Eccentric cone with angle 45° (ASME VIII-1) 1

[Jezovuk]

Hello to all,

I have a little problem with one pressure vessel with eccentric cone. (α~45°- see the attached picture)
In UG-32 (g)(2) stands that angle should not be larger than 30°. However, 1-5 (g) say that junctions with angle grater than 30° are allowed but only if design is based on special analysis.
My question is: What is the simplest way to resolve this issue and is the FEM Analysis allowed?

Thank you for your answer in advance!

 

[Jezovuk]

Anyone?
I have one more question regarding the same vessel.

If the "End of scope" is marked like on the picture, does the Positions 1, 2, 3 have to be made from ASME Materials or are they out?

What is the correct way in this case to interpret U-1 (e) (1) (-d)? Or there is some other rule that must be taken into consideration?

Thank you!

 

[prex]

Yes, you can use FEM, but be warned: to interpret it you need to know how to classify stresses into membrane, bending, discontinuity, local, etc.
And, accepting your end of scope limit, item 1 is like a flange (out of scope), item 2 is like a bolt (out of scope) and item 3 is like a nut (out of scope). However your detail appears to be a pressure retaining cover, not a connection to an external piping or device per U-1(e)(1), so it should be included per U-1(e)(3).

prex
[URL unfurl="true"]http://www.xcalcs.com[/url] : Online engineering calculations
[URL unfurl="true"]http://www.megamag.it[/url] : Magnetic brakes and launchers for fun rides
[URL unfurl="true"]http://www.levitans.com[/url] : Air bearing pads

 

[Jezovuk]

Thank you prex!
Yes, u are right, U-1(e)(3) is clear.
I have a pressure retaining cover (item 2) so it must be included, together with attaching "like a bolt" (item 3) and "like a nut" (item 1).

 

[Jezovuk]

How would u interpret this result of FEA?

Conditions:
Material: X5CrNi18-10 (1.4301)
External loads:
Inner pressure: 5bar
Temperature: 50 °C
Fixed geometry: upper surface of cylindrical shell
Criterion: Von Mises

In order to avoid any peak stress in transition area between cone and cylinder i made a round fillet area which represents inner weld and thus is close to real conditions.

Can i make the following conclusion: "Maximum stress appears on the upper edge of cylinder shell and is result of given initial conditions (fixed geometry)."?

 

[prex]

The stress is quite low, so you should be OK. However IMO you should determine the stress in the transition zone for your report. Also, if your model, as I suppose, is shell type, you won't see any peak stress at the transition and you should avoid creating a round transition. If on the contrary your model is with solid elements, then you need to determine the bending stress at the transition, and this one is given by the difference of surface stresses at inner and outer face.

prex
[URL unfurl="true"]http://www.xcalcs.com[/url] : Online engineering calculations
[URL unfurl="true"]http://www.megamag.it[/url] : Magnetic brakes and launchers for fun rides
[URL unfurl="true"]http://www.levitans.com[/url] : Air bearing pads

 

[Jezovuk]

Thank you prex!
It is a solid element. How can i now detemine bending stress at the transition? (i am using solidworks simulation)
Maybe u have some example?
Is this an answer:

http://help.solidworks.com/2014/English/SolidWorks/cworks/t_linearizing_Stress_Results.htm

?

 

[TGS4]

I'm going to give you some blunt, yet hopefully productive, comments and advice:

- your mesh is crap. The fluctuations that you show in your stress plot ought not to be there, and are as a result of a very poor mesh. You have likely used tetrahedral elements - I truly hope that you have used quadratic tetrahedrals, because linear tets are all kinds of bad. I would take prex's advice and use shell elements, but if you are bound and determined to use solid elements, please use hexahedral elements. Ensure that you have a minimum of 3 quadratic bricks in the through-thickness direction, and at least 96 in the circumferential direction.

- do not model any sort of fine fillet radius at the corner. The methodology will sort out the peak stresses.

- cone-to-cylinder junctions often result in compressive stresses, which lead to a different failure mode that is less dependent on the magnitude of the stress: buckling.

- follow the methodology presented in ASME Section VIII, Division2, Part 5. You will need to satisfy ALL of the failure modes: Plastic Collapse, Local Failure, Collapse From Buckling, and Failure From Cyclic Loading: Ratcheting. And you will also need to consider possibly fatigue if you will be in cyclic service. You are performing calculations for an ASME Section VIII, Division 1 vessel, utilizing the statement U-2(g). Although there is not (yet) guidance on how to use FEA to accomplish this, I have written a post that addresses what I believe to be industry best practice in this regard -

http://becht.com/blog/performing-an...ision-1-to-qualify-an-article-u-2-g-component

My recommendation to you is that if you have never done this before, either get a good mentor or hire an expert. I would estimate that a design like this would probably take me a day to do, and then another day or two to write up the report, suitable for submission to the most challenging jurisdictions in the world.