Modeling a vessel nozzle 3

[PhilEduard]

Hi all,

I need to model a vessel nozzle with specific length, thickness, material specs and flange to mate a standard pipe specs. My main goal is to obtain a stiffness value (lb/inch and lb/inch/degree of roration). I need to figure this out when modeling and finally analyzing a piping system. And my question is where specifically should I apply the load and anlyze so ANSYS could give me a rotational stifness.

Regards.

PhilEduard

 

[EricZhao]

Just give your model a torque, and Ansys could calculation the rotational angle for you. You do a hand calculation by torque/angle= rotational stifness

 

[TGS4]

There have been a number of good papers written on the subject of modelling nozzles in cylinders using FEA. The most recent would be WRC 493. You can get it at

http://www.forengineers.org/store.php?crn=55&rn=748&action=show_detail

That said, my appraoch is to model the end of the pipe with a spyder arrangement and then apply the loads (forces and/or moments) to the single spyder node. Let me know if this is what you are after, and I will try to give you more details.

 

[PhilEduard]

Thanks a lot for your tip Eric & TGS4. TGS4 I would think that you really know what I am looking for as a new learner to FEA and it seems like you work on pipe stress too. Could you please elaborate more on that sypder arrangement and please give more details if you would. I really appreciate your help. Thank you so much.

Phil

 

[PhilEduard]

I probably has to add this question. I am studying FEA via ANSYS eduational version and I think it is only capable of modeling up to 500 elements. Is there any affordable version of ANSYS I can use for training maybe less than ($1000.00)that could handle more than 500 elements? Thank you very much.

Phil

 

[PhilEduard]

Never mind, I saw that the new ANSYS Ed 9.0 has allowed up to 1000 elements.

Phil.

 

[TGS4]

A spyder arrangement can be best described as a set of spokes on a bicycle wheel. These spokes are beam element, but with very special (non-physical) properties. You want them to offer no resistance in their axial direction, but to be infinitely stiff in bending. This can be accomplished by applying real constants of very high Ixx and Iyy, but very low cross-sectional area. What I do is create a node at the center of the end of the nozzle, and then connect this node with these beam elements to the nodes that make up the end of the nozzle.

As a word of caution, I would feel very confident in saying that an FE model of a vessel-nozzle intersection that uses less than 1000 elements is NOT going to give you good results. For calculating nozzle stiffness, such an undersized model may tend to over-estimate the stiffness. On the other hand, it may under-estimate it too. The only way to know for sure is to make sure that your mesh is "grid-converged", that is that your answer is independant of the mesh size. Trust me, you'll need a heck of a lot more elements than 1000.

Good luck.

 

[PhilEduard]

Thanks TGS4. When you say 1000 elements does it matter if the actual size of your nozzle is small, say 10" diameter by 6" length? Assume there is no flange at all but just a sharp cut. Thanks.

 

[TGS4]

It doesn't really matter. I tend to try to use at least 96 elements around the nozzle/shell interface. Then, your nozzle will be however long it will be in reality. Finally, you'll want to model your shell a minimum of 2.5*sqrt(r*t) away from the nearest nozzle-shell intersection (5*sqrt(r*t) is better). Most of my models have 15-20k elements. Oh - and you don't need to model the flange directly, a sharp cut is acceptable.

 

[PhilEduard]

Thanks for all your help TGS4. More power to you. Regards.

 

[napoleonm]

I am trying to a FEA model for a single nozzle shell interception according WRC 107 -297 and WRC 368 with the goal to compare results from my FEA software.

Can some help me to understand the boundary conditions that I need to place on the nozzle edge?. I have tried to do a simple model with “ALL”: d/D , T/t etc parameters according with those methods.

My “model” is a shell model (with pro/mechanical as software) and I have placed the two shell body ends far enough from the nozzle interception so no distortion are done by this two boundary conditions (both have all translation and rotations fixed).

I have tried to simulate the effect of the flange stiffness adding to the model a flange in this nozzle extreme, so the bore is preserved round when internal pressure is applied.

The circumferential membrane stress just due to internal pressure (cylindrical coord system aligned with the shell body) on the shell-nozzle interception are quite similar with those from WRC368 but the bending components are high with those by WRC 368.

In others words, how WRC368 and WRC107-297 considerer the nozzle “FREE” edge?.

Regards.

 

[TGS4]

First of all, let me applaud your ambitious plan to "compare" FE results to these cookbook methods.

Second - I would not be overly surprised by differences in beding stresses between FEA and the WRC method(s). All of these WRC methods are based on some rather simplying assumptions and/or calculation methodologies. They simply cannot take into account every little detail that a well-designed FE model can. So, how big is the difference.

Lastly - Although I think that _some_ work like this (comparing FE result to WRC 107/297/368) has been done, I think that they have only looked at a few select cases. If in fact you are trying "ALL" - or even a big chunk of - the relevant parameters, this would be very interesting indeed. I would seriously suggest that you consider publishing such an interesting bit of research. Perhaps you would consider presenting it at the ASME Pressure Vessels Piping Conference

http://www.asmeconferences.org/PVP06

To answer your last question - I don't know if there is enough information in the WRC bulletins to say for certain how they handle the nozzle "free" end. Like I said before, if the authors made some simplifying assumptions, then they have neglected such a detail.

Good luck!

 

[PhilEduard]

Hi NapoloeonM,

Your question is another interesting one to me too. Could you post this thread on Caesar forum? Maybe Ray and rick could handle the question. Or let me know, I couldn copy and paste exactly your question, refer your name and post it in Caesar forum. Thanks.

Phil

 

[napoleonm]

PhilEduard..

Can you give me the adress of this forum

Thanks.

 

[PhilEduard]

Please try this link:

http://www.coade.com/support_discussion.asp

Phil

 

[TGS4]

napoleonm,

I am still very interested in your work. With the deadline for the ASME PVP Conference rapidly approaching, have you thought about submitting your evaluations as a paper? Contact me off-line at tgs4mail@gmail.com to discuss further.