Mechanical APDL Structural Analysis Guide

It is important to understand which matrices are used in the linear perturbation analysis:

• If the base analysis is nonlinear, the consistent tangent matrix from the prior Newton-Raphson iterations
  is regenerated based on the material behavior specified by the PERTURB command and based on the
  current geometry configuration if large-deflection effects are included (NLGEOM,ON).


• If contact elements are present in the base analysis, the stiffness matrix includes the effects of contact
  based on the contact status (set via PERTURB or CNKMOD).


• If the base analysis is linear, the linear stiffness matrix plus the stress stiffening matrix is used (automatically
  included).


• The spin-softening or gyroscopic effect is also included in this matrix regeneration phase as long as this
  spin-softening or gyroscopic effect is included in the base analysis.

Other commands such as PSTRES,EMATWRITE,OMEGA, and CMOMEGA are not needed in this phase,
as they are accounted for automatically.

9.2.4. Second Phase of the Linear Perturbation Analysis

The second phase of a linear perturbation analysis is performed immediately following the SOLVE,ELFORM
command from the first phase without exiting the solution processor (/SOLU); this is in order to correctly
retain the snapshot of the restart status from the base analysis. Also, for the case of geometric nonlin-
earity, the nodal coordinates are updated automatically based on the restart point (you do not need
to issue the UPCOORD command).

The second phase of the linear perturbation analysis varies slightly depending on whether you are
performing a static, modal, eigenvalue buckling, or full harmonic analysis. Details for each type of linear
perturbation are discussed in the following sections.

9.2.4.1. Second Phase - Static Analysis

9.2.4.2. Second Phase - Modal Analysis

9.2.4.3. Second Phase - Eigenvalue Buckling Analysis

9.2.4.4. Second Phase - Harmonic Analysis

9.2.4.1. Second Phase - Static Analysis

As described in Figure 9.1: Flowchart of Linear Perturbation Static Analysis (p. 288), the second phase of
a linear perturbation static analysis consists of the following actions:

1. Apply linear perturbation loads to generat e {Fperturbed}. (Note that thermal loads can be applied in

the second phase of a linear perturbation static 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. Perform the linear perturbation static analysis to solve i

T

 { Perturbed}={Perturbed}.

User action is needed only for the steps (1) and (3) shown above. The program performs step (2) auto-
matically (see Static Analysis Based on Linear Perturbation in the Mechanical APDL Theory Reference).

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

General Procedure for Linear Perturbation Analysis