The following topics concerning adding prestress effect to a modal analysis are available:
Use a prestressed modal analysis to calculate the frequencies and mode shapes of a prestressed structure, such as a spinning turbine blade. This procedure is applicable only if the prior (base) analysis is a purely linear, small deflection solution.
If the prior static analysis includes large-deflection effects (NLGEOM,ON), use the linear perturbation procedure described in Performing a Prestressed Modal Analysis from a Large-Deflection Base Analysis. If the base analysis includes other nonlinearities, use the linear perturbation procedure as described in Linear Perturbation Analysis. (Note that the linear perturbation analysis procedure is also valid for cases where the base analysis is linear and, therefore, can be used instead of the prestressed modal analysis procedure described here.)
The procedure for performing a prestressed modal analysis from a linear base analysis is essentially the same as that of a standard modal analysis, except that you must first prestress the structure by performing a static analysis:
Build the model and obtain a static solution with prestress effects turned on (PSTRES,ON). The same lumped mass setting (LUMPM) used here must also be used in the later prestressed modal analysis. Structural Static Analysis describes the procedure to obtain a static solution. Use EMATWRITE,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.
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.
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.
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:
Perform a nonlinear static solution with the prestress load. Define the necessary restart files (RESCONTROL).
Restart the previous static solution from the desired load step and substep.
Issue PERTURB to define the analysis type, material behavior to be used, contact status (
ContKeyargument) and load values to be retained from the previous static solution (LoadControlargument).Modify the behavior of individual contact pairs, as needed, via CNKMOD.
Issue SOLVE,ELFORM to regenerate the matrices.
Issue MODOPT and MXPAND to specify the modal analysis option.
Issue SOLVE to perform the eigensolution.
Postprocess the results from the Jobname.rstp file.
Note: Verify the resulting frequencies when the model includes contact. If the accuracy of the eigensolution is of concern, you can either increase the contact stiffness or change the contact algorithm in the nonlinear static run (using the Lagrange multiplier method for standard contact or the MPC method for bonded contact).
For detailed information about the linear perturbation analysis procedure, see Linear Perturbation Analysis in the Structural Analysis Guide.