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.

Use this option to specify a modal analysis.

Select one of the following mode-extraction methods:

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 Ansys, Inc. product license in use at your site.)

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

This option is required for all mode-extraction methods.

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

For the unsymmetric and damped methods, requesting a larger number of modes than necessary reduces the possibility of missed modes, but requires more solution time.

MXPAND specifies which extracted modes to expand (that is, which extracted modes to write to the results file) and how to calculate element quantities (stress, strains, forces, energies, etc.) for subsequent postprocessing or for downstream mode-superposition analyses (such as spectrum, PSD, transient, or harmonic analyses).

You can specify the following methods of mode expansion via MXPAND:

In a mode-superposition analysis, the degree-of-freedom results can either be combined in the expansion pass and the element results calculated from the combined degree-of-freedom 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= YES (MXPAND,ALL,,,YES,,YES), the element results are written to the mode file and then directly combined during the expansion pass. The expansion using this option reduces the requires solution time. This option is the default when all of the following conditions exist:

If MSUPkey= NO (MXPAND,ALL,,,YES,,NO), the element results are not written to the mode file. For subsequent downstream mode-superposition analysis, the degree-of-freedom results are combined in the expansion pass and the element results are calculated from the combined degree-of-freedom results. This option is used to obtain the NMISC results, or it can be used to calculate 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, DMPR on MP command)

Issue OUTRES to expand only items of interest and in the areas of interest to limit the size of the results file Jobname.rst. For subsequent mode-superposition analyses (spectrum, PSD, transient, or harmonic), issue OUTRES during the modal analysis to control their output as well.

Use this option to specify the default formulation (which is element-dependent) or lumped mass approximation. The default formulation is suitable for most applications; however, for some problems (such as those involving 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.

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.

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

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 MODOPT description for the meaning of the fields.

Table 3.3: Load Commands for a Modal Analysis lists all the commands you can use to apply loads in a modal analysis.

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:

To list existing loads, follow this GUI path:

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) via MXPAND. If MXPAND is not issued, the element results are not written by default and therefore cannot be postprocessed.