Cancel
Showing results for 
Search instead for 
Did you mean: 

Plastic Buckling of Plate

Valued Contributor
Valued Contributor

Hi,

Thanks for this forum, I was able to resolve & obtain quite accurate results with SOL 106 Inelastic column buckling. Trying to move up the order, I was trying to repeat the inelastic buckling for a 2D plate.

 

I am having some issues and hopefully will get similar responses.

 

As usual, I chose a problem from Bruhn.

 

Bruhn Plate Problem DetailsBruhn Plate Problem Details

The expected critical buckling stress with plasticity correction factor is 32800 psi, which translates in to 9250 lbs.

 

I ran a SOL 105 and the buckling factor matches very closely with theoritical results. I applied the first deformation mode to nodes scaling them down by a factor of 0.01/0.001 (tried both values).

 

I applied a compressive load of 100,000 lbs and ran SOL 106 analysis. Images shows cards of various parameters.

 

Non-linear CardNon-linear CardNon-linear Material Card definitionNon-linear Material Card definition

FYI, I also tried using plastic hardening modulus. I also had a compressive stress-strain curve function plotted and tried to use it, but got errors in F06 file.

SOL 106 Case time output setSOL 106 Case time output set

My understanding is that the plate has buckled between a load of 11210 to 11250 lbs. The difference between FE & theoritical calc is 21%, which is hard to accept.

 

Non-linear Minor Prinicipal Stress OutputNon-linear Minor Prinicipal Stress Output

The above output is Nonlinear Minor Stress vector. The peak stress exceeds 44000 psi and lowest is 32856 psi which corresponds very well to theoritical hand calc.

 

Question is, how to improve the output with respect to critical buckling force Fcr? Any inputs if the above looks OK.

 

Thx,

 

PS: My new project has a very punishing schedule. So my responses may get delayed a little bit.

10 REPLIES

Re: Plastic Buckling of Plate

Legend
Legend

Hi,

 

Looking at the detalis that you are given:

- mesh size seems to be ok

- material defintion also. Compressive side is not necesssary for Von Mises criteria. At least in other solvers. It takes the same for tensile/compression as Von Mises is just an absolute value

- bulk data section: did you apply large displacement/strain?., sol 106 sutibale for plastic strains <10%

- element formulation: cquad4/cquad4R? kirchoff midlin?

 

I am not familar with theoretical soltuion so I do not know which assumtions are done

 

 

Re: Plastic Buckling of Plate

Valued Contributor
Valued Contributor

Draw a graph of the movement of the plane of the sheet points . on this schedule is easy to determine the moment of reaching the critical force

NL.png

Re: Plastic Buckling of Plate

Valued Contributor
Valued Contributor

Cfytr,

Did you try to replicate my (Bruhn's set up)? Were you able to achieve a result closer to theoritical prediction? Its hard for me make it out from your node (point) vs out of plane translation.

 

Jon Morga, I will try to provide some of the details you've asked on Friday, but I am pretty sure large disp (if not large strain) option was turned ON. 

 

My current project is brutal and I hardly get time to work on side projects. Sorry for the late reply. 

 

Also, thanks for taking time to reply. 

Re: Plastic Buckling of Plate

Siemens Phenom Siemens Phenom
Siemens Phenom

Looking at the results load factors in Femap is not accurate way to determine the initial nonlinear buckling load. The only thing you know for certain when looking at only the the load factors, is that Nastran created results for those load factors. They may not even be converged results, dependidng on your NLPARM settings.

 

You must inspect the f06 file and find the first load factor where the following message occurs:

*** USER WARNING MESSAGE 4698 (DCMPD)
STATISTICS FOR DECOMPOSITION OF MATRIX KLLRH .
THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN
1.00000E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL.

 

This message indicates that mathmetically your problem has started to encounter stability issues. Your model might continue to carry more load after this point, but then the questions one of what is your criteria for considering the structure as failed.

 

Plotting the displacement vs load factor is also a valid approach, however the question then also becomes choosing the criteria or change in slope that indicates a failure.

 

Hope this helps.

 

Joe

 

 

Re: Plastic Buckling of Plate

Siemens Phenom Siemens Phenom
Siemens Phenom

I believe if you make the following adjustments to your model you will see better agreement:

 

Set the Yield stress to the corrected stress value of 32800psi

Set the total load to 15000lbs and the number of increments to 100. The smaller load steps result in more refinement of your answer.

 

With these settings, and looking in the f06 file, the UWM 4698 occurs at load increment of 0.61 which corresponds to a critical of 9150lbs vs 9250lbs using hand method from Bruhn.

 

If you plot nonlinear von mises stress, then you should see that the stress is always below your yield value. You have selected VM as the criteria for Nastran to evaluate.

Re: Plastic Buckling of Plate

Valued Contributor
Valued Contributor

Folks,

Sorry for the late reply. Finally, I got some time to work on the above issue. Was able to make it work! 

 

It turns out that LGDISP/LGSTRN was not turned ON. I assumed it was ON in my previous runs. Thanks to Jon_Morga who brought it up.

 

I am getting a Pcr closer to hand calc one. In my previous runs, I was not able to find the following statements in the F06 file. 

 

You must inspect the f06 file and find the first load factor where the following message occurs:

*** USER WARNING MESSAGE 4698 (DCMPD)
STATISTICS FOR DECOMPOSITION OF MATRIX KLLRH .
THE FOLLOWING DEGREES OF FREEDOM HAVE FACTOR DIAGONAL RATIOS GREATER THAN
1.00000E+07 OR HAVE NEGATIVE TERMS ON THE FACTOR DIAGONAL.

 

In my most recent run, I was able to find the above statement and recorded the corresponding loading factor. 

 

I hope to move on to Stiffened Panels after my current project or when I find time. I don't know currently, how I will verify if my modeling procedure is correct as I don't have any hand calc references to compare the results against. Perhaps, I will post here again.

 

Thanks a ton again to all the posters who responded. This forum and its members are an immense asset to the FEA community. 

Re: Plastic Buckling of Plate

Phenom
Phenom
As a general recommendation, you must be very careful when switching from one analysis type to another. I suggest never "recycling" eg. a linear static Analysis Set to become a non-linear static Analysis Set. When you choose an analysis type in a new Analysis Set, Femap sets a few defaults appropriate to that analysis. However, if you switch from one analysis type to another in an existing Analysis Set, Femap does not change any of those defaults. So for example, in a new non-linear static Analysis Set, Femap always switches LGDISP on. However, if you change an existing Analysis Set from linear to non-linear static, it will never switch LGDISP on by itself.

Re: Plastic Buckling of Plate

Experimenter
Experimenter

Hello,

 

I've just been trying to simulate the same example, as a test to tune the local pocket buckling analysis. However, I find the same buckling load for linear and non linear analysis. According to Bruhn, the load without plasticity correction should be 10829lbs, and I find 10416lbs for the linear buckling analysis. For non-linear, it's around the same value, slightly less, but nowhere near 9250lbs.

 

Is it at all possible to find the buckling load including plasticity reduction as calculated in Bruhn, or is manual correction such as mentioned above required in this case? (although I'd expect a reduced modulus of elasticity instead). I'm not fully familiar with the need for plasticity reduction, since no area exceeds the yield stress until after the structure starts to buckle. So including the actual stress/strain relation doesn't make a difference, as the analysis is fully elastic until after buckling. Is it because the theoretical plasticity correction takes into account a certain amount of imperfection, either in shape or in load distribution that I am missing in this model?

Re: Plastic Buckling of Plate

Phenom
Phenom

Hi there,

 

For the non-linear analysis, did you note the original poster's statement:

 

"I ran a SOL 105 and the buckling factor matches very closely with theoritical results. I applied the first deformation mode to nodes scaling them down by a factor of 0.01/0.001 (tried both values)."

 

For non-linear, it is quite important (if loads are fully in-plane) that some kind of geometric imperfection is introduced, otherwise as you note, the analysis will struggle to exhibit any buckling until the in-plane yield stress has been reached - and that would be substantially above a realistic buckling load for an actual test piece.