Eigenvalue buckling analysis generally yields unconservative results and should not be used for design of actual structures. If you decide that eigenvalue buckling analysis is appropriate for your application, follow this process:
Only linear behavior is valid. Nonlinear elements, if any, are treated as linear. If you include contact elements, for example, their stiffnesses are calculated based on their initial status and are never changed. The program assumes that the initial status of the contact elements is the status at the completion of the static prestress analysis.
Young's modulus (EX) (or stiffness in some form) must be defined. Material properties can be linear, isotropic or orthotropic, and constant or temperature-dependent. Do not use rate-dependent material behavior. Other nonlinear properties, if any, are ignored.
For more information about building the model, see Building the Model in the Basic Analysis Guide and the Modeling and Meshing Guide.
The procedure to obtain a static solution is the same as described in Structural Static Analysis, with the following exceptions:
Prestress effects (PSTRES) must be activated. Eigenvalue buckling analysis requires the stress stiffness matrix to be calculated.
Unit loads are usually sufficient (that is, actual load values need not be specified). The eigenvalues calculated by the buckling analysis represent buckling load factors. Therefore, if a unit load is specified, the load factors represent the buckling loads. All loads are scaled. (Also, the maximum permissible eigenvalue is 1,000,000 - you must use larger applied loads if your eigenvalue exceeds this limit.)
It is possible that different buckling loads may be predicted from seemingly equivalent pressure and force loads in a eigenvalue buckling analysis. The difference can be attributed to the fact that pressure is considered as a "follower" load. The force on the surface depends on the prescribed pressure magnitude and also on the surface orientation. Forces are not considered as follower loads. As with any numerical analysis, it is recommended to use the type of loading which best models the in-service component. See Pressure Load Stiffness of the Mechanical APDL Theory Reference for more details.
Note that eigenvalues represent scaling factors for all loads. If certain loads are constant (for example, self-weight gravity loads) while other loads are variable (for example, externally applied loads), you need to ensure that the stress stiffness matrix from the constant loads is not factored by the eigenvalue solution.
One strategy that you can use to achieve this end is to iterate on the eigensolution, adjusting the variable loads until the eigenvalue becomes 1.0 (or nearly 1.0, within some convergence tolerance).
Consider, for example, a pole having a self-weight W0, which supports an externally-applied load, A. To determine the limiting value of A in an eigenvalue buckling solution, you could solve repetitively, using different values of A, until by iteration you find an eigenvalue acceptably close to 1.0.
You can apply a nonzero constraint in the prestressing pass as the static load. The eigenvalues found in the buckling solution will be the load factors applied to these nonzero constraint values. However, the mode shapes will have a zero value at these degrees of freedom (and not the nonzero value specified).
At the end of the solution, leave SOLUTION (FINISH).
This step requires files Jobname.emat (if created) and Jobname.esav from the static analysis. Also, the database must contain the model data (issue RESUME if necessary). Follow the steps below to obtain the eigenvalue buckling solution.
Enter the solution processor (/SOLU).
Specify the analysis type (ANTYPE).
Note: Restarts are not valid in an eigenvalue buckling analysis.
Note: When you specify an eigenvalue buckling analysis, a menu that is appropriate for buckling analyses appears. The menu will be either "abridged" or "unabridged", depending on the actions you took prior to this step in your session. The abridged menu contains only those solution options that are valid and/or recommended for buckling analyses. If you are on the abridged menu and you want to access other solution options (that is, solution options that are valid for you to use, but their use may not be encouraged for this type of analysis), select the option from the menu. For details, see Using Abridged Solution Menus in the Basic Analysis Guide.
Specify analysis options (BUCOPT,
Method,NMODE,SHIFT,LDMULTE,RangeKey):For
Method, specify the eigenvalue extraction method. The methods available for buckling are Block Lanczos and Subspace Iteration. Both methods use the full system matrices. See Eigenvalue and Eigenvector Extraction in the Theory Reference for more information on these two methods.For
NMODE, specify the number of buckling modes (that is, eigenvalues or load multipliers) to be extracted. This argument defaults to one, which is usually sufficient for eigenvalue buckling. We recommend that you request an additional few modes beyond what is needed in order to enhance the accuracy of the final solution.For
SHIFT, specify the initial shift point about which the buckling modes are calculated (defaults to 0.0). WhenRangeKeyis set to RANGE,SHIFTis the lower end of the load multiplier range of interest. Modifying the shift point can be helpful when numerical problems are encountered.For
LDMULTE, specify the boundary of the load multiplier range of interest (defaults to
). When RangeKeyis set to CENTER,LDMULTEis used to determine the lower and upper ends of the load multiplier range of interest. WhenRangeKeyis set to RANGE, theLDMULTEvalue is the upper end of the load multiplier range of interest.For
RangeKey, specify either CENTER or RANGE. WhenRangeKey= CENTER, the program computesNMODEbuckling modes centered aroundSHIFTin the range of (-LDMULTE, +LDMULTE). WhenRangeKey= RANGE, the program computesNMODEbuckling modes in the range of (SHIFT,LDMULTE).
Specify expansion pass options (MXPAND,
NMODE,,,Elcalc):For
NMODE, specify the number of modes to expand. This argument defaults to the total number of modes that were extracted.For
Elcalc, indicate whether you want Mechanical APDL to calculate stresses. "Stresses" in an eigenvalue analysis do not represent actual stresses, but give you an idea of the relative stress or force distribution for each mode. By default, no stresses are calculated.
Specify load step options.
The only load step options valid for eigenvalue buckling are output controls: database (OUTRES) and results file output (OUTPR,NSOL,ALL).
Save a backup copy of the database to a named file (SAVE).
Start solution calculations (SOLVE).
The output from the solution mainly consists of the eigenvalues, which are printed as part of the printed output (Jobname.out). The eigenvalues represent the buckling load factors; if unit loads were applied in the static analysis, they are the buckling loads. No buckling mode shapes are written to the database or the results file, so you cannot postprocess the results yet. To do this, you need to expand the solution (explained next).
Sometimes you may see both positive and negative eigenvalues calculated. Negative eigenvalues indicate that buckling occurs when the loads are applied in an opposite sense. This statement applies to linear buckling only, and is not the case for a linear perturbation buckling analysis. For linear perturbation buckling analysis, the buckling loads follow Equation 15–260 in the theoretical discussion (see Eigenvalue Buckling Analysis Based on Linear Perturbation in the Theory Reference).
Exit the SOLUTION processor (FINISH).
Results from a buckling expansion pass are written to the structural results file, Jobname.rst. They consist of buckling load factors, buckling mode shapes, and relative stress distributions. You can review them in POST1, the general postprocessor.
Note: To review results in POST1, the database must contain the same model for which the buckling solution was calculated (issue RESUME if necessary). Also, the results file (Jobname.rst) from the expansion pass must be available.
See the Command Reference for a discussion of the ANTYPE, PSTRES, D, F, SF, BUCOPT, EXPASS, MXPAND, OUTRES, SET, PLDISP, and PLNSOL commands.