures: 

– natural frequencies 

• at what frequencies the structure would tend to naturally vibrate 

– mode shapes 

• in what shape the structure would tend to vibrate at each frequency 

– mode participation factors 

• the amount of mass that participates in a given direction for each mode 

• MMost t ffundamental d t l of f all ll the th dynamic d i analysis l i types. t 



L02-3 

Release 13.0 

March 2011


Description & Purpose 


Benefits of modal analysis 

• Allows the design to avoid resonant vibrations or to vibrate at a 

specified frequency (speaker box, for example). 

• Gives engineers an idea of how the design will respond to different 

types of dynamic loads. 

• Helps p in calculating g solution controls (time ( steps, p , etc.) ) for other 

dynamic analyses. 

Recommendation: Because a structure’s vibration characteristics 

determine how it responds to any type of dynamic load, it is generally 

recommended to perform a modal analysis first before trying any other 

dynamic analysis. 



L02-4 

Release 13.0 

March 2011


Terminology 

• A “mode” refers to the pair of one 

natural frequency and 

corresponding mode shape. 

– A structure can have any number of 

modes, up to the number of DOF in 

the model. 



L02-5 


mode 1 

← {φ} 1 

f f1 = 109 Hz 

mode 2 

← {φ} 2 

f 2 = 202 Hz 

mode 3 

← {φ} 3 

f 3 = 249 Hz 

Release 13.0 

March 2011


Assumptions & Restrictions 

• The structure is linear (i.e. constant stiffness and mass). 


• There is no damping. 

– Damped eigensolvers (MODOPT,DAMP or MODOPT,QRDAMP) may be 

accessed using Commands Objects, but will not be covered here. 

• The structure has no time varying forces, displacements, pressures, 

or temperatures applied (free vibration). 



L02-6 

Release 13.0 

March 2011


Development 

• Start with the linear general equation of motion: 

[ M ]{ ]{ u u& 

& } + [ C C]{ 

]{ u u& 

} + [ K]{ 

]{ u } = { F } 

• Assume free vibrations, and ignore damping: 

• Assume harmonic motion: 



} 0 

} 0 

[ M ]{} u& 

& + [ C] 

{} u& 

+ [ K ]{} u = { F} 

[ M ]{ ]{ u u& 

& } + [ K ]{ ]{ u } = { 0 } 

{ } { } ( ) 

{} {} ( ) 

{ } { } ( ) 

i i 

i i 

u = φ i sin ωit 

+ θi 

u& 

= ω φ cos ω t + θ 

2 { u& & } = −ω 

{ φ} 

sin ( ω t + θ ) 

i 

i 

L02-7 

i 

i 


Release 13.0 

March 2011


Development 

• Substitute and simplify 

−ω 

2 

i 

[ M ]{ ]{ u u& 

& } + [ K ]{ ]{ u } = { 0 } 

[ M ]{} φ i sin ( ωit 

+ θi 

) + [ K ]{} φ i sin ( ωit 

+ θi 

) = {} 0 

( 2 

ωω 

[ M ] + [ K ] ){ ){ φφ 

} = { 0 } 

− i 

i 


• This equality is satisfied if {φ} i = 0 (trivial, implies no vibration) or if 

( [ ] 2 

K ] −ωω [ M ] ) = { 0 } 

det = 

K i 

• This is an eigenvalue problem which may be solved for up to n 

eigenvalues eigenvalues, ω 2 

i , and n eigenvectors eigenvectors, {φ}i {φ} i, where n is the number of 

DOF. 



L02-8 

Release 13.0 

March 2011


Extraction & Normalization 

• Note that the equation 

( [ ] 2 

−ωω [ M ] ) = { 0 } 

det M 

K i 

has one more unknown than equations; therefore, an additional 

equation is needed to find a solution. solution 

– The addition equation is provided by mode shape normalization. 

• Mode shapes can be normalized either to the mass matrix 

{ } T [ M ]{ φ} 

= 1 

φ 

i 

i 


or to unity, where the largest component of the vector {φ} i is set to 1. 

• Workbench displays results normalized to the mass matrix. 

• Because of this normalization, only the shape of the DOF solution 

has real meaning. 



L02-9 

Release 13.0 

March 2011


Eigenvalues & Eigenvectors 

• The square roots of the eigenvalues 

are ω i, the structure’s natural 

circular frequencies (rad/s). 

• Natural frequencies fi can then 

calculated as f fi = ω ωi/2π /2π (cycles/s) (cycles/s). 

– It is the natural frequencies, f i in Hz, 

that are input by the user and output 

by Workbench. 

• The eigenvectors {φ} i represent the 

mode d shapes, h ii.e. th the shape h 

assumed by the structure when 

vibrating at frequency fi. ANSYS, Inc. Proprietary 


L02-10 


mode 1 

← {φ} 1 

f f1 = 109 Hz 

mode 2 

← {φ} 2 

f 2 = 202 Hz 

mode 3 

← {φ} 3 

f 3 = 249 Hz 

Release 13.0 

March 2011


Equation Solvers 

( [ ] 2 

−ω [ M ] ) = { 0} 

• The equation 

det K i 

can be solved using one of two solvers available in Workbench 

Mechanical: 

– Direct (Block Lanczos) 


• To find many modes (about 40+) of large models. 

• Performs well when the model consists of shells or a combination of shells 

and solids. 

• Uses the Lanczos algorithm where the Lanczos recursion is performed with a 

block of vectors. Uses the sparse matrix solver. 

– Iterative (PCG Lanczos) 

• To find few modes (up to about 100) of very large models (500,000+ DOFs). 

• Performs well when the lowest modes are sought for models that are 

ddominated i t d by b well-shaped ll h d 3-D 3 D solid lid elements. l t 

• Uses the Lanczos algorithm, combined with the PCG iterative solver. 

• In most cases cases, the Program Controlled option selects the optimal 

solver automatically. 



L02-11 

Release 13.0 

March 2011


Participation Factors (Solution Information) 

• The participation factors are calculated by 

γ = 

i 

T { φ} 

[ M ]{ D} 

i 


where {D} is an assumed unit displacement spectrum in each of the global 

Cartesian directions and rotation about each of these axes. 

– This measures the amount of mass moving in each direction for each mode. 

– Th The “Ratio” “R ti ” iis simply i l another th list li t of f participation ti i ti factors, f t normalized li d to t the th 

largest. 

• The concept of participation factors will be important in later chapters. 



L02-12 

Release 13.0 

March 2011


Participation Factors (Solution Information) 


• A high value in a direction indicates that the mode will be excited by forces in 

that direction. 



mode 1 mode 3 mode 5 

L02-13 

Release 13.0 

March 2011


Effective Mass (Solution Information) 

• Also printed out is the effective mass. 

2 

γ i 

2 

T 

M eff , i = = γγ 

i , if { φφ 

} i [ M ]{ ]{ φφ 

} i = 1 

T { φ } [ M ]{ ]{ φ } 

i 

i 


• Ideally, the sum of the effective masses in each direction should equal total 

mass of structure structure, but will depend on the number of modes extracted. extracted 

• The ratio of effective mass to total mass can be useful for determining 

whether or not a sufficient number of modes have been extracted. 



L02-14 

Release 13.0 

March 2011


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: 

Contact Type Static Analysis 

Linear Dynamic Analysis 

Initially Touching Inside Pinball Region 

Outside Pinball 

Region g 

Bonded Bonded Bonded Bonded Free 

No Separation No Separation No Separation No Separation Free 

Rough Rough Bonded Free Free 

Frictionless Frictionless No Separation Free Free 

Frictional Frictional 

μ = 0, No Separation 

μ > 0, Bonded 

Free Free 

• Contact behavior will reduce to its linear counterparts. 

– It is generally recommended, however, not to use a nonlinear contact 

type in a linear-dynamic analysis 



L02-15 

Release 13.0 

March 2011


Unconstrained Systems 


• An unconstrained system is one that has no constraints or supports 

and can move as a rigid body in at least one direction. 

– Rigid-body motion can be considered to be a mode of oscillation with 

zero frequency. 

– In practice, these modes may not have a frequency of exactly zero. 

“rigid-body” 

or 

“zero” zero modes 

• Note that a well-connected system can have at most six rigid-body 

modes. 

– Obt Obtaining i i more than th six i rigid-body i id b d modes d may indicate i di t that th t assemblies bli 

are not well connected. 



L02-16 

Release 13.0 

March 2011


MModal d l 

Prestress Effects 



Dynamics 



L02-17 

Release 13.0 

March 2011




• A prestressed modal analysis can be used to calculate the 

frequencies and mode shapes of a prestressed structure, such as a 

spinning turbine blade. 

– The prestress influences the stiffness of the structure through the stressstiffening 

matrix contribution. 



L02-18 

Release 13.0 

March 2011




• In free vibration with prestress analyses, two solutions are required. 

– A linear static analysis is initially performed: 

[ K K]{ 

]{ u } = { F } → [ σ ] 

– Based on the stress state [σ] from the static analysis, a stress stiffness 

matrix [S] is calculated (see Theory Reference for details): 

[ σ ] → [ S] 

– The free vibration with pre-stress analysis is then solved, including the 

[S] term: 

( 2 [ K + S ] −ω 

[ M ] ){ ){ φ } = { 0 } 

S K φ ω 

+ i i M 

• Note that the prestress only affects the stiffness of the system. 

– ie i.e. the static prestress will not be added to the modal stress 



L02-19 

Release 13.0 

March 2011




• Mechanical employs the new MAPDL linear perturbation technique 

for all prestressed eigenvalue analysis 

• Linear perturbation supports 

– Large deflection, nonlinear pre-stress 

– Prestressed modal from any y restart ppoint 

– Handling true contact status from the static analysis 

– Cyclic symmetry 

[K T [K T 

i ] 

• Any time point from a static or 

transient structural analysis 

can be perturbed. p 

• Uses global tangent stiffness 

matrix [K i T ] from the time point. 

• Restart files must be available. 



L02-20 

t i 

Release 13.0 

March 2011



• Tangent Stiffness matrix 

K = K + K + 

T 

i 

+ 

Mat 

i 

SpinSoftening 

i 

Contact 

i 

K + 

• Material Stiffness [K i Mat ] 

K 

K 

LoadStiffness 

i 

StressStiffness 

i 

[K i T ] 


– For nonlinear materials, only the linear portion is used 

– For hyperelastic materials, the tangent material properties at the point of restart 

are used 

• Stress Stiffening [K i StressStiffness ] / Spin softening [Ki SpinSoftening ] 

– Effects included automatically in large deflection analyses 

• Contact stiffness [K i Contact ] 

– Contact behavior can be changed prior to the modal analysis 

– (more on this later) 



L02-21 

t i 

Release 13.0 

March 2011


MModal d l 

Procedure 



Dynamics 



L02-22 

Release 13.0 

March 2011


Procedure 

• Drop a Modal (ANSYS) system into the project schematic. 



L02-23 


Release 13.0 

March 2011


Procedure 

• Create new geometry, or link to 

existing geometry. 



L02-24 


• Edit the Model cell to bring up the 

Mechanical application. 

Release 13.0 

March 2011


Preprocessing 

• Verify materials, connections, and mesh settings. 

– This was covered in Workbench Mechanical Intro. 



L02-25 


Release 13.0 

March 2011


Preprocessing 

• Optional: Specify “Cyclic Region” 

– Matched mesh will be created at the low-high regions 



L02-26 


Select Harmonic 

Indices of interest in 

Analysis Settings 

Release 13.0 

March 2011


Preprocessing 

• Add supports to the model. 

– Displacement constrains must have a magnitude of zero. 



L02-27 


Release 13.0 

March 2011


Solution Settings 

• Choose the number of modes to 

extract. 



L02-28 


• If needed, upper and lower bounds 

on frequency may be specified to 

extract the modes within a specified 

range. 

Release 13.0 

March 2011


Solution Settings 

• If the Program-Controlled solver 

selection is not appropriate, the 

solver type can be changed to 

either Direct or Iterative. 



L02-29 


• Stress and strain results may be 

turned on under Output Controls. 

Release 13.0 

March 2011


Postprocessing 

• Total-deformation results may be 

quickly inserted by highlighting 

multiple rows in the tabular view or 

histogram view. view 



L02-30 


Release 13.0 

March 2011




• If stress/strain were requested, these results may also be access from the 

Solution Toolbar. 



L02-31 

Release 13.0 

March 2011




• If cyclic symmetry was activated, results will be automatically expanded. 

Cyclic Expansion 

Harmonic 

Index 

Control 



Interactive Frequency-Spectrum Display 

L02-32 

Modes listed 

by Harmonic 

Indices 

Release 13.0 

March 2011


MModal d l 

Prestressed Procedure 



Dynamics 



L02-33 

Release 13.0 

March 2011


Procedure 

• The procedure to do a prestressed 

modal analysis is essentially the 

same as a regular modal analysis, 

except that you first need to 

prestress the structure by doing a 

static analysis. 

• The static analysis results in a 

stressed structure, which is used as 

the initial condition for the modal 

analysis. l i 



L02-34 


Release 13.0 

March 2011


Procedure 

• Drop a Static Structural (ANSYS) system into the project schematic. 



L02-35 


Release 13.0 

March 2011


Procedure 

• Drop a Modal (ANSYS) system onto 

the Solution cell of the Modal 

system. 



L02-36 


• Note the circular-ended connector, 

indicating a data transfer from the 

Static to the Modal analysis. 

Release 13.0 

March 2011


Procedure 

• Create new geometry, or link to 

existing geometry. 



L02-37 


• Edit the Model cell to bring up the 

Mechanical application. 

Release 13.0 

March 2011


Static: Preprocessing 


• In the Static Structural system, insert the loads and supports that will cause 

the prestressed-state to occur. 



L02-38 

Release 13.0 

March 2011


Preprocessing 

• Optional: Specify “Cyclic Region” 

– Matched mesh will be created at the low-high regions 



L02-39 


Select Harmonic 

Indices of interest in 

Analysis Settings 

Release 13.0 

March 2011


Static: Analysis Settings 


• Setup restart controls of parent static structural analysis according 

to requirements. 

– Default is to retain a restart point for the last substep of the last load step. 

– Recall: any substep can be perturbed, providing there is a restart point. 



L02-40 

Release 13.0 

March 2011


Static: Postprocessing 



L02-41 


• Review the static results before 

proceeding. 

Release 13.0 

March 2011


Analysis Settings: Prestress Environment 

• In the modal analysis, user can specify 

which restart point from the static 

analysis will be used as the prestress 

environment. 

• This can be specified by either 

(1) End of load step 

(2) Time 



L02-42 


Release 13.0 

March 2011


Analysis Settings: Contact Status 

• The user also has some control over the 

contact status. 

• Available options are: 

(1) Use True Status 

– Use the status at the restart point. 

(2) Force Sticking 

– For frictional contact with mu>0, set 

sliding elements to sticking. 

(3) Force Bonded 

– Use bonded contact for all contact 

pairs that are closed. 



L02-43 


Release 13.0 

March 2011




• The modal results may be reviewed as described in the previous section. 



L02-44 

Release 13.0 

March 2011




• Note that the prestressed state increased the frequencies of this structure. 

– e.g. the first mode in this example increased from 108.3 Hz to 274.6 Hz 

Not Prestressed Prestressed 

• A prestress may not always increase the natural frequencies; a compressive 

load will decrease the frequencies. 

– In fact, fact a sufficiently-high compressive load will result in a natural frequency of 

zero, effectively replicating the results of a buckling analysis. 



L02-45 

Release 13.0 

March 2011


D. Workshop - Modal Analysis 

This workshop consists of two problems: 

1. Modal analysis of a plate with a hole 


– A step-by-step description of how to do the analysis. 

– You may choose to run this problem yourself, or your instructor may 

show it as a demonstration. 

(WS2A: Modal Analysis - Plate with a Hole). 

22. Pre-stressed Pre stressed Modal analysis of a model airplane wing 

– This is left as an exercise to you. 

(WS2B: Modal Analysis - Model Airplane Wing). 



L02-46 

Release 13.0 

March 2011

ANSYS Mechanical Linear and Nonlinear ... - web page for staff

Create successful ePaper yourself

Delete template?

Save as template?