How does a FEM program know when a pipe buckles? 1

[BuckTU]

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 thick 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

 

[rob768]

To my knowledge, It calculates a buckling value. If this value large than 1, you have a safey, if it is smaller than one, buckling will occur. (a value of 1 means you are on the threshold of buckling, 2 means you are at 50% of buckling load). Of course, the program does not include material imperfections, geometry flaws etc. It calculates buckling purely on a theoretical basis. So be sure to eningeer with a safety in mind!

 

[gwolf]

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.

 

[Modey003]

Just to ellaborate on what gwolf and rob768 said. There are two ways that buckling can be predicted in FEA. One method stated by rob768 is a buckling criterion. During postprossing you can have the program plot contours to see if the buckling criterion has been exceed in a given region.

But lets say you don't have that kind of data availible. gwolf's method of doing a displacement analysis after introducing defects in the model can be used. Using unsymmetric nodal forces as your loading boundary conditions will also work.

Modey

 

[corus]

Euler buckling and buckling through large displacements will give different answers. Euler buckling gives a larger load to buckle and so is not conservative.

I don't know about Marc either but your model isn't a perfect pipe but will have slight imperfections in the geometry. Perhaps this is why it buckled. It is normal practice to introduce a slight imperfection into the geometry or to introduce another small load to induce buckling through large displacements.

corus

 

[gwolf]

Thanks corus, I'd never done the comparison. Bit of a nonlinear fan myself. These days unless I'm on a huge model I prefer to run nonlinearly for everything anyway and just output the last load increment - removes another question mark and saves time in the long run.

 

[Denial]

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.

 

[Kwan]

Euler buckling is only accurate for long columns. Using (2PI()/E)^.5 compared to the slenderness ratio will tell you if you have a long or short column.

Short columns are analyzed using Johnson curves (dependent on crippling strength). You may also have to consider beam column effects (if you have any moment in the column). This may be why Corus noticed Euler buckling giving unconservative results.

These checks should be done to validate your fem. I've seen fem models give very inaccurate results due to bc's, element refinement issues, and such. Murphy loves to hide behind fem analysis and the only way to keep Murphy away is to validate your results.

 

[kellnerp]

BuckTU

How does the FEA program know the pipe will buckle? Why doesn't it collapse into a big disk?

When you use a static solution in an FEA program the pipe will collapse into a flat disk?

When you use a buckling solution in an FEA program the pipe will be shown to have several buckling loads. The way the FEA program knows when the pipe will buckle is by looking for points in the static solution for the structure that have more than one correct answer. This is the same thing that happens when a hand calculation is done for Euler buckling loads. The assumption is that elastic buckling will occur before plastic collapse.

 

[amanpreet]

the finite elements requires you to put several input like you want the non linear range ? for that you have to declare your material properties in a non linear graph. but keep it in mind never show that your curve has negative slopes then you cannot able to model anything.
so everytime you have to give the curve after yeeilding a very small slope.
and then while you tries to run a solution check for the problem make sure that the laod is increasing in the increment by that you can get the load the deflection curve non linear.

then you can compare your results with the results gievn by standard solution in advanced mechancis of material.
regards
aman

regards
Amanpreet