Buckling Analysis of a rectangular plate

[joncardenas]

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

 

[joncardenas]

Sorry, on the last sentence should be: Linear perturbation does NOT calculate load or displacements only eigenvalue and eigenmode.

 

[JSDaniel]

This is what the Riks method (Static, Riks) is intended for. From your description, it sound like you have a snap-through buckling problem, which requires no special consideration. (If there is a potential for bifurcation, you have to take extra modeling steps and introduce an initial imperfection to the problem to dictate the buckling configuration).

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.

 

[joncardenas]

JSDaniel I ran a (static,riks) with lateral distributed load and compression force but the reaction force(Compressive force Ny) is larger than the Ncr given by the linear perturbation. Shouldn't this analysis be aborted when reaction force reaches Ncr for the first buckling load

 

[joncardenas]

JSDaniel I was able to figure out and I did an initial imperfection in the middle of the plate and ran a static, riks and was able to get a load displacement curve. Now I want to match up this using a dynamic explicit analysis. Can you please tell me how to put the compressive force(load control) or displacement/velocity (displacement control)using dynamic explicit Abaqus? Also, do i have to do a initial imperfection as risks analysis. Thank you

 

[JSDaniel]

Glad you got the Riks to work. To control the load vs. time in an explicit analysis, use the "amplitude" feature. If you are using Abaqus/CAE as your pre-processor, define a concentrated force as usual with some magnitude that exceeds the critical load. Then, assign it an amplitude which varies from 0 to 1. The "time" column of the amplitude should correspond to your step time for the explicit step. A linear variation should be fine for your purposes, so you'll just need 2 entries in the amplitude definition: (0,0) and (stepTime, 1).

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!

 

[joncardenas]

Yes, thanks for the information. Is it possible to use the *IMPERFECTION command to input imperfection into the dynamic explicit analysis as follow:


*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