turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- CAE Simulation - Femap Forum
- Plastic Buckling of Plate

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-09-2016 11:00 AM

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.

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.

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.

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.

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

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-11-2016 06:28 AM

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

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-12-2016 03:39 PM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-19-2016 12:51 PM

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.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-20-2016 09:44 AM

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

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-20-2016 03:10 PM

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.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-30-2016 04:57 AM

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.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

07-31-2016 07:31 PM

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

11-07-2017 07:39 AM

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?

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Permalink
- Email to a Friend
- Report Inappropriate Content

11-08-2017 10:36 PM

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.

Start with these Femap Basics videos

Watch Femap How To videos on YouTube

Watch Femap Tips & Tricks videos on YouTube

Download the Femap 45 day Free Trial

Download the Femap Student Edition

Watch Femap How To videos on YouTube

Watch Femap Tips & Tricks videos on YouTube

Download the Femap 45 day Free Trial

Download the Femap Student Edition

Follow Siemens PLM Software

© 2018 Siemens Product Lifecycle Management Software Inc