Descrepancy between FEA and Euler's formula 5

[zaist]

Hello,

I have a problem with buckling analysis for long columns. According to Euler's formula my long column should buckle.
But performing FEA with ANSYS workbench I do not see buckling. My long column behavior in ANSYS model similiar to short column - just vertical deformation, not buckling with a load twice more than critical.
Appreciate any advice!
Thanks,
Ilia Ekchtout

 

[israelkk]

What type of elements are you using? You should use elements that support buckling.

 

[ivymike]

I'm not a big FEA guy, but the results you describe could possibly result from having "perfectly centered" applied loads, which would result in compressive loading only with no moments. To make your column buckle, you should probably make the loading a tiny bit eccentric, so that it will start to bend slightly.

 

[zaist]

Hello Ilia,

Your first question appears to concern the full ANSYS interface. Is it an eigenvalue buckling analysis that you have done, or are you trying a nonlinear large displacement analysis?

If it is an eigenvalue problem, you do two runs, one is a static run in which you save the stress stiffness matrix. You exit the /SOLU processor with the FINISH command, then re-enter with the /SOLU command. The second run is an eigenvalue buckling run, in which you use the stress stiffness matrix from the first run. Ask for the results to be expanded so that you can see the deformed shapes. The eigenvalues are factors by which the applied load would be multiplied to get the eigenvalue buckling load. Most structural element types will support eigenvalue buckling analysis.

If you are doing nonlinear buckling, then if the structure has no way to bend given the applied loading, you may need something to perturb the shape. A very small perpendicular force, or a geometric imperfection may do this. Some analyses will use a deformed shape that is based on the eigenvalue buckled shape to disturb the “perfect” shape of the structure slightly.

Within Workbench, eigenvalue buckling is available. Please see the four attached image files which should clarify how to select the eigenvalue analysis and review the result. Behind the scenes, ANSYS will run two analyses—one for the static solution that generates the stress stiffening matrix, and one to form the eigenvalue solutions and eigenfunction expanded shapes. Note that the deflection amplitude is arbitrary. Run an animation to make the eigenfunction more clear to the eye.

Peter

 

[JStephen]

Two factors involved- first, the real world is not perfect, so you get minor eccentricities involved. Add some small eccentricity or lateral load to the problem if no buckling is shown.

Secondly, the model has to calculate loading based on the deflected model, not on the original configuration- a "second order" situation, as I recall. If it just uses the original configuration and calculates deflection, it won't include the additional moment caused due to the deflection.

 

[zaist]

Thanks for everybody who answered my question.

Regards,
Ilia Ekchtout,
Ottawa

 

[TheTick]

You shouldn't need to "uncenter" loads to perform a buckling analysis. The FEA program is not calculating buckling that way.

israelkk's advice is most sound so far. Also, buckling is a special analysis type in most softwares. It is in NASTRAN, at least. Are you running a buckling analysis, or just watching for buckling during a static or dynamic analysis?

"When everyone is thinking alike, no one is thinking very much." --Eckhard Schwarz (1930--2004)

http://www.EsoxRepublic.com

 

[JStephen]

Something else to watch for- your model has to be adequate to model the buckling. On Euler buckling in a column, that's probably not an issue, unless you try to model it as a single element. But to model thin-wall axial buckling or torsional buckling in that same column would require a much more detailed analysis. If you know the behaviour in advance, no problem. But it could be a problem trying to show something won't buckle.

 

[zaist]

Guys,

My model is not a single column but 3" ball screw inside a telescopic lift tubes which are 12" and 8" HSS.
It a support structure of Passenger Boarding Bridges for aircraft landing.

Thanks for everybody,
Ilia

 

[GregLocock]

As the Tick asked, Are you specifically performing a buckling analysis in the software? A conventional linear FEA will not (and can not) catch elastic buckling.

Cheers

Greg Locock

 

[ivymike]

You shouldn't need to "uncenter" loads to perform a buckling analysis. The FEA program is not calculating buckling that way.

If that isn't buckling, then what would you call it? "the bending induced by a slightly eccentric compressive load that results in a rapidly increasing bending moment as deflection increases?"

http://www.du.edu/~jcalvert/tech/machines/buckling.htm

 

[corus]

Euler's method provides does not provide a conservative method of determining the buckling load. The answer you get from using Euler's method will not be the same as that provided by looking at the rate of increase in deformation with an increase in load. The correct method is to use an imperfection in the geometry or to use a slightly offset load, as has been said.

corus

 

[zaist]

Greg,

I am specifically performing a buckling analysis in the software. ANSYS Workbench can do it - it has buckling mode. I already got the result.

Thanks for everybody!

 

[zaist]

Guys,

I can explain the case. I am performing special buckling analysis within ANSYS 8.1 Workbench. When I was applying a load as an equally spreaded pressure on the top of the column it was not working. When I apllied this load as a force, not a pressure, and placed it excentrically, it started to work.
Another remark for ANSYS users. Buckling mode was not working within the same environment with the other stress tools. I have copied an environment and analysed buckling only. Then I got a result.
I did it per advice of technical support:

Hello Ilia,

The problem seems to be that you are asking for too much within one “environment”. Try duplicating your environment, remove results from the duplicate, and insert a buckling analysis. The SOLVE that you execute will give structural results in your first environment, and buckling results in your second environment… please see the three attached image files.

Peter
_______________________________
Peter C. Budgell, P.Eng
Technical Support Manager
ROI Engineering Inc