How does a FEM program know when a pipe buckles, PART 2? 1

[BuckTU]

How does a FEM program know when a pipe buckles, PART 1?
BuckTU (Mechanical) 5 Sep 05 5:05
Dear FEM users,

I have made a pipe FEM model from solid elements in Msc.Marc. If I axially compress this pipe, it will buckle.

But if you think about it…How does this FEM program know this?

This perfect pipe in FEM has a uniform geometry and material properties. This FEM model will only be subjected by a longitudinal or axial force on the outer pipe ends.

Why does this pipe buckle and why doesn't it deform plastically in one big flat disk?

Does a FEM program use an initial deformation?

Thanks in advance,

BuckTU

Oké, so only gwolf agrees that if a perfect pipe will compress in a flat disk...

gwolf (Aeronautics) 5 Sep 05 9:45
The answer is that if you just perform a very large displacement analysis, it will flatten out into a disk. If there are any imperfections in your model, they will seed an unsymmetric displacement and buckling will follow shortly.

There are a number of ways to simulate buckling in FE but all boil down to some form of geometric imperfection be it localised mesh distortion or a long wavelength bend of small initial magnitude.

You can tackle this linearly using eigen-mode based buckling analyses or nonlinearly by actually including imperfections in the mesh.

In the case of Marc, I have little experience with this program but your question seems general rather than Marc-specific. I hope my comments shine some light on the subject.

but does someone know why a FEM program doesn't do this?[/color red] Without referring to any Euler or eigen value problems. What is the background of a FEM program, according to the pipe to disk problem.

Thanks in advance,

BuckTU

 

[TGS4]

In your first thread, Denial anserwed it the best.

Denial (Structural)
5 Sep 05 19:09
Corus is correct in commenting that minute numerical round-off errors in your model, or in the subsequent matrix manipulations of that model, can be the trigger for buckling. However (as Corus also says) you should not count on that happening, because Murphy keeps a wary eye out for such opportunities.

Buckling will be initiated - numerically speaking - by ANY imperfaction. Even a rounding error or discretization error is usually enough to not "squish" your cylinder, but rather to buckle it. BUT, as Denial said - I woudl never rely on that.

 

[SWComposites]

Are you running a nonlinear (material? geometric?) analysis, or an eignevalue analysis? When you say it "buckles", what is the deflected shape in the model? Is this a model of a short thick pipe, a short thin pipe or a very long pipe?

 

[BuckTU]

Hi "SWComposites"

I'm running a non-linear analysis, it is a short thick pipe. "SWComposites", Do you have any MSC.MARC experience?

Hope I gave you enough info on the type of FEM model I’m running.

Thanks in advance

Nabil

 

[SWComposites]

No, I have not used Marc; I have used Abaqus and various flavors of Nastran for FE analysis.

Please describe the deflected shape of your model; in other words what is the "bucking" mode shape? Until we understand the deflected shape its hard to guess what is going on.

Do you have linear or non-linear material properties in your model?

Like the other folks who have replied, I suspect that it is numerical round-off or small geometric imperctions in the model which is producing the "buckling" effect.

 

[BuckTU]

Hi "SWComposites",

non-linear material properties and the mode is a symmetrical outward buckling mode.

But if a numerical round-off or a geometric imperfection is causing buckling, who can simulate the approximation with FEM?....

BuckTU.

 

[rb1957]

do we want to rely on a result that is the consequence of round-off errors ? ... this is how i've read some of the posts; it is of course different if you deliberately deform the geometry.

personally, i doubt that an FE code "knows" that a structure had buckled, tho' it may output stresses consistent with a buckled phenomenon ... symantics ??

i would say that the only way a linear code allows us to predict buckling is from the eigenvalues of the stiffeness matrix, rather than from some numerical representation of euler buckling. i'm guessing that there's something inside of non-linear codes that applies the same knowledge. if the column is "short" (has a low L/rho) then the NL code should predict that the column will crush itself before long column buckling occurs.

btw, this is there a way to predict shear buckling (similar to compression buckling, ie the eigenvalue way) ?

 

[TGS4]

***Soap-box warning***

If you go back to University-level Strength of Materials, you'd find the formulations for Euler Buckling. In those formulations, the deviation from a "perfect" structure is defined as an infinitesimal perturbation. And then the mathematics follow from there, even employing small-displacement assumptions (second order derivatives can be ignored, etc).

***End of soap-box***

Once you've understood that, think about how your non-linear FE program works. As rb1957 stated, the program does not "know" when a structure has buckled. For a non-linear case, the program will let you know when your solution fails to converge, indicating infinite deflections, or negative pivots in the stiffness matrix. This comes from three possible definitions of instability (and really, buckling is an instability problem):
1) A system becomes unstable when a negative stiffness overcomes the natural stiffness in the structure
2) For each increment of load/deflection, the stiffness of the structure decreases, and/or
3) For an increment of load/deflection, the deflected solution is "un-defined"

Of course, if your model does not do any of the above, then it really hasn't buckled - yet. As with most situations, you need to apply a load in excess of your expected load in order to define your design margins. For most buckling-type problems, I usually try to buckle the structure and back-calculate the design margin. This is similar in process to calculating the first eigenvalue buckling mode and using the eigenvalue as the design margin.

So, back to the perturbation model of instability - if you have anything that is a perturbation from perfection in your numerical simulation, then that _may_ be enough to initiate non-linear buckling. But, as many posters have said, Murphy has a way of kicking you in the a$$ if you rely solely on this. It usually only shows up when you are not expecting it.

Note that one exception to my discussion of hwo a FE program lets you know that buckling may have occured is if you set it up to look at post-buckling behavior - such as snap-through analysis (ANSYS uses the arc-length method for example). In these cases, if your program can get through a local instability to find a new globally stable structure, then although buckling may have occured, it did not lead to "failure".

I think that the moral of this story is that the engineer using the FE program has to evaluate the results critically to determine the "failure" mode, and in many instances it is through engineering judgement that the decision to call it "buckling failure" has to be made.

I'll get off my soap-box now and get back to work... ;-)

 

[rb1957]

whilst i wouldn't describe analysis as "judgement", i agree with TGS4. i think aerospace is a little different to the rest of the structures world in that we have to pay attention to compression and shear alot more, 'cause typically
1) our sections are smaller than RSJs and compression strength is typically less than yield (due to crippling)
2) we have to rely on post-buckled structures (particularly shear buckled, ie diagonal tension) for strength.

we typically spend more time calculating allowables than we do on the FEA ! (well, maybe the same amount of time). i believe that some of the larger companies have automated approaches, but few things beat a pencil and paper (alright, a keyboard and a spreadsheet) and a big budget.

 

[SWComposites]

BuckTU -

A couple of ideas:

1) run your model with a perfectly linear, isotropic material and see if you get a different result.

2) carefully look at your boundary conditions and the stress distribution in the model at different load levels. If you have constrained the ends too rigidly, then you could be getting local non-linear material behavior at the boundaries. This could introduce local moments (eccetricities) which then result in the deflection shape you describe.

3) Let us know the result of #1 above, and describe in detail the boundary conditions on the model.

 

[mtnengr]

The use of any computer program, the user must fully understand the numerical methods being employed in the program. When performing a linear analysis, say based upon the stiffnes method, the response of the model will be proportional to the loads applied. No buckling will be observed no matter what the load.

When the analysis considers the resulting intermmediate deformation as part of the response to an incrementally applied load, often the underlying method of analysis uses a Newton-Rasphon or tangent slope method. Here an iterative solution is comprared to the previous step and a convergence criteria is satisfied. When the convergence has been violated, the structure is said to be "unstable" and buckling is assumed. However, this non-convergence can be instead the a result of the numerical method failing and "buckling" can not be assured. So you need some other criterion to establish buckling.

Many theories have been suggested for using the eigenvalue analysis, which establishes the numerical state of bifurcation. Perhaps the most classical approach is that of Koiter (1943). He suggests an energy approach that defines the critical point of application of load to the bifurcation point. The effects of imperfections are also considered. These imperfections are physical deviations from the true form not numerical inaccuracies of the computer!

Some theories include large deformations and rotations in the original analysis method. In the equations of equilibrium, terms that couple forces and displacement (rotations) are included. Strain-displacement relations consider additional higher order terms. If all of these factors are correctly considered in the analysis program, problems like the elastica (which an end loaded rod or pipe results in deformation patterns similar to a pretzel) can be solved. Buckling or bifurcation is not experienced.

Some computer methods employ Rik's method to move the analysis through a bifurcation point. But again, large deformations and large strain displacement relations must be included as part of the analysis.

A greater complication is included when the material becomes nonlinear. The analysis program must consider which failure law is the be followed- deformation or flow theory. Again, the analysis program must provide a procedure that uses either or both of these material laws as part of its analysis procedure. This later approach has been covered in a paper by this author in an ASME publication PVP Vol. 124.

Again, know the analysis procedure that is being used. Relying upon "numerical round-off" as the answer is not correct and has no basis. Most commercial programs have added extra considerations that include the above coupling procedures, but they are not necesarily employed automatically. You must activate these conderations.