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

[MarkCopland]

How to constrain a closed ring beam element for 90, 180 degree symmetry cases under external pressure.

I need help to define the following simple constrain beam case

I got a “circular closed ring” with a square profile 25x25 mm and an mean radius of 518 mm, material steel, the ring is has a external pressure of 100 N/mm2 as example.

I would like to simulate this case using a FEA software, as a 1D beam element.

But I would like to use 3 different constrains sets (case A: 90 degree, case B: 180 degree symmetry) and case C: the full 360 degree model.

My intention is to compare results for buckling pressure values, (so I took this 3 cases to evaluate non symmetrical buckling cases -90 and 180 degrees- with regards to the 360 full model.

My question is how to set the constrains for this 3 cases.

Any help will be welcome

 

[rb1957]

mark
first, "pressure" is N/mm^2, not N nor N/mm. Timoshenko is calc'ing pressure per unit width (i believe), leaving it as a running load (N/mm) is fine as it matches the load you're applying.

2nd, how are you applying a radial pressure load to a beam element ? maybe ProE allows this; in a model i'm working on now I wanted to do the same thing and settled for adding dummy skin elements that would take the pressure (normal to the panel = radial) and apply it to the beam elements.

3rd, "I run a static analysis and from those results I run a buckling analysis" ... what does the 2nd part of the sentence mean ? what "buckling analysis" are you running with the FEA stresses ?

 

[MarkCopland]

Thanks rb1957
To be more clear:
1) Load is: newtons per unit length ( N/mm)..not pressure (let try not confuse with my original case post..let run the simple case as described before).

2) Before to run a skin model for load distribution, let set the model for as simple ring as described before.

3) to run a buckling analysis, a static analysis need to be performed (at least with pro/mechanical), so the buckling load you get is times the load you set in your static analysis.

CRIBS:
180 degree model…OK
Semi circle restrained out of plane.. you mean you no out of plane movement and rotatrion for your semi circle…so you pick all your semi circle and set rotations for x,y,z fix.?

One end point fully restrained translation and rotation… you mean point fully fix

other point also fully restrained except free to move towards first point…you mean only translation movement towards firt point allowed and rotation in X,Y,Z are fix?

Theory: 18.85 you get 25. 3.

I try to do it and I don’t get the same, could you let me know what are the frequency of your model ( just for me to verify) and what is the stress for your static analysis?.. does make sense the deformation shape of your static analysis for this load?.

How can you get those symmetrical shapes for buckling when you got a fully fix point?.

 

[crisb]

Mark:
Semi circle restrained out of plane...y translation only.
One end point fully fixed....yes
Other end point fully fixed except z translation.
Theory 18.85 I get 25.1 (smallest mesh attempted).
First mode shape attached.
I think but am not certain that the element type could have a lot to do with the results, am doubtful that standard straight beam elements will give you good results.

 

[crisb]

My model is getting the critical buckling pressure very close to 4EI/r^3, so there is probably a boundary condition problem that I haven't figured out!

 

[crisb]

Cosmos verification manual problem B5 is very similar to this problem, and is showing the theoretical solution as 4EI/r^3. Any comments?

http://www.stresscalc.ru/cosmos/BasicSystem_2.pdf

 

[johnhors]

Cris, the cosmos example is for 90 degrees only.

http://www.Roshaz.com

 

[IDS]

This is all very interesting.

Firstly considering only the in-plane buckling:

A few years ago I did an investigation of restrained buckling of pipes (I have attached a paper I did on it, although it only mentions unrestrained buckling in passing). In the course of that I compared Euler's solution with FEA solutions, using Strand7. I found that the "linear buckling" solver in Strand7 gave a solution very close to 4EI/R^3, rather than the theoretical solution of 3EI/R^3, but if I did a non-linear analysis, applying a very small additional point load at one node to initiate buckling, I got a buckling load close to 3EI/R^3.

I have just re-run this analysis with the section properties quoted above, and get the same results; i.e.:

Non-linear analysis buckling load = approx 18.9 N/mm
Linear buckling load = 25.16 N/mm (4EI/R^3 = 25.14 N/mm)

The FEA model was a full circle modelled with 80 beam elements, with global freedom conditions set to "2D beam", i.e. Z displacement and bending about X and Y restrained. The top and bottom nodes were fully restrained except for Y translation, and the mid height nodes were restrained in the Y direction. A quarter circle model with the same restraints would have been equivalent.

I never worked out why the linear buckling analysis gave different results to the buckling equation and the non-linear analysis, and I still don't know, but it interesting that the COSMOSM results are similar, and they quote a theoretical value of 4EI/R^3. I'm not familiar with the Donnell Approximation.

If I allow out of plane deformation, from the linear buckling analysis I get two buckling modes at 15.3 N/mm, then the third is the in-plane buckling mode at 25.16 N/mm. With the non-linear analysis I get out of plane buckling at about 8.8 N/mm. At the moment I'd recommend going with the 3D non-linear results, remembering that a small out of plane force or initial deformation is required to initiate buckling in the analysis.

If anyone can shed any light on the difference between the linear buckling analyses and the non-linear analyses, I'd be very interested.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[IDS]

Looking at the thread in the Mech Eng forum:

http://eng-tips.com/viewthread.cfm?qid=288326&page=1

if this is for a stiffner to a cylindrical pipe subject to external pressure, the pipe will provide significant restraint to out of plane buckling, so taking the fully unrestrained case would be very conservative.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[crisb]

IDS: I am wondering if the difference could be the application of load and the 3* is if the load is normal to the deformed shape and 4* is in the original undeformed direction. Presumably your nonlinear analysis is a traditional nonlinear analysis and not an eigenvalue buckling analysis. This is obviously now becoming a highly theoretical topic, see following paper as an example of different factors quoted over the years:

http://www.springerlink.com/content/k2r7ww787732738h/fulltext.pdf

Johnhors: The first mode shope is doubly symmetric so should be identical to the 90 degree mode.

 

[MarkCopland]

I don't get these buckling load ( 209 !!!!).
and I habe been playing with all BC possible.

and including 3D solid model.

I tried to do it and I don't get the same, could you let me know what are the frequency of your model ( just for me to verify) and what is the stress for your static analysis?.. does make sense the deformation shape of your static analysis for this load?.

for the out plane buckling I get around 59 ( which comes as the 1 buckling mode)...the 209 is the buckling for the 1 inplane mode shape.

 

[crisb]

I haven't run natural frequency or static analyses. I don't think its helpful for us to compare freqencies, as this is introducing another variable (mass or density). The static stress can easily be checked from simple hand calculations.

The usefulness of simple hand calculations as a sanity check has been "stressed" to other posters many times recently but seems to fall on deaf ears.

Please check carefully your geometry, section properties, and modulus of elasticity, and perhaps post a picture of the first mode showing elements, loadings, and boundary conditions for the in plane mode.

 

[IDS]

Mark - your numbers keep changing! Could you post a sketch of your simplest model showing dimensions and end-restraints, and summarising the buckling loads you get for different modes and methods of calculation.

crisb - do you have a simple hand calculation method for out of plane buckling of a circular ring? If so, could you post it.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[IDS]

I am wondering if the difference could be the application of load and the 3* is if the load is normal to the deformed shape and 4* is in the original undeformed direction.

That seems to be the case.

If I do the non-linear analysis with point loads directed towards the centre of the circle at each node I get a buckling load of about 25.3 N/mm, which is in good agreement with the linear buckling analysis and the 4EI/R^3. The earlier analysis used distributed beam loads, applied perpendicular to the beam, so the load direction would be adjusted at each iteration.

As you surmised, my non-linear analysis is simply a static analysis including geometric non-linear effects, with the load incremented in small steps until the response becomes clearly non-linear. The linear buckling analysis is an eigenvalue analysis.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[crisb]

Doug: Equation 146 in the following reference appears to give an expression for the out of plane buckling pressure on a ring, which seems to be attributed to Wah. I just got it from Googling and am not commenting on it's accuracy.

http://archives.njit.edu/vol01/etd/1970s/1979/njit-etd1979-005/njit-etd1979-005.pdf

 

[IDS]

Mark - the paper here:

http://202.114.89.60/resource/pdf/2638.pdf

looks like a good practical introduction to the analysis of submarine pressure hulls.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/