Studded Outlets per Section VIII div 2 2

[JCrash]

In performing area reinforcement calculations (in accordance with section VIII div 2) for a studded outlet with a machined flat, I have noticed the results do not line up well with an FE model. When I perform the same calculations for a welded on nozzle, the FE model follows very accurately.

The major difference that I can find is in the stress linearization from the FE model. With the welded on nozzle, my pressure boundary extends itself to the end of the nozzle (since it's full pen welded to the vessel), which causes the maximum linearized stresses (and the shortest path through the thickness) to occur along a path as shown:

           | | nozzle
___________| |
 wall      [COLOR=red]\[/color] |
____________[COLOR=red]\[/color]|
            [COLOR=red]^----------linearization [/color]

For the studded outlets, though, I don't think the bolted connection allows me to take the attached flange as part of my pressure boundary. This changes the shortest path through the thickness and means I have to linearize across a path as shown:

_____________
 wall        [COLOR=red]| <-------linearization (along side of hole)[/color]
_____________[COLOR=red]|[/color]

The stresses along the side of the hole are much higher than the stresses along the nozzle's linearized path. This causes the FEA results to give much higher membrane stress values than the area reinforcement calcs do.

My question is: Do the Div 2 area reinforcement calcs accurately depict stresses for studded connections on a pressure vessel, and if so, is there something incorrect about the FEA?

(I have noted that in div 1, there is a specific note that states studded connections shall use the same calculations as welded on connections. I have found no such note for div 2, nor really anything in div 2 that would pertain to studded connections.)

 

[jte]

Crash-

Who ever said anything about area of reinforcement for either Div. 1 or Div. 2 being directly related to stress? You may not be comparing apples and oragnges here, but probably no closer than apples and pears. Since you are dealing with linearizing the stress, it seems that you are dealing with the old Div. 2. Which does not require FEA for opening reinforcement calc's, and for which you cannot use an FEA to "override" the explicit opening reinforcement thru area replacement requirement. Can you tell us a bit more about what you are trying to accomplish?

jt

 

[JCrash]

Absolutely:

The reason for the FEA was because our customer performs it on their pressure vessels instead of doing the area reinforcement calcs. In Appendix 4 of Div 2 (Table 4-120.1 i think), there is a stress requirement for the membrane stress near a nozzle to be below the local membrane limit (1.5*Sm). From what I remember of the code theory, the point of the reinforcement calcs is to provide enough extra material to handle the stresses caused by the concentration around the penetration. This would imply that the reinforcement calcs are directly related to the stresses at the nozzle. One would imagine that if a design met the reinforcement calcs and contained no strange or complex loading pattern near the penetration, it would also meet the code stress limits. I have found this to be the case for welded on nozzles.

The issue is that, while the reinforcement calcs say that the design with the studded connections is acceptable, the FEA does not. I would have guessed that the calcs would either be very close to the FEA, or more conservative - I would not have guessed they they be less conservative.

If, as you said, FEA cannot override the reinforcement calcs, can you give a source that states this? I'm certain my customer would like to know if their analysis is unwarranted.

And also, yes, we're still using 2004. I have not had a chance to look through 2007 yet.

Thanks for the reply, jt

 

[jte]

JCrash-

Well, you got me. I haven't heard of this being done before and spoke without double checking. It seems clear from Interpretation VIII-2-04-12 that you may use FEA instead of area replacement.

From Int VIII-2-04-12:
Question (3): Do the provisions of AD-100(c) permit the Designer to use stress analysis in accordance with the requirements of Appendices 4 and 5 in lieu of the rules in Article D-5 for nozzles and other connections?

Reply (3): Yes.

Now, I don't do a lot of stress linearization, and will defer to those on this forum who do, but I'd venture that you are dealing with peak stresses which you can ignore except for fatigue analysis. Chances are that if you were to do a nonlinear analysis, you'd see an entirely different result.



jt

 

[TGS4]

JCrash - your linearization path which goes through the corner of the nozzle is an "inappropriate" path. The path should be perpendicular to either the shell or the nozzle.

Take a look at the 2007 Edition of Division 2, in Part 5. It gives a much better description of the linearization procedure. I've been away for 2 weeks, so if I haven't answered your question, please let me know.

 

[JCrash]

TGS4 -

I have gotten a chance to look at 2007, and you're right - the SCL needs to be perpendicular to the shell or nozzle.

However, from my read of Part 5 (primarily Annex 5.A), I still haven't found anything that guides me for when there isn't a nozzle. When I machine a flat onto the shell and bolt a flange up to it, where does my SCL belong?

The only guidance I can imagine is the criteria in 5.A.3.c, which I'm not sure is clear enough to rule out the path directly on the side of the hole (shown above). The hoop and axial stress aren't exactly monotonically increasing or decreasing, but there is a stress concentration due to the hole. The radial (through-thickness) stresses are not monotonic either, and even though it is perpendicular to the start point and the end point of the SCL, it is parallel to the surface it travels along.

Where would you place your SCL if you were analyzing this machined flat case?

Thanks again!

JCrash

 

[prex]

the point of the reinforcement calcs is to provide enough extra material to handle the stresses caused by the concentration around the penetration

This is not necessarily incorrect, but I prefer a clearer picture of the situation.
The reinforcement material is needed to replace the material cut away in order to keep the primary stresses near the opening within the allowables. A primary stress may normally be calculated from an equilibrium equation. As an example PD/2t tells us that the total force PDL tensioning the axial section of a shell of length L is resisted by the area of metal 2tL.
This is no more true if the axial section passes through a hole, but if the metal cut in the hole is replaced by an equivalent amount suitably distributed close to the hole, then...
The important point in the reasoning above is that only primary stresses are concerned. When you do a stress linearization as in your first sketch above, you inevitably catch the secondary stresses coming from the interaction of the shell and the nozzle: these are mainly bending stresses, but not only, and it surprises me that you can stay within the limits for primaries (as of course also peak stresses will be there as noted above).
Coming to your questions and your second sketch, I wonder why you find unacceptable stresses on the hole periphery, as there are no secondary nor peak stresses there. However it all depends on how your model is built.
In my opinion you should conform to the following directives:
-apply pressure only on the inner face of the shell
-apply a distributed linear load around the periphery of the hole equivalent to the pressure acting on the hole
-include any required reinforcement material not included in the shell thickness by thickening the shell on the outside around the hole
If you now take your section across the thickened portion of shell, I would expect that the stresses are acceptable.

prex

http://www.xcalcs.com

: Online tools for structural design

http://www.megamag.it

: Magnetic brakes for fun rides

http://www.levitans.com

: Air bearing pads

 

[JCrash]

prex -

You are correct. I was assuming that the secondary stresses were practically all bending, and that my membrane was mostly primary, when this may not be the case.

In addition to the loads you recommended, I have the pressure pushing back on the outside of the shell up until the RTJ portion of the flange. I also have a blowoff load acting at the bolt circle of the machined flange face, and a blowoff load pulling axially at the end of the shell.

With regards to reinforcement, we're dealing with shell that was ~3" in thickness with no reinforcement. The reinforcement calcs say the thickness needs to increase to ~4.5" to replace the area removed. However, the membrane stress intensity along the inside of the hole did not get below 1.5*Sm until the thickness was over 6". We have several of these penetrations and are designing this shell to have its reinforcement integral to the shell, instead of a pad.

I'm with you when you say

"If you now take your section across the thickened portion of shell, I would expect that the stresses are acceptable."

and I was very surprised when they weren't. Which is why I am thinking my linearization paths might be suspect. Myself and a couple highly experienced analysts have checked over my model and my results, and there is currently an argument in the analysis department over whether or not the stresses I'm seeing are real or important.

Please note, as I'm not sure if I made this clear previously and I think it may be important, that this is a linearization path on a 3D model. The stresses along the inside of the circle vary greatly as you rotate from the axial facing side to the hoop facing side. The linearization path chosen goes perpendicular through the thickness on the axial side. This was the highest stressed path perpendicular to the thickness on the model.

Thanks,

JCrash

 

[prex]

Didn't think of it before, but you have a stress concentration (or a peak stress) in any tensioned plate with a hole. In a plate with a tension in a direction that's half the tension in the perpendicular direction (like in a shell), the maximum stress is 2.5 times the stress in the undisturbed region (independent of hole diameter).
Of course this is a peak stress and you shouldn't account for it. I think this is the explanation of the discrepancies you find.
I've always thought that FEM is highly impractical for checking primary stresses, and here I have a confirmation for my opinion. The separation of non primaries from the total stress is difficult, unless we go for an elastoplastic approach (personally never did it).
Your only resort would be to subtract the peak stress distribution (that has a relatively simple analitical formulation) from FEM results, but this doesn't seem very practical (nor elegant) to me.

prex

http://www.xcalcs.com

: Online tools for structural design

http://www.megamag.it

: Magnetic brakes for fun rides

http://www.levitans.com

: Air bearing pads

 

[TGS4]

I have done the non-linear analysis before and have found it to be significantly easier than the linearization method. I would recommend that you perform a limit load analysis (5.2.3) and see what the strain distribution is. Because you have a flat portion, some of those bending stresses may in fact be primary bending stresses, so the only way to know for certain is to perform the non-linear analysis.

Believe me, once you go non-linear, you will never go back to stress linearization.

 

[JCrash]

prex and TGS4 -

Thank you both. I have taken your advice and run the limit load analysis for my shell. TGS4, you are absolutely correct, it was much easier and significantly more informative than performing the linearization. I'm pretty sure this has helped solve the argument in the analysis group about the correct way to analyze this problem.

I am still curious what the correct linearization path would be in a case like this, since the limit load analysis shows, as prex commented, that the stresses along the side of the hole are just peak.

Thanks again for your help,

JCrash

 

[prex]

In fact there is no placement of the linearization path that will work, as the peak stresses will be inevitably there. The only way is to subtract the peak stresses from the calculated distribution, but this is really impractical, because a different approach is required for each situation, whilst the limit analisys is a standard procedure that works for all cases.
Too bad that when I was sufficiently young to be enthusiast of these calculations, computers were not that performant...


prex

http://www.xcalcs.com

: Online tools for structural design

http://www.megamag.it

: Magnetic brakes for fun rides

http://www.levitans.com

: Air bearing pads