Buckling analysis problem - very strange...

[jacksonfem]

Hi,

I 'm working for years Femap, since 9.3 version and I didn 't ever faced such a problem.
On Femap 11.0.1, I perform a buckling analysis to a compressed steel member (HEB 240), just to give geometric imperfection from the first buckling mode, as I always do.
For example, for a compressed HEB 240 of 3m length with 2 pin ends, the buckling load for the first mode, according to Euler, is 9034kN.
The column is loading with a load of 1kN at the top.

The first 19 eigenvalues, correspond to the same critical load of 5932.96kN!!! It 's crazy!!! 19 critical loads with exactly the same value and below the Euler critical load, and with crazy eigenforms like the member is a chain!!!

The 20th eigenvalue is the Euler load, 8901kN. What the f*ck is all these eigenvalues???

Something to mention...all these 19 eigenvalues, have almost zero total translation, as you will see at the pictures. The correct eigenvalue (20th), has almost 1m total translation, as always.

Please, could somebody help me???

1st picture: 1st eigenvalue with critical load 5932.596
2nd picture: 19th eigenvalue with critical load 5932.596 (as 2nd-18th eigenvalues)
3rd picture: 20th eigenvalue. The right one according to Euler.

 

[jacksonfem]

Here are the pictures.

Link
Link
Link

 

[BlasMolero]

Hello!,
Post your model here and we will take a look to it.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[ThomasH]

Hi

It can be som kind of rotational buckling. If you use pinned supports at both ends the member can rotate around it's own axis. And that can lead to numerical issues. If you constrain that rotation that may solve it.

Also, the translation is not 1 m. The buckling mode is normalized, which means that the max value is 1.

Best Regards

Thomas

 

[Naffoussi]

Hi,


19 same eigenvalues, humm so strange!!. You have 19 elements (except the one you constrained) coincidence?? for sure no . May be that each elements represent a unique eigenvalue if rotational DOF are allowed as Thomas mentioned above.


Regards,
SN

Seif Eddine Naffoussi, Stress Engineer

http://www.Innovamech.com

33650 Martillac – France

 

[rb1957]

what do the modes look like ? you should always view modes (to understand what's being excited and whether you should get excited too).

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

 

[ThomasH]

Hi again

You can look at the rotational deformations. I have seen something similar some years ago and the small deformations yoa have in the figures can be due to round off error in the solver.

I may be wrong but I have seen sometning similar.

Another "trick" would be to run eigen frequency analysis and see if there are any free modes.

Regards

Thomas

 

[jacksonfem]

First of all, thank you very much aaaall of you!!!...and sorry for my english...

Dear BlasMolero, I have upload a new file that I made it in 10.3.0 version cause the other file is at my job, where I 'm far from now. Same problems...19 same eigenvalues and the 20th is the right one!

ThomasH, I have constrained the rotational degree of freedom around it 's own axis. Also, I know that the buckling modes are normalized at 1 unit translation. But not the 19 eigenvalues. Their normalized translation is almost 0.

compositevurves very interesting this one!!! I have 20 elements...

rb1957 you can see 2 of the 19 similar in post #2! Also, I upload in a pdf file 6 modes from the 19 similar of my new file.

The beam is reacting as it should to static transverse loads, right moment diagram, shear forces etc, there is nothing wrong with the modelling...I believe it 's something in the solver.
You can also see the Femap file that I upload.

I 'm waiting with agony for you answers...

Thank you again!!!

 

[jacksonfem]

Here are the files

Femap file
Buckling modes

PS. I made 2 attachments in my previous post and nothing uploaded...

 

[jotunn]

At first I thought you had an axial constraint issue (as is previously mentioned)...but after looking at it, your model appears correct. You have "5" direction constraints at both ends and no CBEAM releases...

The strange thing is, your R2 rotation result vector is high for the first 19 "anomalous" output sets (and it shouldn't be). I share your frustration! How do a series of beam elements, constrained axially internally and externally, end up with axial rotation eigenvalues?

To further compound the issue, I ran your model through the NeiNastran solver. The results appear normal, with the first eigenvalue at 8883 (like your 20th). I haven't compared the higher values to theory, but mode shapes appear normal. I suppose this supports your conjecture: "I believe it 's something in the solver."

Neutral file with Nei's results attached if you're curios.

 

[ThomasH]

Hi again

I agree with jotunn.

I also ran your model through the NEiNastran solver and things behaved as expected. The first eigenvalue is 8883 and then they increase and the plots look ok.

It's difficult to know what happens in your model since I can't reproduce the results. I took a glance at your model setup before I ran it but there were no obvious mistakes.

I would run an eigen modes analysis. It's in principle the same type of analysis but you use a mass matrix so you have to add density to the material.

And I would send the model to Seimens to let them check it. I think BlasMolera uses NX Nastran so he may be able to reproduce the results. For me it is just guessing since I don't have the problem.

Good Luck

Thomas

Ps It would be interresting to know what the problem actually is.

 

[jacksonfem]

Guys really thank you for your response!

I have made many many models in the past with older versions of Femap, which I never had such a problem. I have good experience.
It 's very strange...

 

[jacksonfem]

I FOUND IT!!!

But it makes no sense to me...i you set the torsional constant J at the element property to zero (0)...the problem disappears and the results are the Euler critical loads!!!

As jotunn said, the 19 odd eigenvalues have big R2 rotation, something that is related to the torsional stiffness. But it make no sense that when I set it to 0, it 's all OK! That 's a GREAT FAULT!!!

Can someone think why???

 

[jacksonfem]

FINALLY I FOUND IT!!!

So...the cause of the problem, is that as you can see at the beam properties, the warping constant is 0!!!

And the critical load that appears 19 times, is the critical torsional load, for torsional buckling.

With the warping constant set to 0, the torsional buckling load, is smaller than the bending buckling load!

I just had to tick the "compute warping constant" when I set the section shape!!!

I feel silly...

Guys, again, thank you for your response!!!

 

[BlasMolero]

Dear jacksonfem,
I am glad you discovered the importance of the warping effect in open beam cross sections!!. Since the beam is an open "I" section, buckling failure can occur through a combination of torsion and bending about the element x-axis or the lateral bending, then the use of warping coefficients on the PBEAM entry are necessary to capture these effects (in case of open beam cross sections).

With NX NASTRAN for CBEAM elements warping motion is expressed by the seventh DOF (Theta x,x, here X is axial direction) so if one beam end is cronstrained we should also constrain the seventh DOF (by means of scalar point and SPC command) at the corresponding beam end to restrain the warping motion.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/