Mechanical APDL Structural Analysis Guide

The following example shows typical command input to accomplish these steps.

Example Input for Linear Perturbation Static Analysis

F,NODE,...! Add linear perturbation loads

TIME,...! End time

SOLVE

FINISH

In a linear perturbation static analysis, the strain/stress calculation is done within the time substeps as
it is in a standard static analysis.

Although a linear perturbation static analysis is a linear static analysis, these differences from a linear
static analysis should be noted:

• The linear perturbation static analysis treats the process as a one-step analysis. It internally enforces
  the command NSUBST,1,1,1 and ignores user-specified inputs entered via the NSUBST or DELTIM
  commands.


• If the base analysis is nonlinear and the tangent matrix becomes nearly singular (for example,
  reaching the nonlinear buckling point) or indefinite (for example, a plastic hinge) at the restart point,
  then a message concerning negative or small pivots may be printed out from the linear perturbation
  static analysis. This typically does not happen in a purely linear static analysis if the model is properly
  constrained. When this occurs in a linear perturbation analysis, it is your responsibility to verify the
  correctness of the solution.

9.2.4.2. Second Phase - Modal Analysis

As described in Figure 9.2: Flowchart of Linear Perturbation Modal Analysis (p. 289), the second phase
of a linear perturbation modal analysis consists of the following actions:

1. Apply linear perturbation loads to generat e {Fperturbed}. (Note that thermal loads can not be applied

in the second phase of a linear perturbation modal analysis. See Generating and Controlling Non-

mechanical Loads (p. 299) for more information.)

2. If the base analysis included NLGEOM,ON, update the nodal coordinates by using the total displace-
   ment from the base analysis (similar to the UPCOORD command, but executed automatically and
   internally in this phase). From this point on, the deformed mesh is used for calculating perturbation
   loads and for postprocessing results from the linear perturbation analysis.


3. Regenerate other needed matrices such as mass and damping matrices ([M] and [C]).


4. Perform the linear perturbation modal analysis.

User action is needed only for steps (1) and (4) shown above. The program performs steps (2) and (3)
automatically (see Modal Analysis Based on Linear Perturbation in the Mechanical APDL Theory Reference).

The following example shows typical command input to accomplish these steps.

Example Input for Linear Perturbation Modal Analysis

MODOPT,eigensolver,number_of_modes,

... (include commands to add or remove linear perturbation loads)
MXPAND,number_of_modes,
SOLVE
FINISH

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

Linear Perturbation Analysis