I guess you could use F_max = element_stress_max*element_area ?

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

which area?
it is a solid element

maybe the element area (normal to the element stress) ?

but I'm not sure this is heading the right way ...

i know the eigenvalue tells you something about the buckling critical load, but I don't think it's as you've written (P_critical = eigenvalue*P_applied) ... 'cause I was thinking a better approach for MS is applied load compared to critical bucking load. Maybe try out a test case, with a simple column ?

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

how do you suggest calculating the critical buckling load?

is not a typical column or geometry of literature, is another complex structure

leo16

Now you have started several threads in different forums with variations of the same question.

Why don't you start with something simple to understand what results the software gives you. For a complex structure that must be modeled with solids, where beams och shells are inadequate, is using P-critical and P-applied even a valid concept? For some applications I would use buckling stress since everything can be based on stress.

Without knowing anything about the geometry it is impossible to have any informed opinion.

But if you want F_max, shouldn't that be compared to total_mass * gravity?

What is it that you are trying to achieve?

Thomas

You're asking the wrong question, and potentially using the wrong analytical tool.

First, do you know, for certain, that your structure will remain elastic at the critical buckling load? Or, more specifically, will your average/through-thickness stress be less than 55% of yield at the critical buckling load. If so, then carry on with your eigenvalue buckling analysis. If not, then you will find no answers in an eigenvalue buckling analysis - and you will need to evaluate an elastic-plastic buckling solution, including initial imperfections (you have considered fabrication tolerances in your initial imperfections, right? Because there is an interplay between the magnitude of imperfections and design margin (note that I absolutely LOATHE the term "factor of safety" or the even more dubious "margin of safety")).

Thank you

MoS = FoS - 1
FoS = Factor of Safety = eigenvalue = critical load / applied load
The applied load is proportional to the 1g gravity so the critical gravity = eigenvalue * 1g

I don't know what you mean by F_max_obtained. A maximum force doesn't seem to make any sense for a solid with distributed loading.

Assuming elastic deformation, no initial imperfections, bifurcation bucking, etc.

As TGS4 pointed out, linear buckling is pretty unsafe. You have to really know what you're doing to use it. Prefer general nonlinear analysis with explicitly defined initial imperfections for a more reliable buckling margin of safety.

leo16.
Yes I answer in this forum. The idea was to use the latest thread. Regarding trying to get a quicker answer, perhaps you should read the rules regarding double posting .

And the question remains you say, so does mine. What are you trying to achive and have you tried something simple to understand the methodology? What does your model look like?

If you look in the literature it is not uncommon to express buckling in terms of critical stress instead of critical force. The approach depends on the problem.

If you try to describe your problem more and not just how to find F_Max it will perhaps be easier to help you. It may be simple to find F_Max if the we could see the geometry. What pre/post processor are you using for example?

Regards

Thomas

isn't this like a simple column MS = P_euler/P_applied -1 ?

I think you know "P_euler" from the eigenvalue, what is your "P_applied" from in-service/required loading ?

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

leo16.

I thought about about another way of explaining this that may or may not help you.

You have stated that you need to solve the following: F_critic = eigenvalue x F_applied

If it was a "simple" column you could instead rewrite the equation to: sigma_critic x area = eigenvalue x sigma_applied x area.
The same could be applied for shells by using thickness. And since area (or thickness) are on both sides the can be removed.

So you can conclude: sigma_critic = eigenvalue x sigma_applied.

Shouldn't that solve the issue?

Thomas

I think the OP is trying to relate the overall critical load (from eigenvalue analysis) to the local stresses in the model (under some sort of loadcase), which is a difficult thing to do.

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

rb1957
I think you are correct.

But based on his post in the Nastran forum the question there was how to get force from solid elements. My idea was to make the buckling based on stress instead of force.

But it is difficult to understand what the issue really is.

Thomas

Yes, I think he's mixing two different things.

Element force ... well, if you had a centroidal stress and the element area normal to this, then you could calculate a force.

The eigenvalue gives you the collapse load of the structure, which you can't relate (sensibly) to an element force.

Maybe you could look at how the structure is collapsing, which elements seem to be triggering the collapse (you can't have element stress from the eigenvalue) and look at the MS for these elements under the true applied loads. But I think it's better to compare the eigenvalue load to the load applied to the structure under service conditions.

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