Irregular Shaped Openings BPVC 2

[PipingEquipment]

Section VIII Div 1 doesn't explicitly prohibit the use of certain shapes for openings, other than corners must have a radius (doesn't specify how much of a radius), but it recommends circular, ellipsoidal and obround. My question is, if we have a shape not covered in the nozzle calculations what is the recommended method of figuring out the reinforcement and nozzle calculations? Would FEA be the best (or an acceptable) way to do this?
This particular shape is two circles that intersect, and at the point of intersection the corner would be rounded, I recommended an obround opening but they want to make the heat transfer as efficient as possible and would like to make the shape have the smallest cross-sectional area possible.

 

[TGS4]

You would follow the rule in U-2(g) for that situation. An FEA would be permissible, provided that you can demonstrate to the Inspector that your design is "as safe as" the rules are otherwise in VIII-1.

I have written a post about the topic of performing an FEA to meet U-2(g).

 

[SnTMan]

PipingEquipment, if I understand correctly, I believe this opening could be reinforced per UG-37, if properly accounting for the finished size and orientation of the opening. It sounds as though you could treat it as essentially obround. It would likely have to be checked in two or more planes, i.e., longitudinal, circumferential, and perhaps an intermediate plane. I doubt canned software will do this properly, you will have to "roll you own".

Regards,

Mike

 

[PipingEquipment]

Ok I've never done an obround calculation, basically I just calculate it like a circle with the developed opening in the plane under consideration equal to the opening in that direction?
I also found the attached in "Theory and Design of Pressure Vessels" by John Harvey, which gives some max stress concentration as a supplemental check.

However, my concern is the portion that would be straight on an obround is now more like a really sharp corner (where the two circles intersect, that I will round) but I have no idea how much of a stress concentration this will add, the best way that I think I could figure this out is with FEA... I guess the question is how much of a radius would that corner have to have an acceptable stress, or do you not think that the non-flat portion will add considerable stress as opposed to an obround opening?

 

[PipingEquipment]

part 2 of attachment

 

[PipingEquipment]

part 3 (uploaded pages not in order)

 

[SnTMan]

PipingEquipment, generally speaking, localized stress concentrations are not explicitly accounted for in Sec VIII, Div 1 design. See UG-23(c).

As for your opening, treating it a circle in the given plane is essentially correct, as "d" is taken as the dimension of the finished opening in the plane of interest. The portion of the vessel wall represented by the intersection of the circles will have a lower stress than the portions at the"major" and "minor" diameters of the (obround) opening. I would radius the peak at 2x or 3x the plate thickness, and think no more about it. Stress concentrations are of more interest at inside corners, such as a rectangular opening.

Again, the foregoing is based on my understanding of the opening from your OP. Many unknowns here.

Regards,

Mike

 

[PipingEquipment]

I decided to the evaluation with Section VIII and supplement with FEA, in both cases the design passed. SnTMan, you were correct that the radius portion didn't have much of a stress concentration and the highest stress indeed occurred because of the opening in the shell (actually the jacket which the nozzle penetrates).
Attached are screenshots from my FEA if anyone is curious.

Thanks TGS4 and SnTMan for the advise!

 

[TGS4]

If you don't mind some feedback, I'd like to give you some regarding your FEA. I'll start with some questions:

First off, did you use linear or quadratic elements? Second, how many elements through-thickness do you have? Did you include the manway pressure thrust? How? What's your estimate of your discretization error? What are your boundary conditions? Do they have an effect on the results?

 

[PipingEquipment]

Yeah I would really like some feedback here. I have been trying to get my company to get me into an FEA class (and it looks like they will be sending me to one next month), I have a solid science and math background, I have a BS and MS in Mechanical Engineering but didn't specifically take an FEA course in college. I've seen some tutorials and read some books but I would really like someone to learn more from and actually talk to about some of the more technical aspects of the theory and software.

I choose a curved element due to the shape of the structure.
On the thinnest shell (jacket) there is only one element across its width, a warning popped up that said that element was being treated as a solid because of it being so thin, I wasn't sure if refining the mesh size would be the best way to produce more accurate results, I think it would, but the computation time would be increased.
The opening I'm analyzing isn't actually a nozzle in the typical sense, it has no internal pressure (there is external pressure of the pressure between the jacket and shell though), its actually more like a sheath around two nozzles that go into the shell that need to go through the jacket, and this shape I'm analyzing provides the opening for them to go through. Do you think manway pressure thrust needs to be added here?
I don't have an estimate of discretization error, and am unsure how to perform this...any help here is appreciated.
I am currently modifying my fixed points, originally I choose the end of the shell as fixed, but due to the close proximity of the nozzle to the end of the shell I'm adding the heads to ensure I didn't induce artificial stresses by having the fixed points so close. Then I will make the skirt that attaches to the head as the fixed point.
Thanks again for any feedback/help you can provide.

BTW I am using the BPVC calcs as the official calculations that the AI will review.

 

[TGS4]

As far as training goes, have you contemplated something like this?

I would recommend to have at least two and preferably a minimum of three quadratic elements through-thickness. If you can, use bricks rather than tets. Full fixity is a bad choice for boundary conditions - your decision to include a head was a good one. Whatever pressure the opening will see will generate a pressure thrust that must be applied. (And we haven't even started on how to evaluate the stresses...).

 

[PipingEquipment]

Do the ASME calcs cover Pressure Thrust, I don't remember seeing anything in there about it. Is the thrust equal to a point force of the pressure times the area?
About evaluating stresses, I used the Section II stress values for the stress in the analysis at the correct temperature, is there something else you think I should do or know to evaluate the stress?

THanks.

 

[PipingEquipment]

Yeah that class is the type of thing I want to attend, I think my company will pay for me to go the ASME course since it's online and I don't have to travel very far and its much less expensive. I think the one you listed would be better but I can't pay to attend that and, although I will try, I don't think my company would want to send me all that way and pay that much.

 

[TGS4]

Yes, the pressure thrust is equal to the pressure multiplied by the area. It can be a point force or a distributed pressure around the edge of the nozzle.

As far as the "ASME calcs", I am assuming that you mean the area replacement calculations in ASME Section VIII, Division 1, or the nozzle reinforcement calculations in ASME Section VIII, Division 2. If so, then yes, this load is considered in the calculations.

As far as the stress evaluation goes, there's way more than just using the allowable stress from Section II, Part D. I would recommend to follow the rules in Part 5 of Division 2.