# Module 2 Modal Analysis ANSYS Dynamics.

## Presentation on theme: "Module 2 Modal Analysis ANSYS Dynamics."— Presentation transcript:

Module 2 Modal Analysis ANSYS Dynamics

A. Define modal analysis and its purpose.
Module 2 Modal Analysis A. Define modal analysis and its purpose. B. Discuss associated concepts, terminology, and mode extraction methods. C. Learn how to do a modal analysis in ANSYS. D. Work on one or two modal analysis exercises. July 22, 2004 Inventory #002110 2-2 ANSYS Dynamics

Modal Analysis A. Definition & Purpose
What is modal analysis? A technique used to determine a structure’s vibration characteristics: Natural frequencies Mode shapes Mode participation factors (how much a given mode participates in a given direction) Most fundamental of all the dynamic analysis types. July 22, 2004 Inventory #002110 2-3 ANSYS Dynamics

Modal Analysis … Definition & Purpose
Benefits of modal analysis Allows the design to avoid resonant vibrations or to vibrate at a specified frequency (speakers, for example). Gives engineers an idea of how the design will respond to different types of dynamic loads. Helps in calculating solution controls (time steps, etc.) for other dynamic analyses. Recommendation: Because a structure’s vibration characteristics determine how it responds to any type of dynamic load, always perform a modal analysis first before trying any other dynamic analysis. July 22, 2004 Inventory #002110 2-4 ANSYS Dynamics

Modal Analysis B. Terminology & Concepts
General equation of motion: Assume free vibrations and ignore damping: Assume harmonic motion ( i.e ) The roots of this equation are i2, the eigenvalues, where i ranges from 1 to number of DOF. Corresponding vectors are {u}i, the eigenvectors. Modal analysis assumes a linear elastic structure (i.e., [M] and [K] remain constant). Harmonic motion is of the form u = u0cos(wt), where w is the natural circular frequency (radians/second). July 22, 2004 Inventory #002110 2-5 ANSYS Dynamics

Modal Analysis … Terminology & Concepts
The square roots of the eigenvalues are wi , the structure’s natural circular frequencies (radians/sec). Natural frequencies fi are then calculated as fi = wi /2p (cycles/sec). It is the natural frequencies fi that are input by the user and output by ANSYS. The eigenvectors {u}i represent the mode shapes - the shape assumed by the structure when vibrating at frequency fi. July 22, 2004 Inventory #002110 2-6 ANSYS Dynamics

Modal Analysis … Terminology & Concepts (cont.)
Mode Extraction is the term used to describe the calculation of eigenvalues and eigenvectors. Mode Expansion has a dual meaning. For the reduced method, mode expansion means calculating the full mode shapes from the reduced mode shapes. For all other methods, mode expansion simply means writing mode shapes to the results file. July 22, 2004 Inventory #002110 2-7

Modal Analysis - Terminology & Concepts Mode Extraction Methods
Several mode extraction methods are available in ANSYS: Block Lanczos (default) Subspace PowerDynamics Reduced Unsymmetric Damped (full) QR Damped Which method you choose depends primarily on the model size (relative to your computer resources) and the particular application. July 22, 2004 Inventory #002110 2-8 ANSYS Dynamics

The Block Lanczos method is recommended for most applications.
Modal Analysis - Terminology & Concepts … Mode Extraction Methods - Block Lanczos The Block Lanczos method is recommended for most applications. Efficient extraction of large number of modes (40+) in most models Typically used in complex models with mixture of solids/shells/beams etc. Efficient extraction of modes in a frequency range Handles rigid-body modes well July 22, 2004 Inventory #002110 2-9 ANSYS Dynamics

Modal Analysis - Terminology & Concepts … Mode Extraction Methods - Subspace
When extracting a small number of modes (<40) in similar size models, the subspace method can be more suitable. Requires relatively less memory but large diskspace May have convergence problems when rigid body modes are present. Not recommended when constraint equations are present. Generally superseded by Block Lanczos July 22, 2004 Inventory #002110 2-10 ANSYS Dynamics

Modal Analysis - Terminology & Concepts … Mode Extraction Methods - PowerDynamics
For large (100K+ DOF) models and a small number of modes (< 20), use the PowerDynamics method. It can be significantly faster than Block Lanczos or Subspace, but: Requires large amount of memory. May not converge with poorly shaped elements or an ill-conditioned matrix. May miss modes (No Sturm sequence check) Recommended only as a last resort for large models. PowerDynamics Method A subspace technique that uses the PowerSolver (PCG) and a lumped mass matrix. Does not perform a Sturm sequence check (for missing modes); this might affect models with multiple repeated frequencies If you use PowerDynamics for a model that includes rigid body modes, be sure to issue the RIGID command (or specify the RIGID option on the Analysis Options dialog box). July 22, 2004 Inventory #002110 2-11 ANSYS Dynamics

Modal Analysis - Terminology & Concepts … Mode Extraction Methods - Reduced
For models in which lumping mass does not create a local oscillation, typically beams and spars, use the Reduced method. Memory and disk requirements are low. In general fastest eigen solver Employs matrix reduction, a technique to reduce the size of [K] and [M] by selecting a subset of DOF called master DOF. Reduction of [K] is exact but [M] loses some accuracy Accuracy of [M] depends on number and location of master DOF. Generally not recommended due to Expertise required in picking master DOF Efficient alternatives such as Block Lanczos reduced cost of hardware Reduced Method Guidelines for selecting master DOF are presented in the Structural Analysis Guide. July 22, 2004 Inventory #002110 2-12 ANSYS Dynamics

Modal Analysis - Terminology & Concepts … Mode Extraction Methods - Unsymmetric
The unsymmetric method is used for acoustics (with structural coupling) and other such applications with unsymmetric [K] and [M]. Calculates complex eigenvalues and eigenvectors: Real part is the natural frequency. Imaginary part indicates stability - negative means stable, positive means unstable. Unsymmetric Method Uses the Lanczos algorithm. Does not perform a Sturm sequence check, so missed modes are possible at the higher end. July 22, 2004 Inventory #002110 2-13 ANSYS Dynamics

Modal Analysis - Terminology & Concepts … Mode Extraction Methods - Damped
Damping is normally ignored in a modal analysis, but if its effects are significant, the Damped method is used. Typical application is rotor dynamics, where gyroscopic damping effects are important. Two ANSYS elements, BEAM4 and PIPE16, allow gyroscopic effects to be specified in the form of real constant SPIN (rotational speed, radians/time). Calculates complex eigenvalues and eigenvectors: Imaginary part is the natural frequency. Real part indicates stability - negative means stable, positive means unstable. Damped Method Uses the Lanczos algorithm. Does not perform a Sturm sequence check, so missed modes are possible at the higher end. Response at different nodes can be out of phase. Response amplitude = vector sum of real and imaginary parts. July 22, 2004 Inventory #002110 2-14 ANSYS Dynamics

Modal Analysis - Terminology & Concepts … Mode Extraction Methods - Q-R damped
A second mode extraction method that considers damping effects is the Q-R Damped method. Faster and more stable than the existing Damped Solver Works with poorly conditioned models All forms of damping allowed including damper elements Combines the best features of the real eigensolution method (Block Lanczos) and the Complex Hessenberg method (QR Algorithm) Outputs complex eigenvalues ( frequency and stability) and damping ratio of each mode Supports the use of a material dependent damping ratio [MP,DMPR] in a subsequent mode superposition harmonic analysis July 22, 2004 Inventory #002110 2-15

Modal Analysis - Terminology & Concepts … Mode Extraction Methods - Q-R damped
MODOPT,QRDAMP,NMODE July 22, 2004 Inventory #002110 2-16

Modal Analysis - Terminology & Concepts … Mode Extraction Methods - Q-R damped
Comparison Demonstrating the Superior Solution Performance of the QR Damped Mode Extraction Method July 22, 2004 Inventory #002110 2-17

Modal Analysis - Terminology & Concepts Summary for symmetric, undamped solvers
July 22, 2004 Inventory #002110 2-18

Modal Analysis C. Procedure
Four main steps in a modal analysis: Build the model Choose analysis type and options Apply boundary conditions and solve Review results Typical commands: /PREP7 ET,... MP,EX,... MP,DENS,… ! Geometry ! Mesh July 22, 2004 Inventory #002110 2-19 ANSYS Dynamics

Modal Analysis Procedure Build the Model
Remember density! Linear elements and materials only. Nonlinearities are ignored. See also Modeling Considerations in Module 1. July 22, 2004 Inventory #002110 2-20

Modal Analysis Procedure Choose Analysis Type & Options
Build the model Choose analysis type and options Enter Solution and choose modal analysis. Mode extraction options* Mode expansion options* Other options* *Discussed next Typical commands: /SOLU ANTYPE,MODAL July 22, 2004 Inventory #002110 2-21 ANSYS Dynamics

Modal Analysis Procedure … Choose Analysis Type & Options
Mode extraction options Method: Block Lanczos recommended for most applications. Number of modes: Must be specified (except Reduced method). Frequency range: Defaults to entire range, but can be limited to a desired range (FREQB to FREQE). Specification of a frequency range requires additional factorizations and it is typically faster to simply request a number of modes which will overlap the desired range. Normalization: Discussed next. Typical commands: MODOPT,... defaults to 1e8 July 22, 2004 Inventory #002110 2-22 ANSYS Dynamics

Modal Analysis Procedure … Choose Analysis Type & Options
Normalization of mode shapes: Only the shape of the DOF solution has real meaning. It is therefore customary to normalize them for numerical efficiency or user convenience. Modes are normalized either to the mass matrix or to a unit matrix (unity). Normalization to mass matrix is the default, and is required for a spectrum analysis or if a subsequent mode superposition analysis is planned. Choose normalization to unity when you want to easily compare relative values of displacements throughout the structure. Modes normalized to unity cannot be used in subsequent mode superposition analyses (transient, harmonic, spectrum or random vibration) July 22, 2004 Inventory #002110 2-23 ANSYS Dynamics

Modal Analysis Procedure … Choose Analysis Type & Options
Mode expansion: You need to expand mode shapes if you want to do any of the following: Have element stresses calculated. Do a subsequent spectrum or mode superposition analysis. Typical commands: MXPAND,... July 22, 2004 Inventory #002110 2-24 ANSYS Dynamics

Modal Analysis Procedure … Choose Analysis Type & Options
Mode expansion (continued): Recommendation: Always expand as many modes as the number extracted. The cost of this is minimal. July 22, 2004 Inventory #002110 2-25 ANSYS Dynamics

Modal Analysis Procedure … Choose Analysis Type & Options
Other analysis options: Lumped mass matrix Mainly used for slender beams and thin shells, or for wave propagation problems. Automatically chosen for PowerDynamics method. Pre-stress effects For Pre-stressed modal analysis (discussed later). Full damping Used only if Damped mode extraction method is chosen. Damping ratio, alpha damping, and beta damping are allowed. BEAM4 and PIPE16 also allow gyroscopic damping. QR damping All types of damping are allowed. Typical commands: LUMPM,OFF or ON PSTRES,OFF or ON ALPHAD,... BETAD,... DMPRAT,… Why use lumped mass matrix for wave propagation problems? Lower order elements usually give better results for wave propagation problems when using lumped mass matrix. For higher order elements consistent mass matrix is usually better. We don’t know why. Only numerical results confirm this. Why use lumped mass matrix for slender beams or very thin shells? We do not want large rotational masses in the model as there is so little stiffness in bending. If these rotations get activated (easy to do) you will get non-physical results i.e. the rotations will be erroneously large. Better to restrict the model to having only translation dofs. Lumped mass matrices avoid rotation dofs. (an exception is torsion dof of 3D beam elements). July 22, 2004 Inventory #002110 2-26 ANSYS Dynamics

Modal Analysis Procedure Apply BC’s and Solve
Build the model Choose analysis type and options Apply boundary conditions and solve Displacement constraints: Discussed next. External loads: Ignored since free vibrations are assumed. However, ANSYS creates a load vector which you can use in a subsequent mode superposition analysis. Solve: Discussed next. July 22, 2004 Inventory #002110 2-27 ANSYS Dynamics

Modal Analysis Procedure … Apply BC’s and Solve
Displacement constraints: Apply as necessary, to simulate actual fixity. Rigid body modes will be calculated in directions not constrained. Non-zero displacements are not allowed. Typical commands: DK,… !or D or DSYM DL,... DA,... July 22, 2004 Inventory #002110 2-28 ANSYS Dynamics

Modal Analysis Procedure ... Apply BC’s and Solve
Displacement constraints (continued): Be careful with symmetry Symmetry BC’s will only produce symmetrically shaped modes, so some modes can be missed. Full Model Symmetry BC Anti-Symmetry BC July 22, 2004 Inventory #002110 2-29 ANSYS Dynamics

Modal Analysis Procedure … Apply BC’s and Solve
Displacement constraints (continued): For the plate-with-hole model, the lowest non-zero mode for the full and the quarter-symmetry case is shown below. The 53-Hz mode was missed by the anti-symmetry case because ROTX is non-zero along the symmetry boundaries. July 22, 2004 Inventory #002110 2-30 ANSYS Dynamics

Modal Analysis Procedure … Apply BC’s and Solve
Typically one load step. Multiple load steps can be used to study the effect of different displacement constraints (symmetry BC in one load step and anti-symmetry BC in another, for example). Typical commands: SOLVE July 22, 2004 Inventory #002110 2-31 ANSYS Dynamics

Modal Analysis Procedure Review Results
Build the model Choose analysis type and options Apply boundary conditions and solve Review results using POST1, the general postprocessor List natural frequencies View mode shapes Review participation factors Review modal stresses July 22, 2004 Inventory #002110 2-32 ANSYS Dynamics

Modal Analysis Procedure … Review Results
Listing natural frequencies: Choose “Read Results > By Pick” in the General Postproc menu. Notice that each mode is stored in a separate substep. Typical commands: /POST1 SET,LIST July 22, 2004 Inventory #002110 2-33 ANSYS Dynamics

Modal Analysis Procedure … Review Results
Viewing mode shapes: First read in results for the desired mode using First Set, Next Set, or By Load Step. Then plot the deformed shape: General Postproc > Plot Results > Deformed Shape… Notice that the graphics legend shows mode number (SUB = ) and the frequency (FREQ = ). July 22, 2004 Inventory #002110 2-34 ANSYS Dynamics

Modal Analysis Procedure … Review Results
Viewing mode shapes (continued): You can also animate the mode shape: Utility Menu > PlotCtrls > Animate > Mode Shape... Typical commands: SET,1,1 ! First mode ANMODE,10,.05 ! Animate with 10 frames, 0.05 sec time delay SET,1,2 ! Second mode ANMODE,10,.05 SET,1,3 ! Third mode July 22, 2004 Inventory #002110 2-35 ANSYS Dynamics

Modal Analysis Procedure … Review Results
Participation Factors: Calculated for each mode in global translation and rotation directions High value in a direction indicates that the mode will be excited by forces in that direction Values are relative based on a unit displacement spectrum The final participation factor value (ROTZ) can be retrieved into a parameter using *GET command. A spectrum analysis with a specified direction (SED,0,1,0) could be used to obtain other values Also printed out (to the output file) is the effective mass. Ideally the sum of the effective masses in each direction should equal total mass of structure Effective Mass = (participation factor)2 July 22, 2004 Inventory #002110 2-36

Modal Analysis Procedure … Review Results
Modal stresses: Available if element stress calculation is activated when choosing analysis options. Stress values have no real meaning, however these can be used to highlight hot spots If mode shapes are normalized to unity, you can compare stresses at different points for a given mode shape Typical commands: PLNSOL,S,EQV ! Plot von Mises stress contours July 22, 2004 Inventory #002110 2-37 ANSYS Dynamics

Modal Analysis Procedure … Review Results
Mode shapes normalized to unity July 22, 2004 Inventory #002110 2-38 ANSYS Dynamics

Modal Analysis Procedure
Build the model Choose analysis type and options Apply boundary conditions and solve Review results July 22, 2004 Inventory #002110 2-39 ANSYS Dynamics

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. Follow the instructions in your Dynamics Workshop supplement (WS2: Modal Analysis - Plate with a Hole, Page WS-17 ). 2. Modal analysis of a model airplane wing This is left as an exercise to you. Follow the instructions in your Dynamics Workshop supplement (WS3: Modal Analysis - Model Airplane Wing, Page WS-23 ). July 22, 2004 Inventory #002110 2-40 ANSYS Dynamics