Mechanical leverages the power of linear perturbation technology for all pre-stress analyses performed within Mechanical. This includes pre-stress Modal analyses, Full Harmonic Response analysis using a Pre-Stressed Structural System analyses, as well as Eigenvalue Buckling analyses.
The following features are available that are based on this technology:
Large deflection static analysis followed by pre-stress modal analysis. Thus the static analysis can be linear or nonlinear including large deflection effects.
Note:If performing a pre-stress modal analysis, it is recommended that you always include large deflection effects to produce accurate results in the modal analysis.
Pre-stress results should always originate from the same version of the application as that of the modal solution.
Although the modal results (including displacements, stresses, and strains) will be correctly calculated in the modal analysis, the deformed shape picture inside Mechanical will be based on the initial geometry, not the deformed geometry from the static analysis. If you desire to see the mode shapes based on the deformed geometry, you can take the result file into Mechanical APDL.
True contact status as calculated at the time in the static analysis from which the eigen analysis is based.
Support for cyclic analysis.
Support for multiple result sets in the static analysis.
For a pre-stressed eigen analysis, you can insert a Commands object beneath the Pre-Stress initial conditions object. The commands in this object will be executed just before the first solve for the pre-stressed modal analysis.
Pressure Load Stiffness
If the static analysis has a pressure load applied "normal to" faces (3D) or edges (2-D), this could result in an additional stiffness contribution called the "pressure load stiffness" effect. This effect plays a significant role in follow-on Modal analyses, Eigenvalue Buckling analyses, and in Harmonic Response (Full) analyses, however, the effect can be more prominent in an Eigenvalue Buckling analysis.
Different buckling loads may be predicted from seemingly equivalent pressure and force loads in a buckling analysis because in the Mechanical application a force and a pressure are not treated the same. As with any numerical analysis, we recommend that you use the type of loading which best models the in-service component. For more information, see the Mechanical APDL Theory Reference, under Structures with Geometric Nonlinearities> Stress Stiffening> Pressure Load Stiffness.
Restarts from Multiple Result Sets
A property called Pre-Stress Define By is available in the Details view of the Pre-Stress object in the eigen analysis. It is set to Program Controlled by default which means that it uses the last solve point available in the parent static structural analysis as the basis for the eigen analysis. There are three more read only properties defined in the Details view of the Pre-Stress object – Reported Loadstep, Reported Substep and Reported Time which are set to Last, Last, and End Time or None Available by default depending on whether or not there are any restart points available in the parent static structural analysis. These read only properties show the actual load step, sub step and time used as the basis for the eigen analysis.
You can change Pre-Stress Define By to Load Step, and then another property called Pre-Stress Loadstep will appear in the Details view. Pre-Stress Loadstep gives you an option to start from any load step in the static structural analysis. If you use this property, then Mechanical will always pick the last substep available in that load step. You can see the actual reported substep and time as read only properties. The input value of load step should be less than or equal to the number of load steps in the parent static structural analysis. Loadstep 0 stands for the last load step available.
You can change Pre-Stress Define By to Time, and then another property called Pre-Stress Time will appear in the Details view. Pre-Stress Time gives you an option to start from any time in the static structural analysis. If there is no restart point available at the time of your input, then Mechanical will pick the closest restart point available in the static structural analysis. You can see the actual reported load step, sub step and time as read only properties. The input value of time should be non-negative and it should be less than the end time of parent static structural analysis. Time 0 stands for end time of the parent analysis. If there is no restart point available in the input loadstep and the number of restart points in the parent analysis is not equal to zero, then the following error message appears:
"There is no restart point available at the requested loadstep. Change the restart controls in the parent static structural analysis to use the requested loadstep."
Note: If you use Pre-Stress Time, then Mechanical will pick the closest restart point available. It may not be the last sub step of a load step; and if it is some intermediate substep in a load step, then the result may not be reproducible if you make any changes in the parent static structural analysis or you solve it again.
If there is no restart point available in the parent static structural analysis, then Reported Loadstep, Reported Substep and Reported Time are set to None Available regardless of the user input of Load Step/Time but these will be updated to correct values once the analysis is solved with the correct restart controls for the parent structural analysis.
Contact Status
You may choose contact status for the pre-stressed eigen analysis to be true contact status, force sticking, or force bonded. A property called Contact Status is available in the Details view of the Pre-Stress object in the eigen analysis. This property controls the CONTKEY field of the Mechanical APDL PERTURB command.
Use True Status (default): Uses the current contact status from the restart snapshot. If the previous run for parent static structural is nonlinear, then the nonlinear contact status at the point of restart is frozen and used throughout the linear perturbation analysis.
Force Sticking: Uses sticking contact stiffness for the frictional contact pairs, even when the status is sliding (that is, the no sliding status is allowed). This option only applies to contact pairs whose frictional coefficient is greater than zero.
Force Bonding: Uses bonded contact stiffness and status for contact pairs that are in the closed (sticking/sliding) state.