3.4. Applying Loads and Obtaining the Solution

In this step, you define the analysis type and options, apply loads, specify load step options, and begin the finite element solution for the natural frequencies, as follows:

3.4.1. Enter the Solution Processor

  1. Enter the solution processor.

    Command(s): /SOLU
    GUI: Main Menu> Solution

3.4.2. Define Analysis Type and Options

After you have entered the solution processor, you define the analysis type and analysis options. Mechanical APDL offers the options listed in Table 3.1: Analysis Types and Options for a modal analysis. Each of the options is explained in detail below.

Table 3.1:  Analysis Types and Options

Option Command GUI Path
New Analysis ANTYPE Main Menu> Solution> Analysis Type> New Analysis
Analysis Type: Modal (see Note below) ANTYPE Main Menu> Solution> Analysis Type> New Analysis> Modal
Mode-extraction Method MODOPT Main Menu> Solution> Analysis Type> Analysis Options
Number of Modes to Extract MODOPT Main Menu> Solution> Analysis Type> Analysis Options
Number of Modes to Expand (see Note below) MXPAND Main Menu> Solution> Analysis Type> Analysis Options
Mass Matrix Formulation LUMPM Main Menu> Solution> Analysis Type> Analysis Options
Prestress Effects Calculation PSTRES Main Menu> Solution> Analysis Type> Analysis Options
Control Output to the Results File OUTRES Main Menu> Solution> Load Step Opts > Output Ctrls > DB/Results Files
Residual Vector Calculation RESVEC This command cannot be accessed from a menu.

When you specify a modal analysis, a Solution menu that is appropriate for modal analyses appears. The Solution menu is either “abridged” or “unabridged,” depending on the actions you took prior to this step in the current session. The abridged menu contains only those solution options that are valid and/or recommended for modal analyses. If you are on the abridged Solution menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the Unabridged Menu option. For details, see Using Abridged Solution Menus in the Basic Analysis Guide.

3.4.2.1. Option: New Analysis (ANTYPE)

Select New Analysis. If you wish to compute additional load vectors, residual vectors, or enforced motion terms subsequent to a prior modal analysis, select Restart.

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)

Select one of the following mode-extraction methods:

Mode-Extraction Method Comments
Block Lanczos

Used for large symmetric eigenvalue problems. This method uses the sparse matrix solver, overriding any solver specified via the EQSLV command.

PCG Lanczos

Used for very large symmetric eigenvalue problems (500,000+ degrees of freedom), and is especially useful to obtain a solution for the lowest modes to learn how the model will behave. This method uses the PCG iterative solver and therefore has the same limitations (that is, it does not support superelements, Lagrange multiplier option on contact elements, mixed u-P formulation elements, etc.).

This method works with the various Lev_Diff values on the PCGOPT command. It also works with MSAVE to reduce memory usage.

By default, this method does not perform a Sturm sequence check; however, internal heuristics have been developed to guard against missing modes. If a Sturm sequence check is absolutely necessary, it can be activated via the PCGOPT command.

Supernode

Used to solve for many modes (up to 10,000) in one solution. Typically, the reason for seeking many modes is to perform a subsequent mode-superposition or PSD analysis to solve for the response in a higher frequency range.

This method typically offers faster solution times than Block Lanczos if the number of modes requested is more than 200. The accuracy of the solution can be controlled via the SNOPTION command.

Subspace

Used for large symmetric eigenvalue problems.

This method uses the sparse matrix solver. The advantage of the Subspace method over the Block Lanczos method is that both [K] and [S] / [M] matrices can be indefinite at the same time. Some options can be controlled via the SUBOPT command.

Unsymmetric

Used for problems with unsymmetric matrices, such as fluid-structure interaction problems or brake squeal problems.

Damped

Used for problems where damping cannot be ignored, such as bearing problems.

QR damped

Faster and achieves better calculation efficiency than the damped method. It uses the reduced modal damped matrix to calculate complex damped frequencies in modal coordinates.

For more detailed information, see Comparing Mode-Extraction Methods.

For most applications, you will use the Block Lanczos, PCG Lanczos, Subspace, or Supernode method. The unsymmetric, damped, and QR damped methods are applicable in special applications. (The damped, unsymmetric, and QR damped methods may not be available, depending upon the Mechanical APDL license in use at your site.)

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

3.4.2.4. Option: Number of Modes to Extract (MODOPT)

This option is required for all mode-extraction methods.

If groups of repeated frequencies are present, make sure you extract all the solutions in each group. For more information, see Repeated Eigenvalues in the Mechanical APDL Theory Reference.

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)

The MXPAND command specifies which extracted modes to expand (i.e., which extracted modes to write to the results file) and how to compute element quantities (e.g., stress, strains, forces, energies, etc.) for subsequent postprocessing or for downstream mode-superposition analyses (e.g., spectrum, PSD, transient, or harmonic).

You can specify the following methods of mode expansion using the MXPAND command:

  • Input the number of modes to expand (NMODE).

  • Select the modes using a table (input using NMODE).

  • Select the modes based on their modal mass or mode coefficient (input as ModeSelMethod). Refer to Using Mode Selection for more information.

  • Specify a frequency range to extract (FREQB, FREQE).

In a mode-superposition analysis, the DOF results can either be combined in the expansion pass and the element results calculated from the combined DOF solution, or the stresses can be combined directly during the expansion pass to reduce computation time. This behavior is controlled by MSUPkey at the modal analysis level.

If MSUPkey is set to YES (MXPAND,ALL,,,YES,,YES), the element results are written to the mode file and then directly combined during the expansion pass.  This option is the default setting. It will reduce the computation time, but it has the following limitations for the downstream mode-superposition analyses:

  • Equivalent strains are evaluated using EFFNU=0.0. Use AVPRIN to set to the appropriate Poisson's ratio value.

  • Thermal loads are not supported.

  • NMISC results are not available.

  • Superelements are not supported (Mechanical APDL automatically sets MSUPkey to NO).

  • To include the damping and inertia contributions for reactions in a harmonic or transient analysis, the element nodal loads must be output (OUTRES,NLOAD,ALL). Otherwise the reactions will only reflect the static contributions.

  • The damping element forces and reaction forces are not available in a mode-superposition harmonic analysis based on QRDAMP eigensolver.

  • Strains and stresses of PIPE elements are not supported when pressure load is applied.

  • Inertia forces and kinetic energies are not available when enforced motion is present (DVAL)

  • Damping forces correspond to the damping settings of the last load step.

If MSUPkey is set to NO (MXPAND,ALL,,,YES,,NO), the element results are not written to the mode file. For subsequent downstream mode-superposition analysis, the DOF results are combined in the expansion pass and the element results are calculated from the combined DOF results. This option is used to obtain the NMISC results, or it can be used to compute thermal loads in the modal analysis for use in a subsequent mode-superposition harmonic or transient analysis. This option cannot be used to obtain the damping forces based on modal damping ratios (MDAMP, DMPRAT)

3.4.2.6. Option: Results File Output (OUTRES)

Use OUTRES to expand only items of interest and in the areas of interest to limit the size of the results file Jobname.RST. Note that for subsequent mode-superposition analyses (e.g., spectrum, PSD, transient, or harmonic), you should use OUTRES during the modal analysis to control their output as well.


Note:  The FREQ field on OUTRES (and OUTPR) can only be ALL or NONE, meaning the data can be requested for all modes or no modes. For instance, you cannot write information for every other mode.


3.4.2.7. 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.

3.4.2.8. 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 Performing a Prestressed Modal Analysis from a Linear Base 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.

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

3.4.2.9. Option: Residual Vector Calculation (RESVEC)

Use this option to include the contribution of higher frequency modes in a subsequent mode-superposition analysis. If rigid body modes are present, you must define pseudo-constraints using the D command with Value=SUPPORT. Only the minimum number of constraints must be specified. Those constraints will only be considered for the residual vector calculation.

3.4.2.10. 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: FREQB, FREQE, PRMODE, Nrmkey. Refer to the MODOPT command description for the meaning of these fields.

3.4.3. Apply Loads

In a modal analysis, the only "loads" that affect the solution are displacement constraints. If you input a nonzero displacement constraint, the program assigns a zero-value constraint to that degree of freedom instead. For directions in which no constraints are specified, the program calculates rigid-body (zero-frequency) as well as higher (nonzero frequency) free body modes. Table 3.2: Loads Applicable in a Modal Analysis 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 Loading in the Basic Analysis Guide.

If you are going to perform a downstream harmonic or transient mode-superposition analysis, you can apply other load types as well (see Generating and Using Multiple Loads in Mode-Superposition Analyses).


Note:  Loads specified using tabular boundary conditions with TIME as the primary variable (see the *DIM command) will have the table value at TIME equal to zero.


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> Define Loads> Apply> Structural> Displacement

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

3.4.3.1. Applying Loads Using Commands

Table 3.3: Load Commands for a Modal Analysis 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
DisplacementSolid ModelKeypoints DK DKDELE DKLIST DTRAN -
Solid ModelLines DL DLDELE DLLIST DTRAN -
Solid ModelAreas DA DADELE DALIST DTRAN -
Finite ElemNodes D DDELE DLIST DSCALE DSYM, DCUM

3.4.3.2. Applying Loads Using the GUI

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

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

GUI:

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

3.4.3.3. Listing Loads

To list existing loads, follow this GUI path:

GUI:

Utility Menu> List>Loads> load type

3.4.4. Specify Load Step Options

The only load step options available for a modal analysis are damping options.

Table 3.4:  Load Step Options (Damping)

Option Command
Global Alpha (mass) Damping ALPHAD
Global Beta (stiffness) Damping BETAD
Material-Dependent Alpha (mass) Damping MP,ALPD or TB,SDAMP,,,,ALPD
Material-Dependent Beta (stiffness) Damping MP,BETD or TB,SDAMP,,,,BETD
Element Damping (applied via element real constant or material tables) R, TB

Constant Structural Damping Ratio

DMPSTR
Material-Dependent Constant Structural Damping Ratio MP,DMPR

Damped and QR damped mode-extraction methods support all types of damping. UNSYM only supports structural damping.

Damping is ignored for the other mode-extraction methods.

If you include damping and specify the damped mode-extraction method, the calculated eigenvalues and eigenvectors are complex. If you include damping and specify the QR damped mode-extraction method, the eigenvalues are complex, but the eigenvectors can be real or complex (Cpxmod on the MODOPT command). The real eigenvectors are used for the mode-superposition analysis. See Comparing Mode-Extraction Methods for details.

For more information about different forms of damping, see Damping.

Damping specified in a non-damped modal analysis Damping (MP,DMPR) can be specified in a non-damped modal analysis if a spectrum or mode-superposition 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 in the subsequent analysis; see the Mechanical APDL Theory Reference.

3.4.5. Solve

Before you solve, save (SAVE) a backup copy of the database to a named file. You can then retrieve your model by reentering the program and issuing RESUME.

Now start the solution calculations.

Command(s): SOLVE
GUI: Main Menu> Solution> Solve> Current LS

3.4.5.1. Output

The output from the solution consists mainly of the natural frequencies, which are printed as part of the printed output (Jobname.OUT) and also written to the mode shape file (Jobname.MODE). The printed output may include mode shapes and the participation factor table, depending on your analysis options and output controls. Element results are written to the results file (Jobname.RST) using the MXPAND command. If the MXPAND command is not issued, the element results are not written by default and they cannot be post-processed.

3.4.6. Participation Factor Table Output

The participation factor table lists participation factors, mode coefficients, and mass distribution percentages for each mode extracted. The participation factors and mode coefficients are calculated based on an assumed unit displacement spectrum in each of the global Cartesian directions and rotation about each of these axes. The mass distribution is also listed.

The total mass used to calculate the ratio of effective mass to total mass is the mass output in the mass summary. Only the precise mass summary (used for 3-D models) accurately calculates the total rigid body mass and thus the directional masses. For more information, see Mass Related Information in the Mechanical APDL Theory Reference.

If you want to include the effect of boundary conditions and CP/CE in the calculation of the total mass, you can use APDL Math. For an example, see Example 4.9: Calculate the Participation Factors and Total Rigid Body Mass in the ANSYS Parametric Design Language Guide.

Rotational participation factors will be calculated when a real eigensolver mode-extraction method (such as Block Lanczos, PCG Lanczos, Supernode, or Subspace) is used.

For rotational DOFs, the participation factor table output shows the ratios of effective mass to total mass only when the precise mass summary is calculated.


Note:  The modal effective mass is equal to the participation factor squared. For a list of exceptions, see Effective Mass and Cumulative Mass Fraction in the Mechanical APDL Theory Reference.


Retrieving a participation factor or mode coefficient You can retrieve a participation factor or mode coefficient by issuing a *GET command (Entity=MODE).

3.4.7. Exit the Solution Processor

You must now exit the solution processor.

Command(s): FINISH
GUI: Main Menu> Finish

Release 18.2 - © ANSYS, Inc. All rights reserved.