Chapter 1 * Chapter 2 * Chapter 3 * Chapter 4 * Chapter 5 * Chapter 6 * Chapter 7 * Chapter 8 * Chapter 9 * Chapter 10 * Chapter 11 * Chapter 12 * Chapter 13 * Chapter 14
You can do modal analysis on a prestressed structure, such as a spinning turbine blade. Another useful feature is modal cyclic symmetry, which allows you to review the mode shapes of a cyclically symmetric structure by modeling just a sector of it.
Modal analysis in the ANSYS family of products is a linear analysis. Any nonlinearities, such as plasticity and contact (gap) elements, are ignored even if they are defined. You can choose from several mode extraction methods: subspace, Block Lanczos, PowerDynamics, reduced, unsymmetric, and damped. The damped method allows you to include damping in the structure. Details about mode extraction methods are covered later in this section.
Section 3.6, "Sample Modal Analysis (Command or Batch Method)," shows you the sequence of commands you issue (either manually or while running ANSYS as a batch job) to perform an example modal analysis. Section 3.5, "Sample Modal Analysis (GUI Method)," shows you how to execute the same sample analysis using menu choices from the ANSYS GUI. (To learn how to use the commands and GUI selections for building models, read the ANSYS Modeling and Meshing Guide.)
For detailed, alphabetized descriptions of the ANSYS commands, see the ANSYS Commands Reference.
1. Build the model.
2. Apply loads and obtain the solution.
3. Expand the modes.
4. Review the results.
1. Enter the ANSYS solution processor.
Command(s):
Main Menu>Solution
2. Define the analysis type and analysis options. ANSYS offers these options for a modal analysis. Each of these options is explained in detail below:
Table 31 Analysis types and analysis options
Option

Command

GUI Path

New Analysis

ANTYPE

Main Menu>Solution>Analysis TypeNew Analysis

Analysis Type: Modal

ANTYPE

Main Menu>Solution>Analysis TypeNew
Analysis>Modal

Mode Extraction Method

MODOPT

Main Menu>Solution>Analysis Options

Number of Modes to Extract

MODOPT

Main Menu>Solution>Analysis Options

No. of Modes to Expand*

MXPAND

Main Menu>Solution>Analysis Options

Mass Matrix Formulation

LUMPM

Main Menu>Solution>Analysis Options

Prestress Effects Calculation

PSTRES

Main Menu>Solution>Analysis Options

NoteRestarts are not valid in a modal analysis. If you need to apply different sets of boundary conditions, do a new analysis each time (or use the "partial solution" procedure described in Chapter 3 of the ANSYS Basic Analysis Procedures Guide).
When you specify a mode extraction method, ANSYS automatically chooses the appropriate equation solver.
NoteThe damped and unsymmetric methods are not available in the ANSYS/LinearPlus program.
For the unsymmetric and damped methods, requesting a larger number of modes than necessary reduces the possibility of missed modes, but results in more solution time.
NoteYou can use only axisymmetric loads for prestressing harmonic elements such as PLANE25 and SHELL61.
Field: FREQB, FREQE
Specify a frequency range for mode extraction. The FREQB field specifies the first shift pointthe point about which eigenvalues converge the fastest. In most cases, you do not need to specify this field because it defaults to 1. FREQE is valid only for the reduced method.
Field: PRMODE
Number of reduced modes to print. Use this option to get a listing of the reduced mode shapes on the printed output file (Jobname.OUT). Valid only for the reduced method.
Field: Nrmkey
Mode shape normalization. Choose between normalization to the mass matrix [M] (default) and normalization to unity [I]. If you plan to do a subsequent spectrum or mode superposition analysis, the mode shapes must be normalized to [M]. To later obtain the maximum response of each mode (modal response), multiply the mode shape by the mode coefficient. You can accomplish this by retrieving the mode coefficient with the *GET command (after the spectrum analysis) and using it as a scale factor in the SET command.
Field: RIGID
Used to extract zero frequency modes for subspace iteration analyses with known rigidbody motions. Valid for subspace and PowerDynamics methods only.
Field: SUBOPT
Used to specify various subspace iteration options. See the ANSYS Commands Reference for details. Valid for subspace and PowerDynamics methods only.
Field: CEkey
Used to specify the method for processing constraint equations. Options are the direct elimination method, the Lagrange multiplier (quick) method, or the Lagrange multiplier (accurate) method. Valid for Block Lanczos method only. (Refer to Table 36, CE Methods in Section 3.10, "Modal Analysis of a Cyclically Symmetric Structure.")
3. Define master degrees of freedom. These are required only for the reduced mode extraction method.
Main Menu>Solution>Master DOFs>User SelectedDefine
4. Apply loads on the model. The only "loads" valid in a typical modal analysis are zerovalue displacement constraints. (If you input a nonzero displacement constraint, the program assigns a zerovalue constraint to that DOF instead.) Other loads can be specified, but are ignored (see Note below). For directions in which no constraints are specified, the program calculates rigidbody (zerofrequency) as well as higher (nonzero frequency) free body modes. Table 32 shows the commands to apply displacement constraints. Notice that you can apply them either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). For a general discussion of solidmodel loads versus finiteelement loads, see Chapter 2 of the ANSYS Basic Analysis Procedures Guide.
NoteOther loadsforces, pressures, temperatures, accelerations, etc.can be specified in a modal analysis, but they are ignored for the mode extraction. However, the program will calculate a load vector and write it to the mode shape file (Jobname.MODE) so that it can be used in a subsequent modesuperposition harmonic or transient analysis.
Table 32 Loads applicable in a modal analysis
Load Type

Category

Cmd
Family

GUI Path

Displacement (UX, UY,
UZ, ROTX, ROTY, ROTZ)

Constraints

D

Main Menu>Solution>LoadsApply>
StructuralDisplacement

Table 33 Load commands for a modal analysis
Load Type

Solid
Model or
FE

Entity

Apply

Delete

List

Operate

Apply
Settings

Displacement

Solid
Model

Keypoints

DK

DKDELE

DKLIST

DTRAN




Solid
Model

Lines

DL

DLDELE

DLLIST

DTRAN




Solid
Model

Areas

DA

DADELE

DALIST

DTRAN




Finite
Elem

Nodes

D

DDELE

DLIST

DSCALE

DSYM DCUM

For example, to apply a displacement load to a line, follow this GUI path:
GUI:
Main Menu>Solution>LoadsApply>StructuralDisplacement>On lines
GUI:
Utility Menu>List>Loads>load type
5. Specify load step options. The following options are available for a modal analysis:
Table 34 Load step options
Option

Command

GUI Path

Damping (Dynamics) Options


Alpha (mass) Damping

ALPHAD

Main Menu>Solution>Load Step OptsTime/Frequenc>
Damping

Beta (stiffness) Damping

BETAD

Main Menu>Solution>Load Step OptsTime/Frequenc>
Damping

Constant Damping Ratio

DMPRAT

Main Menu>Solution>Load Step OptsTime/Frequenc>
Damping

MaterialDependent
Damping Ratio

MP,DAMP

Main Menu>Solution>Load Step OptsOther>Change Mat
Props>Temp DependentPolynomial

If you include damping, and specify the damped mode extraction method, the eigenvalues calculated are complex; see "Mode Extraction Methods" for details. See the section "Damping" in Chapter 5 for more information on damping.
NoteDamping can be specified in a nondamped modal analysis if a singlepoint response spectrum analysis is to follow the modal analysis. Although the damping does not affect the eigenvalue solution, it is used to calculate an effective damping ratio for each mode, which is then used to calculate the response to the spectrum. Spectrum analyses are discussed in Chapter 6.
6. Save a backup copy of the database to a named file. You can then retrieve your model by reentering the ANSYS program and issuing RESUME.
Command(s):
Utility Menu>File>Save as
7. Start solution calculations.
Command(s):
Main Menu>Solution>SolveCurrent LS
You can take two steps to investigate the missed mode. See Section 15.10 of the ANSYS Theory Reference (Subspace Method/Sturm Sequence Check and Shifting subsections) for more information.
1. Use more iteration vectors.
Command(s):
Main Menu>Solution>Analysis Options>Subspace
2. Click on OK to display the Subspace Modal Analysis dialog box.
3. Change the shift point used in eigenvalue extraction.
Command(s):
Main Menu>Solution>Analysis Options>Subspace
4. Click on OK to display the Subspace Modal Analysis dialog box.
Command(s):
Main Menu>Finish
Command(s):
Main Menu>Solution
NoteYou must explicitly leave SOLUTION (using the FINISH command) and reenter (/SOLUTION) before performing the expansion pass.
2. Activate the expansion pass and its options. ANSYS offers these options for the expansion pass:
Table 35 Expansion pass options
Option

Command

GUI Path

Expansion Pass On/Off

EXPASS

Main Menu>Solution>Analysis TypeExpansionPass

No. of Modes to Expand

MXPAND

Main Menu>Solution>Load Step OptsExpansionPass>Expand
Modes

Freq. Range for
Expansion

MXPAND

Main Menu>Solution>Load Step OptsExpansionPass>Expand
Modes

Stress Calc. On/Off

MXPAND

Main Menu>Solution>Load Step OptsExpansionPass>Expand
Modes

3. Specify load step options. The only options valid in a modal expansion pass are output controls:
Main Menu>Solution>Load Step OptsOutput Ctrls>Solu Printout
Main Menu>Solution>Load Step OptsOutput Ctrls>DB/Results File
4. Start expansion pass calculations.
Main Menu>Solution>Current LS
5. Repeat steps 2, 3, and 4 for additional modes to be expanded (in different frequency ranges, for example). Each expansion pass is stored as a separate load step on the results file.
Caution: Spectrum analyses expect all expanded modes to be in one load step. In the single point response spectrum (SPOPT,SPRS) and Dynamic Design analysis method (SPOPT,DDAM), the modal expansion can be performed after the spectrum analysis, based on the significance factor SIGNIF on the MXPAND command. If you want to perform modal expansion after the spectrum analysis, choose NO for mode expansion (MXPAND) on the dialog box for the modal analysis options (MODOPT).
6. Leave SOLUTION. You can now review results in the postprocessor.
Command(s):
Close the Solution menu.
NoteThe expansion pass has been presented here as a separate step. However, if you include the MXPAND command in the modal solution step, the program not only extracts the eigenvalues and eigenvectors, but also expands the specified mode shapes.
Command(s):
Main Menu>General Postproc>Read Resultssubstep
2. Perform any desired POST1 operations. Typical modal analysis POST1 operations are explained below:
***** INDEX OF DATA SETS ON RESULTS FILE *****
SET TIME/FREQ LOAD STEP SUBSTEP CUMULATIVE 1 22.973 1 1 1 2 40.476 1 2 2 3 78.082 1 3 3 4 188.34 1 4 4Command(s):
Main Menu>General Postproc>List Results>Results Summary
Main Menu>General Postproc>Plot Results>Deformed Shape
Main Menu>Solution>Master DOFs>List All
NoteTo display the master DOFs graphically, plot the nodes (Utility Menu> Plot>Nodes or command NLIST).
Main Menu>General Postproc>Element Table>Define Table
Main Menu>General Postproc>Plot Results>Contour PlotNodal Solu or Element Solu
Main Menu>General Postproc>Element Table>Plot Element Table
Main Menu>General Postproc>Plot Results>Contour PlotLine Elem Res
Caution: Derived data, such as stresses and strains, are averaged at the nodes by the PLNSOL command. This averaging results in "smeared" values at nodes where elements of different materials, different shell thicknesses, or other discontinuities meet. To avoid the smearing effect, use selecting (described in Chapter 7 of the ANSYS Basic Analysis Procedures Guide) to select elements of the same material, same shell thickness, etc. before issuing PLNSOL.
Main Menu>General Postproc>List Results>solution option
Main Menu>General Postproc>List Results>Sorted ListingSort
Nodes or Sort Elems
See the ANSYS Commands Reference for a discussion of the ANTYPE, MODOPT, M, TOTAL, EXPASS, MXPAND, SET, and PLDISP commands.
2. Enter the text "Modal analysis of a model airplane wing" and click on OK.
3. Choose menu path Main Menu>Preferences.
4. Click the Structural option on. Click OK.
2. Click on Add. The Library of Element Types dialog box appears.
3. In the left scroll box, click once on "Structural Solid."
4. In the right scroll box, click once on "Quad 4node 42."
5. Click on Apply.
6. In the right scroll box, click once on "Brick 8node 45."
7. Click on OK.
8. Click on Close in the Element Types dialog box.
2. Click on OK to specify material number 1. A second dialog box appears.
3. Enter 3800 for EX.
4. Enter 1.033e3 for DENS.
5. Enter .3 for NUYX.
6. Click on OK.
2. Enter 1 for keypoint number, and 0,0,0 for the X, Y, and Z locations. Use the TAB key to move between fields.
3. Click on Apply.
4. Repeat this procedure for the following keypoints and X, Y, and Z locations:
Keypoint 2: 2,0,0
Keypoint 3: 2.3,0.2,0
Keypoint 4: 1.9,.45,0
Keypoint 5: 1,.25,0
5. After you have entered the last keypoint, click on OK.
6. Choose menu path Utility Menu>PlotCtrls>Window Controls>Window Options.
7. In the scroll box for Location of triad, scroll to "Not shown" and select it.
8. Click on OK.
9. Choose menu path Utility Menu>PlotCtrls>Numbering.
10. Click Keypoint numbering on and click on OK. The numbered keypoints appear in the ANSYS Graphics window.
2. Click once on keypoints 1 and 2, in that order. A line appears between the keypoints.
3. Click once on keypoints 5 and 1, in that order. A line appears between the keypoints.
4. Click on OK in the picking menu.
5. Choose menu path Main Menu>Preprocessor>ModelingCreate> LinesSplines> With options>Spline thru kps. The BSpline picking menu appears.
6. Pick keypoints 2, 3, 4, 5 in that order and click on OK. The BSpline dialog box appears.
7. Enter 1,0,0 for XV1, YV1, ZV1, and enter 1,.25,0 for XV6, YV6, ZV6.
8. Click on OK. The curved part of the wing appears on the drawing.
2. Click once on all three lines.
3. Click on OK. The area in the lines is highlighted.
4. Click on SAVE_DB on the ANSYS Toolbar.
2. Enter 0.25 for the element edge length.
3. Click on OK.
4. Choose menu path Main Menu>Preprocessor>MeshingMesh> AreasFree. The Mesh Areas picking menu appears.
5. Click on Pick All. (If a warning box appears, click on Close. See Note below.)
NoteThe PLANE42 element is used in this example to accommodate ANSYS/ED users. Using this element results in the following warning: "The mesh of area 1 contains PLANE42 triangles, which are much too stiff in bending. Use quadratic (6 or 8 noded) elements if possible." You can perform this same analysis using the PLANE82 element, if you are not using ANSYS/ED.
6. Click on SAVE_DB on the ANSYS Toolbar.
2. Delete the element edge length.
3. Enter 10 for number of element divisions.
4. Click on OK.
2. Enter 2 for element type number.
3. Click on OK.
4. Choose menu path Main Menu>Preprocessor>ModelingOperate> Extrude/Sweep>AreasBy XYZ Offset. The Extrude Area by Offset picking menu appears.
5. Click on Pick All. The Extrude Areas by XYZ Offset dialog box appears.
6. Enter 0,0,10 for offsets for extrusion.
7. Click on OK. (If a warning box appears, click on Close. See Note below.)
9. Click on "Iso," then on Close.
10. Click on SAVE_DB on the ANSYS Toolbar.
2. Click the modal analysis option on and click on OK.
3. Choose menu path Main Menu>Solution>Analysis Options. The Modal Analysis dialog box appears.
4. Click the subspace option on.
5. Enter 5 for number of modes to extract.
NoteIf you want to perform spectrum analysis afterwards (ANTYPE,SPECTR and SPOPT,SPRS or DDAM), choose NO for mode expansion (MXPAND) and skip step 13.
6. Click on OK. The Subspace Modal Analysis dialog box appears.
7. Click OK to accept the default values.
1. Choose menu path Utility Menu>Select>Entities. The Select Entities dialog box appears.
2. In the top two scroll boxes, select "Elements" and "By Attributes."
3. Click the Elem type num option on.
4. Enter 1 in the Min,Max,Inc. area for the element type number.
5. Click the Unselect option on.
6. Click on Apply.
2. In the top two scroll boxes, select "Nodes" and "By Location."
3. Click the Z coordinates option on.
4. Enter 0 in the Min,Max area for the Z coordinate location.
5. Click the From Full option on.
6. Click on Apply.
7. Choose menu path Main Menu>Solution>LoadsApply>Structural Displacement>On Nodes. The Apply U,ROT on Nodes picking menu appears.
8. Click on Pick All. The Apply U,ROT on Nodes dialog box appears.
9. Click on "All DOF."
10. Click on OK.
11. In the Select Entities dialog box, select "By Num/Pick" in the second scroll box.
12. Click on Sele All.
13. Click on Cancel.
2. Enter 5 for number of modes to expand.
3. Click on OK.
4. Choose menu path Main Menu>Solution>SolveCurrent LS. Review the information in the /STAT Command dialog box, and then close the dialog box using File>Close.
5. Click on OK. Click on Yes to accept the warning: "A check of your model data produced 21 warnings. Should the SOLV command be executed?"
6. Click on Yes to accept the warning: "A check of your load data produced 1 warning. Should the SOLV command be executed?"
7. Click on Close when the solution is done.
2. Choose menu path Utility Menu>PlotCtrls>Animate>Mode Shape. The Animate Mode Shape dialog box appears.
3. Enter .05 for the time delay in seconds.
4. Click on OK. The Animation Controller dialog box appears, and the animation begins.
5. Click on Stop to stop the animation.
6. Choose menu path Main Menu>General Postproc>Read ResultsNext Set.
7. Chose menu path Utility Menu>PlotCtrls>Animate>Mode Shape. The Animate Mode Shape dialog box appears.
8. Click on OK to accept the previous settings. The animation begins.
9. Click on Stop to stop the animation.
10. Repeat steps 69 for the remaining three modes.
2. Choose menu path Utility Menu>PlotCtrls>Animate>Mode Shape. The Animate Mode Shape dialog box appears. Click on OK to display the Media Player  file.avi dialog box.
3. Choose Edit>Options on the dialog box. The Options dialog box appears.
4. Click on "Auto Repeat" and click on OK.
5. Click on the Play toolbar button (>) and observe the animation.
6. Click on the Stop toolbar button ([]).
7. Choose menu path Main Menu>General Postproc>Read ResultsNext Set.
8. Chose menu path Utility Menu>PlotCtrls>Animate>Mode Shape.
9. Click on the Play toolbar button and observe the animation.
10. Click on the Stop toolbar button.
11. Repeat steps 710 for the remaining three modes.
2. Choose QuitNo Save!
3. Click on OK.
/FILNAM,MODAL /TITLE,Modal Analysis of a Model Airplane Wing /PREP7 ET,1,PLANE42 ! Define PLANE42 as element type 1 ET,2,SOLID45 ! Define SOLID45 as element type 2 MP,EX,1,38000 MP,DENS,1,1.033E3 MP,NUXY,1,.3 K,1 ! Define keypoint 1 at 0,0,0 K,2,2 ! Define keypoint 2 at 2,0,0 K,3,2.3,.2 ! Define keypoint 3 at 2.3,.2,0 K,4,1.9,.45 ! Define keypoint 4 at 1.9,.45,0 K,5,1,.25 ! Define keypoint 5 at 1,.25,0 LSTR,1,2 ! Create a straight line between keypoints 1 and 2 LSTR,5,1 ! Create a straight line between keypoints 5 and 1 BSPLIN,2,3,4,5,,,1,,,1,.25 ! Create a Bspline AL,1,3,2 ESIZE,.25 AMESH,1 ESIZE,,10 TYPE,2 VEXT,ALL,,,,,10 /VIEW,,1,1,1 /ANG,1 /REP EPLOT FINISH /SOLU ANTYPE,MODAL ! Choose modal analysis type MODOPT,SUBSP,5 ! Choose the subspace mode extraction method, extracting 5 modes ESEL,U,TYPE,,1 ! Unselect element type 1 NSEL,S,LOC,Z,0 D,ALL,ALL NSEL,ALL MXPAND,5 SOLVE FINISH /POST1 SET,LIST,2 SET,FIRST PLDISP,0 ANMODE,10,.5E1 SET,NEXT PLDISP,0 ANMODE,10,.5E1 SET,NEXT PLDISP,0 ANMODE,10,.5E1 SET,NEXT PLDISP,0 ANMODE,10,.5E1 SET,NEXT PLDISP,0 ANMODE,10,.5E1 FINISH /EXIT
The ANSYS Verification Manual consists of test case analyses demonstrating the analysis capabilities of the ANSYS family of products. While these test cases demonstrate solutions to realistic analysis problems, the ANSYS Verification Manual does not present them as stepbystep examples with lengthy data input instructions and printouts. However, most ANSYS users who have at least limited finite element experience should be able to fill in the missing details by reviewing each test case's finite element model and input data with accompanying comments.
The following list shows you the variety of modal analysis test cases that the ANSYS Verification Manual includes:
1. Build the model and obtain a static solution with prestress effects turned on [PSTRES,ON]. The same lumped mass setting [LUMPM] used here must also be used in the later prestress modal analysis. Chapter 2 describes the procedure to obtain a static solution.
2. Reenter SOLUTION and obtain the modal solution, also with prestress effects turned on (reissue PSTRES,ON). Files Jobname.EMAT and Jobname.ESAV from the static analysis must be available.
3. Expand the modes and review them in the postprocessor.
Step 1 above can also be a transient analysis, but you should remember to save the EMAT and ESAV files at the desired time point.
! Initial, large deflection static analysis ! /PREP7 ... FINISH /SOLU ANTYPE,STATIC ! Static analysis NLGEOM,ON ! Large deflection analysis PSTRES,ON ! Flag to calculate the prestress matrix ... SOLVE FINISH ! ! Prestressed modal analysis ! /SOLU ANTYPE,MODAL ! Modal analysis UPCOORD,1.0,ON ! Add previous displ. to coordinates and then zero the displacements PSTRES,ON ! Prestress effects on MODOPT,... ! Select eigensolver MXPAND,... ! Specify number of modes to be expanded, if desired PSOLVE,TRIANG ! Triangularizes the matrices. Creates .REDM or ! .FULL file depending on solver selected on MODOPT ! command. PSOLVE,EIGxxxx ! Calculates the eigenvalues and eigenvectors. ! Use EIGREDUC, EIGFULL, EIGUNSYM, or EIGDAMP to ! match MODOPT command. FINISH /SOLU !Additional solution step for expansion. EXPASS,ON PSOLVE,EIGEXP ! Expands the eigenvector solution. Required if you ! want to review mode shapes in the postprocessor. FINISH
Figure 32 An example of a cyclically symmetric structure
Figure 33 Some examples of nodal diameters, i
For complicated structures with cyclic symmetry (such as a turbine wheel), lines of zero displacement might not be observable in a mode shape. The mathematical definition of nodal diameter in ANSYS is, therefore, more general and does not necessarily correspond to the number of lines of zero displacement through the structure.
The number of nodal diameters is an integer that determines the variation in the value of a single DOF at points spaced at a circumferential angle equal to the sector angle. For a number of nodal diameters equal to ND, this variation is described by the function cos(ND*THETA).
The above definition allows a varying number of waves to exist around the circumference for a given nodal diameter, as long as the DOF at points separated by the sector angle vary by cos(ND*THETA). For example, nodal diameter = 0 and a 60 degree sector will produce modes with 0, 6, 12, ..., 6n waves around the circumference. (In some references, the term "mode" is used instead of nodal diameter as defined above, and the term nodal diameter is used to describe the actual number of observable waves around the structure.)
NoteThe procedure for modal cyclic symmetry uses two predefined ANSYS macros: CYCGEN and CYCSOL. Both assume a model with structural solid or shell elements.
Figure 34 Procedure for modal cyclic symmetry (stressfree)
1. Define a basic sector model that is cyclically symmetric in the global cylindrical coordinate system (CSYS = 1). (See the ANSYS Modeling and Meshing Guide for information on creating a model.) The angle () spanned by the basic sector should be such that n = 360, where n is an integer. The basic sector must consist only of finite elements; no superelements are allowed. Internal coupling and constraint equations are allowed. Boundary conditions, if any, are applied later (step 5).
2. Select the nodes on the edge with the lowest angle and define a component. Making a component of the other edge is optional.
Command(s):
Utility Menu>Select>Comp/Assembly>Create Component
3. Reactivate all entities.
Command(s):
Utility Menu>Select>Everything
4. Run the CYCGEN macro. This macro creates a second sector that is overlaid on the basic sector. There is a constant nodal offset (parameter NTOT) between the sectors. The modal analysis is conducted with this twosector model. The macro copies internal couplings and constraint equations from the basic sector to the second sector.
Command(s):
Main Menu>Preprocessor>Cyclic Sector
Utility Menu>Plot>Elements
5. While still in PREP7, define all applicable boundary conditions. They must be defined on both sectors. We recommend selecting nodes by location rather than by node numbers. Symmetry boundary conditions are not necessary if there is no prestress.
6. Go into SOLUTION. Define modal analysis and its options. Use only the Block Lanczos (recommended) or subspace method for modal cyclic symmetry. (See the MODOPT command in the ANSYS Commands Reference for information about the options for using the Block Lanczos method.) Also specify the number of modes to be expanded at this time.
Command(s):
Main Menu>Solution >Analysis Type>Modal
Main Menu>Solution >Analysis Options>Block Lanczos
See Table 36 for a list of the CE methods that are available for the Block Lanczos eigensolver:
Table 36 CE methods
Cekey

CEs Processed By:

When Applicable:

0

Direct Elimination Method

When only a few constraint equations (CEs) are present in the
model. For example, in a 100,000DOF problem, only about
1,000 or so CEs are present.
When a large number of CEs are present, the memory requirements of this method very often become too high. In such cases, the Lagrange Multiplier Method (Cekey=1 or 2) is recommended.

1, 2

Lagrange Multiplier
Method

A large number of constraint equations are present in the model.
For example, in a 100,000DOF problem, more than 1,000 or so
CEs are present.
Typically, when CEINTF, CERIG, or CYCSOL is used, several CEs are generated with a single command. In these cases, the Lagrange Multiplier Method is recommended. Cekey = 1: "Quick Solution" is a fast approach, similar in CPU time to the Direct Elimination Method. However, the higher frequencies extracted tend to be approximate by about 1  2%. This error occurs when the higher frequencies are two or more orders of magnitude larger than the lowest frequencies extracted. Cekey = 2: "Accurate Solution" is an exact approach. However, the CPU time taken is roughly twice as much as that taken by the "Quick Solution."

Command(s):
Main Menu>Solution>Modal Cyclic Sym
Load Step

Substep

Comment

1

1

1st mode of nodal diameter 0

1

2

2nd mode of nodal diameter 0

2

1

1st mode of nodal diameter 1

2

2

2nd mode of nodal diameter 1

Command(s):
Main Menu>General Postprocessing>Expand sector
NoteThe /EXPAND command can also be used to show full model results. See the ANSYS Commands Reference for more information about the /EXPAND command (Utility Menu>Plot Cntrls>Style>Symmetry Expansion).
The steps involved are essentially the same as for the stressfree case, except that a static solution is required to calculate the prestress in the basic sector. Thus, steps 14 and 7 and 8 are the same as for the stressfree case. Steps 5 and 6 are described below.
5. Enter SOLUTION and define static loads and boundary conditions that induce the prestress. Use the PSTRES command to achieve prestress calculation, and obtain the static solution [SOLVE].
6. Reenter PREP7 and define modal analysis and its options, as explained for the stressfree case. Be sure to include prestress effects with the PSTRES command.
NoteSymmetry boundary conditions must be removed after the static solution is obtained.
Figure 36 Procedure for modal cyclic symmetry (prestressed)
where = stiffness matrix
= mode shape vector (eigenvector) of mode i
= natural circular frequency of mode i ( is the eigenvalue)
= mass matrix
Many numerical methods are available to solve the above equation. ANSYS offers six methods:
The first four, the subspace, the Block Lanczos, the PowerDynamics, and the reduced methods are the most commonly used. Table 37 compares these four mode extraction methods. Following the table is a brief description of each of the six types of mode extraction methods.
Table 37 Table of symmetric system eigensolver choices
Eigensolver

Application

Memory Required(High Medium Low)

Disk Required (High Medium Low)

Subspace

To find few modes (up to about 40) of large models.
Recommended when the model consists of wellshaped
solid and shell elements. Works well if memory availability is limited.

L

H

Block
Lanczos

To find many modes (about 40+) of large models.
Recommended when the model consists of poorly
shaped solid and shell elements. This solver performs
well when the model consists of shells or a combination
of shells and solids. Works faster but requires about 50% more memory than subspace.

M

L

Power Dynamics

To find few modes (up to about 20) of large models.
Recommended for fast computation of eigenvalues of
over 100K DOF models. On coarse mesh models, the frequencies are approximate. Missed modes are possible when repeated frequencies are present.

H

L

Reduced

To find all modes of small to medium models (less than
10K DOF). Can be used to find few modes (up to about 40) of large models with proper selection of master DOF, but accuracy of frequencies depends on the master DOF selected.

L

L

When doing a modal analysis with a large number of constraint equations, use the subspace iterations method with the frontal solver instead of the JCG solver, or use the block Lanczos mode extraction method. Using the JCG solver when your analysis has many constraint equations could result in an internal element stiffness assembly that requires large amounts of memory.
The Block Lanczos method is especially powerful when searching for eigenfrequencies in a given part of the eigenvalue spectrum of a given system. The convergence rate of the eigenfrequencies will be about the same when extracting modes in the midrange and higher end of the spectrum as when extracting the lowest modes. Therefore, when you use a shift frequency (FREQB) to extract n modes beyond the starting value of FREQB, the algorithm extracts the n modes beyond FREQB at about the same speed as it extracts the lowest n modes.
The PowerDynamics method does not perform a Sturm sequence check (that is, does not check for missing modes), which might affect problems with multiple repeated frequencies. This method always uses lumped mass approximation.
NoteIf you use PowerDynamics to solve a model that includes rigid body modes, be sure to issue the RIGID command or choose one of its GUI equivalents (Main Menu>Solution>Analysis Options or Main Menu>Preprocessor> Loads>Analysis Options).
NoteThe eigenvalue results reported by ANSYS are actually divided by 2*. This gives the frequency in Hz (cycles/second). In other words:
Matrix reduction allows you to build a detailed model, as you would for a static stress analysis, and use only a "dynamic" portion of it for a dynamic analysis. You choose the "dynamic" portion by identifying key degrees of freedom, called master degrees of freedom, that characterize the dynamic behavior of the model. The ANSYS program then calculates reduced matrices and the reduced DOF solution in terms of the master DOF. You can then expand the solution to the full DOF set by performing an expansion pass. The main advantage of this procedure is the savings in CPU time to obtain the reduced solution, especially for dynamic analyses of large problems.
You can choose masters using M and MGEN commands, or you can have the program choose masters during solution using the TOTAL command. We recommend that you do both: choose a few masters yourself, and also have the ANSYS program choose masters. This way, the program can pick up any modes that you may have missed. The following list summarizes the guidelines for selecting master DOF:
The best way to check the validity of the master DOF set is to rerun the analysis with twice (or half) the number of masters and to compare the results. Another way is to review the reduced mass distribution printed during a modal solution. The reduced mass should be, at least in the dominant direction of motion, within 1015 percent of the total mass of the structure.
For meshes with uniform element sizes and properties (for example, a flat plate), the distribution of masters will, in general, not be uniform. In such cases, you should specify some master DOF of your own [M, MGEN]. The same recommendation applies to structures with an irregular mass distribution, where the programselected master DOF may be concentrated in the highermass regions.