Buckling Analysis of a rectangular plate
Buckling Analysis of a rectangular plate
(OP)
Hi guys,
I hope you can help with this problem. I have modeled a thin rectangular plate(Kirchhoff plate)and chosen S4R5 shell elements for my mesh. I did a linear perturbation and the simply-supported plate which gives me the correct eigenvalue and eigenshapes comparing with analytical results. Also, I ran a static general analysis under a distributed transverse load and bending stresses and deflection obey thin plate theory analytical results (Kirchoff). So, I am confident that my model boundary conditions and everything else is well modeled. Now, the key part is that I want to do a buckling analysis in order to obtain the Load-P vs maximum deflection-u (this graph will give me essentially the critical load)which I guess should be the first eigenvalue(lowest Ncr, compressive load). What type of analysis should I do in order to obtain this graph because linear perturbation does calculate load or displacements. Thank you
I hope you can help with this problem. I have modeled a thin rectangular plate(Kirchhoff plate)and chosen S4R5 shell elements for my mesh. I did a linear perturbation and the simply-supported plate which gives me the correct eigenvalue and eigenshapes comparing with analytical results. Also, I ran a static general analysis under a distributed transverse load and bending stresses and deflection obey thin plate theory analytical results (Kirchoff). So, I am confident that my model boundary conditions and everything else is well modeled. Now, the key part is that I want to do a buckling analysis in order to obtain the Load-P vs maximum deflection-u (this graph will give me essentially the critical load)which I guess should be the first eigenvalue(lowest Ncr, compressive load). What type of analysis should I do in order to obtain this graph because linear perturbation does calculate load or displacements. Thank you





RE: Buckling Analysis of a rectangular plate
RE: Buckling Analysis of a rectangular plate
Also, we've had some success using explicit dynamic analysis, with a slowly increasing load, to predict buckling through post-buckling behavior, although I'm sure that's not the most efficient way to go about it.
RE: Buckling Analysis of a rectangular plate
RE: Buckling Analysis of a rectangular plate
RE: Buckling Analysis of a rectangular plate
Selection of the step time does require a little consideration. (Apologies if you know this already, perhaps someone else will have the same question at some point). You need to balance two factors:
1) Select a step time that is too short, and the load will be applied so quickly that dynamic effects will dominate the solution; the load must be applied quasi-statically.I think 1/3 the first natural frequency is generally considered the cutoff for what counts as "quasi-static."
2) Select a step time that is too long, and the problem will take forever to solve.
If you have a small model, the second factor doesn't matter too much. To check the critical time increment of your mesh, go to the "mesh" module, select "Verify Mesh," from the toolbar, go to the "Size Metrics" tab, and check the "stable time increment" box. Make sure the part is already meshed with elements intended for use in explicit, and you'll get some time increment stats. Between that information and some trial-and-error with the solve time, you should be able to work out an appropriate step time to use for the problem.
Finally, I'd recommend using the same model with the same imperfection that worked for Riks. I don't think Explicit "theoretically" requires an initial imperfection to integrate the solution forward, but I suspect that you'd get an unintended buckling path if the Riks method needed an imperfection for the same problem. Good luck!
RE: Buckling Analysis of a rectangular plate
*IMPERFECTION, FILE=Job-0_Initial_Imperfection, STEP=1
1,1
** STEP: Step-2
**
*Step, name=Step-2, nlgeom=YES
*Dynamic, Explicit
, 10.
etc
etc
etc
Also when I ran the Job-0_Initial_Imperfection, which is a static analysis to deflect the plate laterally up to U3=0.1 mm (initial imperfection) at the middle. And the keyword was modified as followed in order to save the displacements (or should I save them in another way)? Should i see a file in the Directory where the U displacements are saved?
*NODE FILE
U
*End Step
However, when I ran the dynamic explicit analysis (job) my results do not reflect the imperfection I am trying to transfer from Job-0_Initial_Imperfection where the U should have been saved. Thank you for the help