Chapter 3: Modal Analysis

Go to the Next Chapter
Go to the Previous Chapter
Go to the Table of Contents for This Manual
Go to the Guides Master Index

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


3.1 Definition of Modal Analysis

You use modal analysis to determine the vibration characteristics (natural frequencies and mode shapes) of a structure or a machine component while it is being designed. It also can be a starting point for another, more detailed, dynamic analysis, such as a transient dynamic analysis, a harmonic response analysis, or a spectrum analysis.

3.2 Uses for Modal Analysis

You use modal analysis to determine the natural frequencies and mode shapes of a structure. The natural frequencies and mode shapes are important parameters in the design of a structure for dynamic loading conditions. They are also required if you want to do a spectrum analysis or a mode superposition harmonic or transient analysis.

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.

3.3 Commands Used in a Modal Analysis

You use the same set of commands to build a model and perform a modal analysis that you use to do any other type of finite element analysis. Likewise, you choose similar options from the graphical user interface (GUI) to build and solve models, no matter what type of analysis you are doing.

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.

3.4 Overview of Steps in a Modal Analysis

The procedure for a modal analysis consists of four main steps:

1. Build the model.

2. Apply loads and obtain the solution.

3. Expand the modes.

4. Review the results.

3.4.1 Build the Model

Specify the jobname and analysis title and then use PREP7 to define the element types, element real constants, material properties, and the model geometry. These tasks are common to most analyses. The ANSYS Modeling and Meshing Guide explains them in detail.

3.4.1.1 Points to Remember

3.4.2 Apply Loads and Obtain the Solution

Define the analysis type and options, apply loads, specify load step options, and begin the finite element solution for the natural frequencies. After the initial solution, you expand the mode shapes for review. Expanding the mode shapes is explained later in Section 3.4.3, "Expand the Modes."

1. Enter the ANSYS solution processor.

Command(s):

GUI:

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 3-1 Analysis types and analysis options

Option

Command

GUI Path

New Analysis

ANTYPE

Main Menu>Solution>-Analysis Type-New Analysis

Analysis Type: Modal

ANTYPE

Main Menu>Solution>-Analysis Type-New 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

Note-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).

3.4.2.1 Option: New Analysis [ANTYPE]

Choose New Analysis.

Note-Restarts 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).

3.4.2.2 Option: Analysis Type: Modal [ANTYPE]

Use this option to specify a modal analysis.

3.4.2.3 Option: Mode Extraction Method [MODOPT]

Choose one of the extraction methods listed below. (For more detailed information, see Section 3.11,"Mode Extraction Methods," later in this chapter.)

For most applications, you'll choose the subspace, reduced, Block Lanczos or the PowerDynamics method. The unsymmetric and damped methods are meant for special applications.

When you specify a mode extraction method, ANSYS automatically chooses the appropriate equation solver.

Note-The damped and unsymmetric methods are not available in the ANSYS/LinearPlus program.

3.4.2.4 Option: Number of Modes to Extract [MODOPT]

This option is required for all mode extraction methods except the reduced method.

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.

3.4.2.5 Option: Number of Modes to Expand [MXPAND]

This option is required for the reduced, unsymmetric, and damped methods only. However, if you want element results, you need to turn on the "Calculate elem results" option, regardless of the mode extraction method. 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).

3.4.2.6 Option: Mass Matrix Formulation [LUMPM]

Use this option to specify the default formulation (which is element-dependent) or lumped mass approximation. We recommend the default formulation for most applications. However, for some problems involving "skinny" structures such as slender beams or very thin shells, the lumped mass approximation often yields better results. Also, the lumped mass approximation can result in a shorter run time and lower memory requirements.

3.4.2.7 Option: Prestress Effects Calculation [PSTRES]

Use this option to calculate the modes of a prestressed structure. By default, no prestress effects are included; that is, the structure is assumed to be stress-free. To include prestress effects, element files from a previous static (or transient) analysis must be available; see Section 3.8, "Prestressed Modal Analysis." If prestress effects are turned on, the lumped mass setting [LUMPM] in this and subsequent solutions must be the same as it was in the prestress static analysis.

Note-You can use only axisymmetric loads for prestressing harmonic elements such as PLANE25 and SHELL61.

3.4.2.8 Additional Modal Analysis Options

After you complete the fields on the Modal Analysis Options dialog box, click OK. A dialog box specific to the selected extraction method appears. You see some combination of the following fields.

Field: FREQB, FREQE

Specify a frequency range for mode extraction. The FREQB field specifies the first shift point-the 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 rigid-body 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 3-6, 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.

Command(s):

GUI:

Main Menu>Solution>Master DOFs>-User Selected-Define

4. Apply loads on the model. The only "loads" valid in a typical modal analysis are zero-value displacement constraints. (If you input a non-zero displacement constraint, the program assigns a zero-value 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 rigid-body (zero-frequency) as well as higher (non-zero frequency) free body modes. Table 3-2 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 solid-model loads versus finite-element loads, see Chapter 2 of the ANSYS Basic Analysis Procedures Guide.

Note-Other loads-forces, 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 mode-superposition harmonic or transient analysis.

Table 3-2 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>-Loads-Apply> -Structural-Displacement

In an analysis, loads can be applied, removed, operated on, or listed.

Applying Loads Using Commands

Table 3-3 lists all the commands you can use to apply loads in a modal analysis.

Table 3-3 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

Applying Loads Using the GUI

All loading operations (except List; see below) are accessed through a series of cascading menus. From the Solution menu, you select the operation (apply, delete, etc.), then the load type (displacement, force, etc.), and then the object to which you are applying the load (keypoint, line, node, etc.).

For example, to apply a displacement load to a line, follow this GUI path:

GUI:

Main Menu>Solution>-Loads-Apply>-Structural-Displacement>On lines

3.4.2.9 Listing Loads

To list existing loads, follow this GUI path:

GUI:

Utility Menu>List>Loads>load type

5. Specify load step options. The following options are available for a modal analysis:

Table 3-4 Load step options

Option

Command

GUI Path

Damping (Dynamics) Options

Alpha (mass) Damping

ALPHAD

Main Menu>Solution>-Load Step Opts-Time/Frequenc> Damping

Beta (stiffness) Damping

BETAD

Main Menu>Solution>-Load Step Opts-Time/Frequenc> Damping

Constant Damping Ratio

DMPRAT

Main Menu>Solution>-Load Step Opts-Time/Frequenc> Damping

Material-Dependent Damping Ratio

MP,DAMP

Main Menu>Solution>-Load Step Opts-Other>Change Mat Props>-Temp Dependent-Polynomial

3.4.2.10 Damping (Dynamics Options)

Damping is valid only for the damped mode extraction method (and ignored for the other mode extraction methods; see Note below).

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.

Note-Damping can be specified in a non-damped modal analysis if a single-point 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.

3.4.2.11 Participation Factor Table Output

Note-You can retrieve a participation factor or mode coefficient by issuing a *GET command. The factor or coefficient is valid for the excitation (assumed unit displacement spectrum) directed along the last of the applicable coordinates (z direction for a 3-D analysis). To retrieve a participation factor or mode coefficient for another direction, perform a spectrum analysis with the excitation set (SED) to the desired direction. Follow with another *GET command.

6. Save a back-up copy of the database to a named file. You can then retrieve your model by re-entering the ANSYS program and issuing RESUME.

Command(s):

GUI:

Utility Menu>File>Save as

7. Start solution calculations.

Command(s):

GUI:

Main Menu>Solution>-Solve-Current LS

Output From Subspace Mode Extraction Method

If you use the subspace mode extraction method, you might see the following warning in the solution printout: "STURM number = n should be m," where n and m are integer numbers. This indicates that a mode has been missed, or that the mth and nth mode gave the same frequencies and only m modes were requested.

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):

GUI:

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):

GUI:

Main Menu>Solution>Analysis Options>Subspace

4. Click on OK to display the Subspace Modal Analysis dialog box.

5. Leave SOLUTION.

Command(s):

GUI:

Main Menu>Finish

3.4.3 Expand the Modes

In its strictest sense, the term "expansion" means expanding the reduced solution to the full DOF set. The "reduced solution" is usually in terms of master DOF. In a modal analysis, however, we use the term "expansion" to mean writing mode shapes to the results file. That is, "expanding the modes" applies not just to reduced mode shapes from the reduced mode extraction method, but to full mode shapes from the other mode extraction methods as well. Thus, if you want to review mode shapes in the postprocessor, you must expand them (that is, write them to the results file). Expanded modes are also required for subsequent spectrum analyses. 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). No expansion is necessary for subsequent mode superposition analyses.

3.4.3.1 Points to Remember

3.4.3.2 Expanding the Modes

1. Re-enter the ANSYS solution processor.

Command(s):

GUI:

Main Menu>Solution

Note-You must explicitly leave SOLUTION (using the FINISH command) and re-enter (/SOLUTION) before performing the expansion pass.

2. Activate the expansion pass and its options. ANSYS offers these options for the expansion pass:

Table 3-5 Expansion pass options

Option

Command

GUI Path

Expansion Pass On/Off

EXPASS

Main Menu>Solution>-Analysis Type-ExpansionPass

No. of Modes to Expand

MXPAND

Main Menu>Solution>-Load Step Opts-ExpansionPass>Expand Modes

Freq. Range for Expansion

MXPAND

Main Menu>Solution>-Load Step Opts-ExpansionPass>Expand Modes

Stress Calc. On/Off

MXPAND

Main Menu>Solution>-Load Step Opts-ExpansionPass>Expand Modes

3.4.3.3 Option: Expansion Pass On/Off [EXPASS]

Choose ON.

3.4.3.4 Option: Number of Modes to Expand [MXPAND, NMODE]

Specify the number. Remember that only expanded modes can be reviewed in the postprocessor. Default is no modes expanded.

3.4.3.5 Option: Frequency Range for Expansion [MXPAND, FREQB, FREQE]

This is another way to control the number of modes expanded. If you specify a frequency range, only modes within that range are expanded.

3.4.3.6 Option: Stress Calculations On/Off [MXPAND, Elcalc]

Choose ON only if you plan to do a subsequent spectrum analysis and are interested in stresses or forces to do the spectrum. "Stresses" from a modal analysis do not represent actual stresses in the structure, but give you an idea of the relative stress distributions for each mode. Default is no stresses calculated.

3. Specify load step options. The only options valid in a modal expansion pass are output controls:

Command(s):

GUI:

Main Menu>Solution>-Load Step Opts-Output Ctrls>Solu Printout

Command(s):

GUI:

Main Menu>Solution>-Load Step Opts-Output Ctrls>DB/Results File

4. Start expansion pass calculations.

Command(s):

GUI:

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):

GUI:

Close the Solution menu.

Note-The 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.

3.4.4 Review the Results

Results from a modal analysis (that is, the modal expansion pass) are written to the structural results file, Jobname.RST. Results consist of:

You can review these results in POST1 [/POST1], the general postprocessor. Some typical postprocessing operations for a modal analysis are described below. For a complete description of all postprocessing functions, see Chapter 4 in the ANSYS Basic Analysis Procedures Guide.

3.4.4.1 Points to Remember

3.4.4.2 Reviewing Results Data

1. Read in results data from the appropriate substep. Each mode is stored on the results file as a separate substep. If you expand six modes, for instance, your results file will have one load step consisting of six substeps.

Command(s):

GUI:

Main Menu>General Postproc>-Read Results-substep

2. Perform any desired POST1 operations. Typical modal analysis POST1 operations are explained below:

3.4.4.3 Option: Listing All Frequencies

You may want to list the frequencies of all modes expanded. A sample output from this command is shown 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         4
Command(s):

GUI:

Main Menu>General Postproc>List Results>Results Summary

3.4.4.4 Option: Display Deformed Shape

Command(s):

GUI:

Main Menu>General Postproc>Plot Results>Deformed Shape

3.4.4.5 Option: List Master DOF

Command(s):

GUI:

Main Menu>Solution>Master DOFs>List All

Note-To display the master DOFs graphically, plot the nodes (Utility Menu> Plot>Nodes or command NLIST).

3.4.4.6 Option: Line Element Results

Command(s):

GUI:

Main Menu>General Postproc>Element Table>Define Table

3.4.4.7 Option: Contour Displays

Command(s):

GUI:

Main Menu>General Postproc>Plot Results>-Contour Plot-Nodal Solu or Element Solu

Command(s):

GUI:

Main Menu>General Postproc>Element Table>Plot Element Table
Main Menu>General Postproc>Plot Results>-Contour Plot-Line 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.

3.4.4.8 Option: Tabular Listings

Command(s):

GUI:

Main Menu>General Postproc>List Results>solution option
Main Menu>General Postproc>List Results>-Sorted Listing-Sort Nodes
or Sort Elems

3.4.4.9 Other Capabilities

Many other postprocessing functions-mapping results onto a path, load case combinations, etc.-are available in POST1. See Chapter 5 of the ANSYS Basic Analysis Procedures Guide for details.

See the ANSYS Commands Reference for a discussion of the ANTYPE, MODOPT, M, TOTAL, EXPASS, MXPAND, SET, and PLDISP commands.

3.5 A Sample Modal Analysis (GUI Method)

In this example, you perform a modal analysis on the wing of a model plane to demonstrate the wing's modal degrees of freedom.

3.5.1 Problem Description

This is a modal analysis of a wing of a model plane. The wing is of uniform configuration along its length, and its cross-sectional area is defined to be a straight line and a spline, as shown. It is held fixed to the body on one end and hangs freely at the other. The objective of the problem is to demonstrate the wing's modal degrees of freedom.

3.5.2 Problem Specifications

The dimensions of the wing are shown in the problem sketch. The wing is made of low density polyethylene with the following values:

3.5.3 Problem Sketch

Figure 3-1 Diagram of a Model Airplane Wing

3.5.3.1 Specify the Title and Set Preferences

1. Choose menu path Utility Menu>File>Change Title.

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.

3.5.3.2 Define Element Types

1. Choose menu path Main Menu>Preprocessor>Element Type>Add/Edit/Delete. The Element Types dialog box appears.

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.

3.5.3.3 Define Material Properties

1. Choose menu path Main Menu>Preprocessor>Material Props> -Constant-Isotropic. The Isotropic Material Properties dialog box appears.

2. Click on OK to specify material number 1. A second dialog box appears.

3. Enter 3800 for EX.

4. Enter 1.033e-3 for DENS.

5. Enter .3 for NUYX.

6. Click on OK.

3.5.3.4 Create Keypoints at Given Locations

1. Choose menu path Main Menu>Preprocessor>-Modeling-Create> Keypoints>In Active CS. The Create Keypoints in Active Coordinate System dialog box appears.

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.

3.5.3.5 Create Lines and Splines between Keypoints

1. Choose menu path Main Menu>Preprocessor>-Modeling-Create> -Lines-Lines>Straight Line. The Create Straight Lines picking menu appears.

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>-Modeling-Create> -Lines-Splines> With options>Spline thru kps. The B-Spline picking menu appears.

6. Pick keypoints 2, 3, 4, 5 in that order and click on OK. The B-Spline 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.

3.5.3.6 Create Cross-Sectional Area

1. Choose menu path Main Menu>Preprocessor>-Modeling-Create> -Areas-Arbitrary>By lines. The Create Area by Lines picking menu appears.

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.

3.5.3.7 Define the Mesh Density and Mesh the Area

1. Choose menu path Main Menu>Preprocessor>-Meshing-Size Cntrls> -ManualSize--Global-Size. The Global Element Sizes dialog box appears.

2. Enter 0.25 for the element edge length.

3. Click on OK.

4. Choose menu path Main Menu>Preprocessor>-Meshing-Mesh> -Areas-Free. The Mesh Areas picking menu appears.

5. Click on Pick All. (If a warning box appears, click on Close. See Note below.)

Note-The 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.

3.5.3.8 Set the Number of Line Divisions

1. Choose menu path Main Menu>Preprocessor>-Meshing-Size Cntrls>-Manual Size--Global-Size. The Global Element Sizes dialog box appears.

2. Delete the element edge length.

3. Enter 10 for number of element divisions.

4. Click on OK.

3.5.3.9 Extrude the Meshed Area into a Meshed Volume

1. Choose menu path Main Menu>Preprocessor>-Attributes-Define> Default Attribs. The Meshing Attributes dialog box appears.

2. Enter 2 for element type number.

3. Click on OK.

4. Choose menu path Main Menu>Preprocessor>-Modeling-Operate> Extrude/Sweep>-Areas-By 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.)

8. Choose menu path Utility Menu>PlotCtrls>Pan,Zoom,Rotate.

9. Click on "Iso," then on Close.

10. Click on SAVE_DB on the ANSYS Toolbar.

3.5.3.10 Enter Solution and Specify Analysis Type and Options

1. Choose menu path Main Menu>Solution>-Analysis Type-New Analysis. The New Analysis dialog box appears.

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.

Note-If 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.

3.5.3.11 Deselect PLANE42 Elements

Unselect the PLANE42 elements used for the 2-D area mesh because they will not be used for the analysis.

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.

3.5.3.12 Apply Constraints to the Model

1. Choose menu path Utility Menu>Select>Entities. The Select Entities dialog box appears.

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>-Loads-Apply>-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.

3.5.3.13 Specify the Number of Modes to be Expanded and Solve

1. Choose menu path Main Menu>Solution>-Load Step Opts- ExpansionPass>Expand Modes. The Expand Modes dialog box appears.

2. Enter 5 for number of modes to expand.

3. Click on OK.

4. Choose menu path Main Menu>Solution>-Solve-Current 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.

3.5.3.14 List the Natural Frequencies

1. Choose menu path Main Menu>General Postproc>Results Summary. Review the information in the dialog box, and then close the dialog box using File>Close.

3.5.3.15 View the Five Modes

X11 Motif Systems Only

1. Choose menu path Main Menu>General Postproc>-Read Results-First Set.

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 Results-Next 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 6-9 for the remaining three modes.

Windows NT or Windows 95 Systems Only

1. Choose menu path Main Menu>General Postproc>-Read Results-First Set.

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 Results-Next 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 7-10 for the remaining three modes.

3.5.3.16 Exit ANSYS

1. Choose QUIT from the ANSYS Toolbar.

2. Choose Quit-No Save!

3. Click on OK.

3.6 A Sample Modal Analysis (Command or Batch Method)

You can perform the example modal analysis of a model airplane wing using the ANSYS commands shown below instead of GUI choices. Items prefaced with an exclamation point (!) are comments.

/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,1,1.033E-3
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 B-spline
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,.5E-1
SET,NEXT
PLDISP,0
ANMODE,10,.5E-1
SET,NEXT
PLDISP,0
ANMODE,10,.5E-1
SET,NEXT
PLDISP,0
ANMODE,10,.5E-1
SET,NEXT
PLDISP,0
ANMODE,10,.5E-1
FINISH
/EXIT

3.7 Where to Find Other Examples

Several ANSYS publications, particularly the ANSYS Verification Manual, describe additional modal analyses.

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 step-by-step 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:

3.8 Prestressed Modal Analysis

Use a prestressed modal analysis to calculate the frequencies and mode shapes of a prestressed structure, such as a spinning turbine blade. 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:

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. Re-enter 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.

3.9 Prestressed Modal Analysis of a Large Deflection Solution

You can also perform a prestressed modal analysis following a large deflection static analysis in order to calculate the frequencies and mode shapes of a highly deformed structure. Use the prestressed modal analysis procedure, except you use the PSOLVE command to obtain the modal solution instead of the SOLVE command, as shown in the sample input listing below. Also, you must use the UPCOORD command to update the coordinates to obtain the correct stresses.

! 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

3.10 Modal Analysis of a Cyclically Symmetric Structure

If a structure exhibits cyclic symmetry (for example, a fan wheel or a spur gear), you can calculate its frequencies and mode shapes by modeling just one sector of it. This feature, known as modal cyclic symmetry, can save a significant amount of your time as well as computer time. An added benefit to modeling just one sector is that you can view the mode shapes of the entire structure. Modal cyclic symmetry is available in the ANSYS/Multiphysics, ANSYS/Mechanical, and ANSYS/Structural products only.

3.10.1 The Basic Sector

The sector that is modeled is known as the basic sector. A proper basic sector represents a pattern that, if repeated n times in global cylindrical coordinate space, (CSYS=1), would yield the complete model (see Figure 3-2).

Figure 3-2 An example of a cyclically symmetric structure

3.10.2 Nodal Diameters

To understand the procedure for modal cyclic symmetry, you need to understand the concept of nodal diameters. (The word nodal here is used in the vibrational sense, not in the finite element sense.) The term "nodal diameter" is derived from the appearance of a simple geometry, like a disk, vibrating in a certain mode. Most mode shapes contain lines of zero out-of-plane displacement which cross the entire disk as shown below. These are commonly called nodal diameters.

Figure 3-3 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.)

3.10.3 Standard (Stress-free) Modal Cyclic Symmetry

The procedures for standard (stress-free) modal cyclic symmetry and prestressed modal cyclic symmetry are described next. Modal cyclic symmetry is available for structures with or without prestress.

Note-The procedure for modal cyclic symmetry uses two predefined ANSYS macros: CYCGEN and CYCSOL. Both assume a model with structural solid or shell elements.

3.10.3.1 Overview

The procedure for stress-free modal cyclic symmetry is outlined in the flow chart below, followed by a step-by-step description.

Figure 3-4 Procedure for modal cyclic symmetry (stress-free)



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).

Figure 3-5 Basic sector definition

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):

GUI:

Utility Menu>Select>Comp/Assembly>Create Component

3. Reactivate all entities.

Command(s):

GUI:

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 two-sector model. The macro copies internal couplings and constraint equations from the basic sector to the second sector.

Command(s):

GUI:

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):

GUI:

Main Menu>Solution >Analysis Type>Modal
Main Menu>Solution >Analysis Options>Block Lanczos

See Table 3-6 for a list of the CE methods that are available for the Block Lanczos eigensolver:

Table 3-6 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 100,000-DOF 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 100,000-DOF 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."

7. Run the CYCSOL macro and define your nodal diameter range and the sector angle as follows:

Command(s):

GUI:

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

8. Enter POSTPROCESSING and expand the model for display. Indicate the number of sectors that you want to expand.

Command(s):

GUI:

Main Menu>General Postprocessing>Expand sector

Note-The /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).

3.10.4 Prestressed Modal Cyclic Symmetry

The procedure for prestressed modal cyclic symmetry is outlined in the flow chart in Figure 3-6.

The steps involved are essentially the same as for the stress-free case, except that a static solution is required to calculate the prestress in the basic sector. Thus, steps 1-4 and 7 and 8 are the same as for the stress-free 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. Re-enter PREP7 and define modal analysis and its options, as explained for the stress-free case. Be sure to include prestress effects with the PSTRES command.

Note-Symmetry boundary conditions must be removed after the static solution is obtained.

Figure 3-6 Procedure for modal cyclic symmetry (prestressed)



3.11 Mode Extraction Methods

The basic equation solved in a typical undamped modal analysis is the classical eigenvalue problem:

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:

Note-The damped and unsymmetric methods are not available in the ANSYS/LinearPlus program.

The first four, the subspace, the Block Lanczos, the PowerDynamics, and the reduced methods are the most commonly used. Table 3-7 compares these four mode extraction methods. Following the table is a brief description of each of the six types of mode extraction methods.

Table 3-7 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 well-shaped 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

3.11.1 Subspace Method

The subspace method uses the subspace iteration technique, which internally uses the generalized Jacobi iteration algorithm. It is highly accurate because it uses the full [K] and [M] matrices. For the same reason, however, the subspace method is slower than the reduced method. This method is typically used in cases where high accuracy is required or where selecting master DOF is not practical.

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.

3.11.2 Block Lanczos Method

The Block Lanczos eigenvalue solver uses the Lanczos algorithm where the Lanczos recursion is performed with a block of vectors. This method is as accurate as the subspace method, but faster. The Block Lanczos method uses the sparse matrix solver, overriding any solver specified via the EQSLV command.

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.

3.11.3 PowerDynamics Method

The PowerDynamics method internally uses the subspace iterations, but uses the PCG iterative solver. This method may be significantly faster than either the subspace or the Block Lanczos methods, but may not converge if the model contains poorly-shaped elements, or if the matrix is ill-conditioned. This method is especially useful in very large models (100,000+ DOFs) to obtain a solution for the first few 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.

Note-If 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).

3.11.4 Reduced Method

The reduced method uses the HBI algorithm (Householder-Bisection-Inverse iteration) to calculate the eigenvalues and eigenvectors. It is relatively fast because it works with a small subset of degrees of freedom called master DOF. Using master DOF leads to an exact [K] matrix but an approximate [M] matrix (usually with some loss in mass). The accuracy of the results, therefore, depends on how well [M] is approximated, which in turn depends on the number and location of masters. Section 3.12,"Matrix Reduction," presents guidelines to select master DOFs.

3.11.5 Unsymmetric Method

The unsymmetric method, which also uses the full [K] and [M] matrices, is meant for problems where the stiffness and mass matrices are unsymmetric (for example, acoustic fluid-structure interaction problems). It uses the Lanczos algorithm which calculates complex eigenvalues and eigenvectors if the system is non-conservative (for example, a shaft mounted on bearings). The real part of the eigenvalue represents the natural frequency and the imaginary part is a measure of the stability of the system-a negative value means the system is stable, whereas a positive value means the system is unstable. Sturm sequence checking is not available for this method. Therefore, missed modes are a possibility at the higher end of the frequencies extracted.

3.11.6 Damped Method

The damped method is meant for problems where damping cannot be ignored, such as rotor dynamics applications. It uses full matrices ([K], [M], and the damping matrix [C]). It uses the Lanczos algorithm and calculates complex eigenvalues and eigenvectors (as described below). Sturm sequence checking is not available for this method. Therefore, missed modes are a possibility at the higher end of the frequencies extracted.

3.11.6.1 Damped Method-Real and Imaginary Parts of the Eigenvalue

The imaginary part of the eigenvalue, , represents the steady-state circular frequency of the system. The real part of the eigenvalue, , represents the stability of the system. If is less than zero, then the displacement amplitude will decay exponentially, in accordance with EXP(). If is greater than zero, then the amplitude will increase exponentially. (Or, in other words, negative gives an exponentially decreasing, or stable, response; and positive gives an exponentially increasing, or unstable, response.) If there is no damping, the real component of the eigenvalue will be zero.

Note-The eigenvalue results reported by ANSYS are actually divided by 2*. This gives the frequency in Hz (cycles/second). In other words:

3.11.6.2 Damped Method-Real and Imaginary Parts of the Eigenvector

In a damped system, the response at different nodes can be out of phase. At any given node, the amplitude will be the vector sum of the real and imaginary components of the eigenvector.

3.12 Matrix Reduction

Matrix reduction is a way to reduce the size of the matrices of a model and perform a quicker and cheaper analysis. It is mainly used in dynamic analyses such as modal, harmonic, and transient analyses. Matrix reduction is also used in substructure analyses to generate a superelement.

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.

3.12.1 Theoretical Basis of Matrix Reduction

The ANSYS program uses the Guyan Reduction procedure to calculate the reduced matrices. The key assumption in this procedure is that for the lower frequencies, inertia forces on the slave DOF (those DOF being reduced out) are negligible compared to elastic forces transmitted by the master DOF. Therefore, the total mass of the structure is apportioned among only the master DOF. The net result is that the reduced stiffness matrix is exact, whereas the reduced mass and damping matrices are approximate. For details about how the reduced matrices are calculated, refer to the ANSYS Theory Reference.

3.12.1.1 Guidelines for Selecting Master DOF

Choosing master DOF is an important step in a reduced analysis. The accuracy of the reduced mass matrix (and hence the accuracy of the solution) depends on the number and location of masters. For a given problem, you can choose many different sets of master DOF and will probably obtain acceptable results in all cases.

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:

Figure 3-7 (a) Possible out-of-plane masters for a flat plate
(b) Motion in X induces motion in Y

Figure 3-8 Choosing masters at locations with (a) large rotary inertia, (b) large mass

Figure 3-9 Choosing masters in an axisymmetric shell model

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 10-15 percent of the total mass of the structure.

3.12.1.2 A Note About Program-Selected Masters

If you let the ANSYS program select masters [TOTAL], the distribution of masters selected will depend on the order in which elements are processed during the solution. For example, different master DOF sets may be selected depending on whether the elements are processed from left to right or from right to left. However, this difference usually yields insignificant differences in the results.

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 program-selected master DOF may be concentrated in the higher-mass regions.


Go to the beginning of this chapter