Nastran Post-Buckled Analysis of Thin Plates

[MBD26]

I'm working with a thin (.040) rectangular panel in an airframe that easily buckles under shear and goes into diagonal tension. The panel is bolted down to frames/stringers on all four edges. I've got a 2D breakout Nastran model of the region detailed down to the fastener level with cbushes, and I'm interested in both pulling the shears at the fasteners and pulling a KtS at a fillet on the edge of the panel when it reaches max loading in the buckled state. I know diagonal tension loading can be easily calculated, but I'm interested to see if this can be done directly with Nastran

My understanding is that sol105 will only give you the eigenvalue (internal loads meaningless) and that sol106 will give you the stress state at the point of buckling, but then fail to converge immediately afterwards. On the latter point, maybe this won't be the case for panel shear buckling (vice column buckling) where the panel is still capable of carrying load? Is there any other way of putting this model through Nastran and getting out meaningful internal loads for the post-buckled state?

 

[aerostress82]

I've performed onset of buckling & post-buckling hand calculations before, but what you are asking seems to be more into Nastran rather than the hand calcs.
So, here it is. I had found this pdf before while looking for diagonal tension. Probably it won't have the answer right away in there but may give you clues on how to manage what you want to do via Nastran:

https://web.mscsoftware.com/support/library/conf/auc99/p05399.pdf

Any feedback from you after reading this pdf will also enable me do some research for you. I'm just very interested in anything related to aircraft stress.

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

 

[SWComposites]

Use sol400. Or better yet, use Abaqus.

 

[aerostress82]

So, I did some reading on this today. What SW says makes sense - but there should be some background to what you want to do, so I'm adding them below:

If you read this, you'll have a better understanding of non-linear buckling. (it helped me some)

http://www.deskeng.com/de/linear-and-nonlinear-buckling-in-fea/

What I'm writing below will make sense "after reading this above link through".

Only for the sympathetic pressure or displacement field for the non-linear buckling seems to be a "changing parameter" due to the different modes you will receive at different locations of your assembly from the linear buckling analysis. So you may need to check it for 5-10 different variations depending on your mode. (or less - I would check it at the first 10 modes to see how the behavior is changing with each mode, as I have never done anything like this before, then at the next times, maybe 3-5 modes could be enough after being able to predict how it may behave by the time)

To perform this, you can look at "MSC Nastran 2014 Nonlinear User's Guide (SOL 400)" pg. 110. It shows a sample SOL400 post-buckling calculation.
Also, I've found this as a whole thesis of what you want to perform. This gentleman states that Abaqus and Nastran give the same results for linear and nonlinear buckling analyses:

http://www.solidmechanics.iei.liu.s...MasterTheses/14-01954MertMuameleciRapport.pdf

If you run into problems with "convergence" of your analysis, try to tweak the epsilon (EPSU, EPSP, EPSW) values in the NLPARM card. (whichever epsilon values you are using will depend on what KMETHOD you are using for stiffness updates)

Looks like you have a whole project ahead Let me know if I can help with anything else.

Spaceship!!
Aerospace Engineer, M.Sc. / Aircraft Stress Engineer

 

[stressebookllc]

I believe there are dedicated diagonal tension elements in NEiNastran.

Aerospace Stress Analysis and FEA Courses

http://www.stressebook.com

Stressing Stresslessly!

 

[Burner2k]

Hi,
I hope its OK to resurrect this thread. I want to perform a Nonlinear (post buckling) analysis on a Wing Box. Currently, I am mainly interested in capturing the load redistribution after post buckling of skin in to stiffening members.

Before I attempt a complex model like a Wing Box, I thought I should analyze simpler structures like stiffened panels.

I went through one of the links posted by aerostress82; will go through the other document i.e. thesis later on today, but I would appreciate pointers towards any tutorials or open source materials which goes in to the details of performing a SOL 106/400 nonlinear buckling analysis (mentioning what pitfalls to avoid etc).

I am sure I will run in to issues. Hopefully, the more experienced members here will help me through the process.

Thanks in advance,
- B

 

[rb1957]

and checking the tension loads on the rivets (prying from the web buckles) ?

and calculating MSs for the web ??

another day in paradise, or is paradise one day closer ?

 

[Burner2k]

RB1957,
Did not understand your reply completely!

The structure/stiffened Panel (as well as Wing Box) initially will be modeled as integrated i.e. no fasteners will be represented in FE. Plan is to scale up the complexity gradually.

Yes, hopefully the additional tension loads induced in the rivets due to web buckling will be captured when we move on to riveted FE representation of the structure.

Edit: Also any tips on how to apply initial imperfection load?

One should never type with half awaken eyes. References mention 5% of thickness of the sheet.

I think in another thread, SWComposites had mentioned that a displacement equal to 1/2 the thickness of the sheet will also do.

But if I have to do a nonlinear for a column (1D line element), how do I determine the initial imperfection amount? 5% of the thickness of the beam/column works?

Also, I would like to ask about the procedure? For a shell element, where does one apply the imperfection? To a series of nodes where max displacement occurs from SOL 105?

 

[Burner2k]

Folks,
Any suggestions or help with the above please? If I can get pointers towards any materials or resources which can help me get started, that is acceptable as well.

Thx

 

[Burner2k]

OK.

I found this good webinar from a company called Predictive Engineering (along with white paper & demo files) about how to do linear & nonlinear buckling in Femap with NX Nastran. Very informative, especially procedural wise!

Buckling Mini-Workshop

For inelastic buckling using SOL 106, the folks had to provide an initial imperfection for the cylinder and this was achieved using a custom API tool "Nodes move by deform with options". I'll have to look in to manual or play around to get a grip on what exactly the command does.

Does Patran has a similar command like the above? I think I can try to create a spatial displacement field based on the SOL 105 Eigen vector mode (& scale it up suitably) and apply it to the undeformed model as the initial imperfection for NL 106 analysis.

Any suggestions on the above would be appreciated.