pass and the element results are calculated from the combined DOF results. This option is used to obtain
the energies or 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.
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.
NoteThe 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 ap-
proximation. 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 (p. 49). 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 superpos-
ition 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-
Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential informationModal Analysis