Mechanical APDL Structural Analysis Guide

program at which time points the necessary data is to be saved for the multiframe restart. Only the
converged substeps of the load step are saved for a multiframe restart, thereby automatically guaran-
teeing that a valid restarting point is used for the linear perturbation analysis.

The following files must be saved from the base analysis for use in the restart performed as the first
phase of the linear perturbation procedure:

Jobname.RDB - ANSYS database file

Jobname.LDHI - Load history file

Jobname.Rnnn - Element saved records (restart files)

For more information on these files and the multiframe restart procedure, see Restarting an Analysis in
the Basic Analysis Guide

9.2.3. First Phase of the Linear Perturbation Analysis

The purpose for the first phase in the linear perturbation analysis procedure is to regenerate the solution
snapshot from the base analysis. Normally, this phase only requires the following command input:

/SOLU

ANTYPE,,RESTART,loadstep,substep,PERTURB

....! (other limited commands are allowed)

PERTURB,MODAL! can be STATIC, MODAL, BUCKLE, or HARMONIC (full harmonic)

SOLVE,ELFORM

! (do not exit solution module yet; do not issue FINISH command)

Upon execution of the SOLVE,ELFORM command, the program restarts the base analysis and regenerates

i

 T





 material data needed for the subsequent perturbation analysis and other possible solution

matrices. Then, by default, the program removes all external loads inherited from the base analysis,
except for displacement boundary conditions, inertia loads, and all non-mechanical loads (including
thermal loads).

Since this phase is strictly used to regenerate solution matrices from the base analysis, no other actions
(commands) are needed in most cases. The following items can be modified, however, so that the final
solution matrices used in the linear perturbation analysis can serve various purposes for the engineering
analysis:

• Change contact status via the PERTURB or CNKMOD command.


• To perform a partial nonlinear prestressed modal analysis for brake squeal simulation, issue the CMROTATE
  command.


• Modify element real constants (RMODIF).


• Modify material properties (TBMODIF or MP command); for example, to change the contact friction
  coefficient.


• Material behavior can be controlled via the PERTURB command. (For more information, see Material
  Properties of Structural Elements in Linear Perturbation in the Element Reference.)


• To include Coriolis effects in the modal analysis when the base analysis is static, issue the CORIOLIS
  command.

Other commands that are allowed in this phase of the linear perturbation analysis are:MP,EALIVE,
EKILL, and ESTIF.

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

Linear Perturbation Analysis