Mechanical APDL Structural Analysis Guide

Structural Static Analysis (p. 9) describes the procedure to obtain a static solution. Use EMAT-

WRITE,YES if you want to look at strain energies from the modal analysis.

This step can also be a transient analysis. If so, save the EMAT and ESAV files at the desired

time point.

2. Enter the solution processor once again and obtain the modal solution, also with prestress effects
   activated (reissue PSTRES,ON). Files Jobname.EMAT (if created) and Jobname.ESAV from the
   static analysis must be available.

If another analysis is performed between the static and prestressed modal analyses, it is necessary

to rerun the static analysis, or keep a copy of the EMAT file from the static analysis.

3. Expand the modes and review them in the postprocessor.

Keep in mind that if you specify nonlinear elements in the modal analysis, Mechanical APDL treats them
as linear. For example, if you include contact elements, their stiffnesses are calculated based on their
initial status and never change. For a prestressed modal analysis, the program assumes that the initial
status of the contact elements is the status at the completion of the static prestress analysis.

3.6.2. Performing a Prestressed Modal Analysis from a Large-Deflection Base Analysis

To calculate the frequencies and mode shapes of a deformed structure or a structure involving nonlinear
(sliding) contact, you can use the linear perturbation analysis procedure to perform a prestressed
modal analysis following a large-deflection (NLGEOM,ON) static analysis.

To obtain the modal solution of a deformed structure, follow these steps:

1. Perform a nonlinear static solution with the prestress load. Use the RESCONTROL command to
   define the necessary restart files.


2. Restart the previous static solution from the desired load step and substep.


3. Issue the PERTURB command to define the analysis type, material behavior to be used, contact
   status (ContKey = CURRENT, STICKING, or BONDED) and load values to be retained from the previous
   static solution (LoadControl = ALLKEEP, INERKEEP, PARKEEP, or NOKEEP).


4. Modify the behavior of individual contact pairs, as needed, using the CNKMOD command.


5. Issue the SOLVE,ELFORM command to regenerate the matrices.


6. Issue the MODOPT and MXPAND commands to specify the modal analysis option.


7. Issue the SOLVE command to perform the eigensolution.


8. Postprocess the results from the Jobname.RSTP file.

For detailed information about the linear perturbation analysis procedure, see Linear Perturbation
Analysis in the Structural Analysis Guide.

3.7. Modal Analysis Examples.

The following modal analysis example topics are available:

Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information

Modal Analysis