FEA on nozzle loads 1

[MikeG7]

I've come across one or two other posts on this forum about applying nozzle loads if performing a FEA. There are some things that I don't quite understand though.
One past post

http://www.eng-tips.com/viewthread.cfm?qid=165306,

suggests adding a RBE3 load distributing constraint or using a "spyder" with stiff "spokes" attached at the nozzle.
What is the aim or reason for doing this?
Where to apply the RBE3 (at the nozzle flange or at the shell junction with the nozzle?
What would be reasonable or recommended support constraints for the vessel shell and how far away to apply any such fixings?
If you know the method of applying RBE3 constraints in Ansys WB please assist with some pointers also.
Thanks chaps.
Mikeg7

 

[MikeG7]

Please some advice....?

 

[TGS4]

The RBE3 is applied at the location of load application - usually the nozzle flange. This distributes the load at the nozzle end.

Regarding distance to supports - follow this logic:
- the decay length for thin-shells is sqrt(R*t)
- 2.5*sqrt(R*t) is usually a good rule of thumb for a decay to almost-nothing.
- Therefore, to keep boundary conditions from interacting with discontinuities, I usually put them a minimum of 5*sqrt(R*t) away.

Since the vessel shell is cylindrical, apply boundary conditions in a cylindrical coordinate system. Permit UR, but restrain Uθ on both, and UZ on one, and apply the pressure thrust on the other. Apply symmetry as appropriate, but keep it in the cylindrical coordinate system.

 

[MikeG7]

Thanks TGS4 for your valued response. It will help me I am sure to "go it right".
Can you clarify further - do you put the RBE3 master node in the nozzle center and attach it to maybe 6 or 8 slave nodes equally spaced on the inside diameter of the flange? or the outside diameter of the flange? I didn't model the flange, would it be necessary?

On the issue of symmetry - I have modeled the whole shell and whole nozzle and created elements. Would I use symmetry making a slice so half the nozzle and half the shell remains? Is this necessary only to reduce computing time? Or is the way I have it also acceptable?
MikeG7

 

[TGS4]

Don't model the flange - the stiffness of the RBE3 is sufficient. However, tie the master node to the entire end of the nozzle.

Only use symmetry at the nozzle if your loads are symmetric; this is not a likely situation.

 

[MikeG7]

Thanks again!

 

[MikeG7]

TGS4
Ok, so past few days I've been working on this. I think I got the model concept right. Tried a few dummy runs to see if results compare to logical results. First I just applied internal pressure to a cylinder with no nozzles or openings (open ended) and results correlate very close to theory and code.
Then with the nozzles modeled, I apply first case of only internal pressure on all internal areas and I'm surprised by the results.
The highest Von Mises stress is at the nozzle end at the intersection of the shell. but on the INSIDE.
Would you care to comment?

 

[TGS4]

First question would be to ask if you have included the pressure thrust on the end if the nozzle? Second question would be to ask if you are using shell elements or 3D-solid elements? Third question would be to ask if the nozzle reinforcement has been done to a recognized Code like ASME Section VIII, Division 1?

 

[MikeG7]

1.Yes, I included the pressure thrust force on the RBE3 independent node.
Note, this node resides not at the the flange end of the nozzle as you previously suggested. Why did I do this? Because I was thinking that strictly speaking the forces, moments and shears act at the nozzle to barrel intersection. So I have used your previous advice but with some adjustment. I have applied this pressure force much closer to the vessel end than the flange end of the nozzle.
2. Solid92 elements. I couldn't quite get my head around how a shell element could be used because there is the nozzle weld also to consider and my understanding is a plate element is like a sheet so I did not know what "path" to apply the plate elements. If it were just 2 cylinders intersecting, then I could imagine plate elements.
3. This is an existing vessel. There is a need to evaluate new nozzle loads. Calcs were done. The wall thickness is substantial for the pressure. Repads were not required due to extra wall thickness. It meets the code criteria for opening reinforcement.
Michael

 

[TGS4]

Ok. I don't think you've done anything unreasonable. Of course, you've just finished the easy part. Now, you need to evaluate the stresses. Follow the rules in ASME FFS-1 / API-579-1 (because this is an existing vessel), Annex B.

You'll be dealing with stress linearization and classification. Pay special attention to the rules on appropriate SCLs. You'll need to satisfy Protection Against Plastic Collapse, Protection Against Buckling Failure (you will need to consider the load combination of zero pressure but full nozzle loads), and Protection Against Ratcheting Failure (assuming you don't have a fatigue issue...).

(BTW - when I teach Design-By-Analysis, this would take about 10 hours of full-time instruction to cover...).

 

[MikeG7]

Oh boy, I thought it was the hard part out the way! You've pointed me to some analysis checks that I would otherwise not have considered, thanks.
At this stage I am not sure if the vessel is yet in service or not. I will clarify, but regardless the checks and stress classification (the hard part) is unavoidable.
Protection to plastic collapse to me reads "make sure the stresses are below yield"?
I have run one load case of only nozzle loads and no pressure - the buckling case you mention. Once again, I should check against P + Q code allowable - correct?
Ratcheting failure - help!

 

[TGS4]

Protection to plastic collapse to me reads "make sure the stresses are below yield"?

No. Not even close.

I hate to break it to you, but you are officially in way over your head. I teach a course in this, and it takes me four days just to present the material. When I mentor new engineers in the intricacies of the methodology, I generally budget for a year of one-on-one mentoring.

You've pretty much reached the limit of what can be provided for free over the internet. I strongly encourage you to find a mentor who can assist you. Read the Code. Read ASME PTB-1. Read all of the referenced papers/documents from PTB-1. Read the papers that those papers reference. (You get the idea...). It is possible to self-teach yourself this stuff, but be prepared to spend about three years, and then be prepared that you will need a mentor regardless. Write a technical paper and let your peers judge you. Attend technical conferences, such as ASME PVP. Etc, etc, etc.

If this stuff were easy anybody could do it. But, it's not - it's difficult and there aren't that many of us that do it; and even fewer that do it right!