Buckling Analysis

[MARIOS75]

Hi,

i'm trying to verify the results of buckling analysis performed by robot.

For a simple frame the results are very different from the exact solution.

The exact solution should be: Pcr=1.82(EI)/(L^2)=1.82(30x8.33)/(25)=18.19KN

(E=30.000MPa, L=5.0m, Sections 10x10cm, I=833.33cm4)

Robot gives Pcr=74.43

Are the results given by robot mean something else than the global instability coeficient and the critical load.?

Thank you.

[Rafal.Gaweda]

Buckling analysis calculates global buckling of the structure. Of course some modes (especially higher ones) correspond to local buckling of some parts of the structure (for instance columns).

For each load case the basic results of this analysis are critical coefficients (eigenvalues) and eigenvectors for appropriate buckling modes. Each critical coefficient corresponds to the factor by which the loads of appropriate load case should be multiplied to obtain appropriate loss of stability (buckling mode).

Basing on these coefficients and results of static analysis for appropriate load case (normal forces in different bars) critical forces for each load case, mode and bar can be calculated. Note that such critical forces are calculated for all bars (except of these which are under tension) disregarding the shape of buckling - these forces may concern bars for which buckling does not occur - in such case they have rather mathematical than physical meaning. For instance critical forces may be are also calculated for not loaded columns - in such case static analysis gives very small compression so the critical force (compression force* critical coefficient but for different (loaded) part of the structure) will be also very small (abnormally small).

Basing on critical forces and Euler's formula the buckling lengths for appropriate load case, buckling mode and bars are calculated.

[MARIOS75]

Thank you,

still the results seem different.

For the first mode,multiplying the critical coef, with the applied load results Pcr=10x7.44=74.4 which is different from the exact solution.

[Rafal.Gaweda · Accepted solution]

First of all - check supports. It seems there are pinned supports in book, fixed in robot.

Then divide columns onto several pieces ie 10, then check results

If it is not the case please attach the model.

[MARIOS75]

You are absolutely right, these are pinned supports and the results given by robot are almost 100% accurate.

Thank you

[tapio.leino]

I would like to ask:   What do you mena? What results are 100% accurate?

Is it the critical load factor, or the critical loads per bar, or the buckling lengths of the bars?

You know Robot calculates all these. They can be seen on the same table by clicking on the right button etc.

[Artur.Kosakowski]

Please mind that buckling analysis in Robot is intended to check the overall stability of the structure rather than determining buckling length of each particular bar of the model in the sense you think while running code checking according to a selected steel design code. In this sense the value of the critical factor is what can be referred to as 100% accurate (again this indicates the critical load level that would cause the entire model /or its part/ to become unstable).

In steel design module user needs buckling length of bar which is a property of bar itself and does not depend on load case and mode. In such case buckling length from buckling analysis can be taken only for very simple models or when load is applied directly to considered member and the buckling mode has local character related to this considered member.

If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.

[t.sautierr]

To follow on a bit this topic.

I read some things about the buckling analysis (general buckling). From this, I now understand that one has not to mix mode corresponding to a local buckling (in this case the analysis gives the same results than the when unsing the checkings member module) with one corresponding to global mode for the whole structure.

What is still hard to understand :

Basically the analysis consists of a matrix problem with eigen values:

1) KF=D is the problem and Robot diagonalize the matrix K and return eigen vectors and critical forces

2) Step 1) is repeated with K' (updated matrix) and D' = x time D till the problem return a K' to low (loss of rigidity), but what is the criteria to consider there is a too big loss of rigidity and then this is a buckling mode?

3) it calculates F crit which is Fat the first step in each member multiply by x (final amplification factor) for all bars, case etc ...

4) With euler's formula, it gives "theoretical" buckling lenght for each member

Second question is : physically, these results/analysis cannot be interpretated as the buckling of the weakest member for a particuliar load case for a particuliar structure? It is a global loss of rigidity and not necesseraly due to the loss of one sole member?

Last question (I thnik the answer is trivial but please confirm): If the analysis is done on a load case with several forces in several directions : all the forces are multiplied by a unique factor ... ? not only the forces which clearly destabilize the structure (horizontal for example) -> here come the engineer to find the appropriate load case / comb to analyse and find the smallest critical coefficient for all the studied situations ?

Thanks a lot for your answers.

TS

[t.sautierr]

Spare question 🙂

in the attached model, I tried a buckling analysis on the dw load case (n°1).
the smallest positive crit force value is very small , but it is found for a bar which is in tension in this case! why?
Of course the load case is a bit silly, and the modal shape correspond to something physically not relevant ... but is there a way / criteria / filter to remove these kind of modes? this is engineer's job but sometimes for large model, it could be useful.

[t.sautierr]

If someone has got time to ansewer ... it will be appreciated 🙂

Thx

[Rafal.Gaweda]

File please.

[t.sautierr]

Oups, sorry 🙂

Here we are.

Case 1 - Mode 1 - Bar 20

[Rafal.Gaweda]

http://forums.autodesk.com/t5/Robot-Structural-Analysis/Buckling-Analysis/m-p/3280277#M2089

[t.sautierr]

Rafal, the link points the topic we are discussing in 

I read that, Iwanted some more explanations.

Thx a lot

[Rafal.Gaweda]

Program calculates critical coeff (for which bar - it is not known because it is global buckling analysis). To calculate critical force Robot uses Euler formula , force in member (whatever value it is) and critical coeff (so critical coeff may not correspond to real critical coeff for abr)

[Victor_FMC]

Hello,

Please check the model/picture. 

Question is why on the middle column buckling length is calculated as to be almost 4? 

I know that for that kind of analysis Robot calculates at as for global buckling model - but still, for my undestanding it still should be about lo=2 (at least thats what i would take for the columns without separate buckling analysis).

Thanks in advance, guys!

[t.sautierr]

Bcuking shape of your structure is this, you were looking at the deformation of the load case not the buckling shape.

I'm not sure that the buckling length means something easely understandable for this kind of shape.

If you keep only two columns and one beam : 

[Victor_FMC]

Thanks for the answer!

Ye, i ve noticed also that the columns having connection with the beam seeming calculated lo- almost 2 which is correct result for that case.

Was just wondering based on what other free standing columns (connected by stiffeners with others on top) having this "lo" twice bigger then should be.

I would continue all these columns calculations in regard of lo=2 for each of those and really was hoping to see exact buckling lengths to be about 2.

[Rafal.Gaweda]

Check these:

http://forums.autodesk.com/t5/robot-structural-analysis/buckling-analysis/m-p/3280277#M2089

http://forums.autodesk.com/t5/robot-structural-analysis/buckling-analysis/m-p/3300465#M2307

[Victor_FMC]

Rafal,

Yes, i ve seen those threads before posting the question here. 

Unfortunatly it does not give me an understanding how i can use this buckling analysis in everyday practices...

For example refering again to my case/model (see attached picture)- I removed all attached parts and in response Robot gives correct buckling length coef. to be 1.89 (lo=1.89) for each column.

And then with more detailed structural model - results are something different.