How to constrain a closed ring beam element for 90, 180 degree symmetr

For a symmetric structure with symmetric loading, you must apply symmetric boundary conditions at the edges of your model. This means you restrain the out-of-plane translation and the 2 out-of-plane rotations. (This allows motion in the 2 in-plane translations and 1 in-plane rotation.) With only symmetrical loading (external pressure), I don't think you'll get information about non-symmetrical cases.

You should get the other 2 symmetric cases just by running the 360 degree case.

Tata

I get solution with case A and Case B, but the 360 degree case, How do I do?.. I am fixing translation and rotation for X, Y, Z in just one point, I get the same stress in all 3 cases, but only deflexion in case A and B are the same, for case C not,,, so when I do a buckling analysis I get diferents answers for case C.
How do I need to model the constrains in case C to get the right deflexions?

does your symmetric boundary condition for case B = case C ?

what do the deflected shapes look like ... plot a whole circumference ... case C, case B (replicated at the symetric boundary), case A.

Now I see your problem with the 360-degree model. Properly restraining rigid body motion with a ring structure can be tricky. But your solution with all d.o.f. at one point seems to be OK since you did get the same stress result (and I assume the reaction forces were near zero). The only difference in displacement would be a rigid body component. (It's not clear to me how a rigid body motion would affect a buckling calculation.) But if you want to get displacements for case C that also match cases A and B, you can apply restraints that are similar. For example, restraining X at 0 and 180 deg, Y at 90 deg, and Z at 0, 90, and 180 deg would take care of the rigid body restraints and should give you symmetric displacement results.

Don't apply any restraints to case C. The first 6 mode shapes will be zero for the 3 translations and rotations. The 7th shape will be the 'first' buckling mode shape.

Tata

CORUS: Well, the only way for a model to run without constrains is for modal analysis only, so I will agreed that the first 6 modes will give you the 6 rigid movements, but for a Buckling analysis with not constrains I don’t see how to do it (and I will guest is not possible).

I am looking to do a buckling analysis for a more complex shape but I would like to verify first with a simple model the results from pro/mechanica so I would like to verify the models constrains to compare with theory (P= 3.E.I/r3).

I have been playing with constrains options, BUT still I don’t get the right constrains set to allow a single ring under external pressure to behave as theory say.

Any other suggestion hoe to constrains this model?

Mark,

"Buckling analysis with not constrains I don't see how to do it (and I will guest is not possible)."

You are quite right. Although modal and buckling analyses are both eigen problems, there is no equivalent to "free-free" analysis with a buckling problem, the structure requires sufficient restraints to prevent rigid body motion. Also a buckling analysis can produce both positive and negative eigen values. Ignore the negative values, they are mathematically valid solutions, but do not represent any real physical solution.

Why don't you model 3D shells or solids instead of 1D beam elements? How is the "real" structure that you are modelling actually supported?

Hello John
I am trying to model a fuselage section, basically simple assumed as a one support ring and a cylindrical shell skin under external pressure. (like a submarine)….

I want to see the stress in the ring, as you could image, the ring is free in the space but supported by the shell skin..

Basically I want to prove my model with a basic ring model, but I cannot get the way to model such simple structure (the ring) and compare with theory.. when I apply the buckling equation 3EI/R3 I get a buckling pressure that do not correspond with what I get in my FEA.

I believe this equation is only for in-plane shapes deformations.. but my FEA is given me in-plane and out plane deformations,, those values for the in plane shapes modes do not mach the theory one.. so what to do.

Dimple model:
Square section 25x25mm
Mean radius R: 1000 mm
E=193053 N/mm2 poisson=0.3
Inertia: 32552.08 mm4

Load case: unitary pressure
Theory buckling pressure: 150.8226 N/mm

Have you compared the theoretical buckling pressure against your applied pressure multiplied by the eigen value that the FEA gives you?

Please can we clarify some basics?

You quote the buckling equation where pressure = 3EI/r^3. In this equation should I be Inertia per unit length?

You state that the material is steel with E=193053N/mm^2. Surely these cannot both be correct?

You quote a theoretical buckling pressure of 150.83N/mm. Shouldn't pressure be in units of N/mm^2, and how do you get the value of 150.83N/mm with the input data you show?

The Timoshenko equation will be the elastic critical buckling pressure. Is your FE analysis an eigenvalue buckling analysis, and not some sort of nonlinear collapse load?

Is Pro/Mechanica a suitable tool for this task, with an adequate range of analysis options and restraints?

If you wan't to emulate the Timoshenko equation will you not need to provide restraints out of plane?

E = 193 GPa is reasonable for steel, = 28E6psi

there's definitely a dimension thing happening 3EI/R^3 doesn't give you pressure. my guess, without checking calcs, is that gives your running load = pressure*width, which is why the answer is N/mm, but i get 18.85 N/mm ... suspiciously 1/8 of 150.83 ??

See
which shows the derivation of this formula.

A 180 degree model should suffice to get the first buckling mode.

Note, in the first post "and an mean radius of 518 mm" was quoted, now it is 1000 mm.


As Crisb has asked "Is your FE analysis an eigenvalue buckling analysis, and not some sort of nonlinear collapse load?"


"I want to see the stress in the ring" - An Eigen solution will not give you an actual stress value. You get an Eigen value (which equals critical load when multiplied by applied load) and an Eigen Mode shape which is always dimensionless whether you are doing modal or buckling analysis. You can of course from the mode shape derive a stress "pattern" (as many solvers do), but not a value at any one point that you can quote.

But, a static non-linear geometry solution could give you a collapse load and stresses as you increment up the applied loading.

Thanks all.

Sorry if I mix up some numbers.
Let fix the case for future reference to R= 1000 mm .
Square section: 25x25 mm
I: 32552 mm4
Yes, material is steel E=193053 N/mm
Load case: unitary external force 1 N/mm (since my benchmark model is beam element)

Timoshenko buckling pressure: 18.85 N.

My FEA is simple lineal buckling calculation, no exotics cases (large deformation, non lineal cases etc) are being taking into account.

I just one to see from my FEA a buckling factor of 18.85, which I don’t get it.. my FEA shows values of 81 as a buckling load factor.

John, I agreed with you, a modal analysis will not give you stress, I just do it to verify the modal shapes and to check any rigid motion in my constrain assumptions.

I run a static analysis and from those results I run a buckling analysis.

I would like to see, if somebody has a FEA tool to verify this simple case I am posting, so we can verify constrains set etc.

I am wondering, if the Timoshenko buckling pressure for a ring (3*E*I/R3) is just for “in plane” deformation cases, my model give me in plane and out planes buckling cases, so I guest this equation was developed from a 2D analysis (strain plane analysis), so if is so, how to get the out plane buckling calculation from hand calculations? For me to compare with my results… (thanks for the paper, I had it before).

Mark, what software are you using and the element type in that software?

I ran this and got the lowest mode with a load factor of 25.1. To get this I had to use isobeam elements which model the beam curvature within each element. Using straight beam elements appeared to give spurious results, however small the mesh. To avoid spurious negative modes I found it better to apply the pressure externally.
Maybe this is a tough test for analysis methods and element formulation?

software is mechanica from proe WF4.
element a beam element with 25x25 section.

crisb,
Could you let me know what are your constrains for your model.
did you modeled as a full 360 Degree model?.
Which one is your software?.

180 degree model in Adina. Semi circle restrained out of plane. One end point fully restrained translation and rotation, other point also fully restrained except free to move towards first point. Relevant mode shapes similar to above paper. 4 node elements with 50mm mesh, LF 25.3 with 2 node elements 100mm mesh.