This content has been marked as final. Show 9 replies
Changed Deformed Shape, I think out that you define wasautomatic.
I have experienced similar problems. Had a cylinder, external dia 1200 mm, Thickness of the sarg is 16 mm. Ends should be DIN 28011 (not my choice..). Theckness of these ends are 14,5mm. Matr. Aisi 316 (1.4404) Internal pressure 30 bar.
After DNV rules; minimum thickness of the ends must be 14,8 mm, After EN 13445-3 Minimum thickness of the ends are 14,7 mm, for once they're close. Fd is 173 MPa, Z=1.0 (one plate). While running it on CW designer, I measure (by probe) more than 400 MPa over large areas.
Edit; just for the record; the tank will be redesigned to a lower DP/ WP, length of the tank will be increased to store enough of the gas in question (If we have enough space, if we have enough space, if we...).
I then took a new study;
A sphere with diameter 1000 mm, thickness 10 mm is as strong as a cylinder with same internal diameter, thickness 20 mm (close too, at least). At the end of a cylindrical area (Length= 1500 or whatever), I attached a half sphere, made the transition smooth (on the outside, sphere area). added an internal force similar to 30 bar on this, (same material as above). I assumed stress in the area to be approx. 75 MPa.
The sphere area ended up with stress in the area 72 - 78 MPa, with a maximum in the transition area from sphere to cylinder shape of approx 90 MPa. (Longer smoothe transition will probably improve that). However; on the cylinder I got around 65 MPa, which surprised me, as I expected this to be minimum 75 MPa, AND also; I had expected that the program would have added the stress force from the sphere. I can't see that it did that, as I expected the stress in the cylindrical area to sum up to something like = V(36*36+75*75) = 83 MPa.
So; I can say that I am a bit confused. I do not know the CW pressure package, as this is not included in the Premium package, but I had expected to get some useful data with CW designer. I have been kicking this problem around for a couple of days now, but have landed back on my old reliable HP15C calculator. The support team have the ball now, so I'll try to report back with the solution they give me, if I forget, pls give me an email to remind me, and I'll inform you.
Hi Knut, the domed pressure vessel has been a staple of my training classes for years so I'm pretty familiar with it. The worst-case stress is in the cylindrical portion and I've run many test cases to show that the analysis compares to hand calcs if set up right. Are you using the thick or thin wall cylinder assumption? That can skew the results. Meshing could be an issue but I'd have to see the problem.
I've attached an image of this study. Hand calcs for cylinders and spheres are typically reporting hoop or tangential stress. This turns out to be P1 in most cases. If you compare your results on this problem to VonMises, you'll get additional error... comparing apples to oranges so to speak. VonMises will be higher.
I've also compared hand calcs to CW on a spherical vessel and the results match within less than a percent. I think I've posted those results elsewhere on the forum.
Hope this helps and glad to see this level of discussion!!!
Pressure Vessel FEA.jpg 82.3 KB
My english is not that good, but is expected to improve...
I can't get my version of CW to let me choose thin wall cylinder (at least; i'm not shure how to do that..).
Attached is a sketch of the last version of the sphere/ cylinder case/ study (no money involved, just my curiosity). 10 mm thickness in the sphere, and 20 mm thickness in the cylindric part. For the sphere area I'm smack on what I expected, but on the cylindric area I'm getting lower values than I had expected. 15% lower than expected actually (the pulling force from the sphere area is not considered by CW, which again give me values more than 20 % below the values that I expected). Size of the mesh varies the result some, but not significally. Have tried to vary the mesh, but the program will not let me use solid mesh for mid surface, but that "will only work for thin objects" i get as a responce...
I may try to redesign it down to 1 and 2 mm thickness, and see if I get better results...(?). Well as I'm a one man band, I'll have to get out some invoices too...
Hi Knut, there is no thick/thin cylinder option in CW. It is only in the calcs to back up the analysis. The "shell model from midsurface" option is not useful for anything more complex than simply constant wall sheet metal. I think you'll need to use solids.
If you want to send my your model (it looks small) and your supporting calculations, I'll see if I can find the discrepancy. With SolidWorks World coming up, it might not be for a week or so. (It might be sooner because I like these problems... just between you and me. I'm glad noone else is reading this!)
I have sent you the model(s) and a hand calculation (for a 3 m3 tank).
Latelatelast night (norwegian time) I discovered the following:
If I run adaptive settings as "none", I like the results much much better. It does not, I believe, still not take into account the sideways (pulling) stress caused by the end, as this would have resulted in somewhat higher stressload for the cylinder area. (P1 as you wrote, is that priority 1?) So this additional stress we will have to ad manually, for instance by a HP15C ( http://hp15c.org/ pls sign in there).
I was earlier told that by setting the properties to h-adaptive I would get better results, but that's not the case so far, at least (btw; I also had some problems software/ machine whatever, but that seen now to be ok after the last upgrade :-) )
Still not confused? Ok I'll try to sum up what I think so far (don't shoot me if I'm wrong!):
1; Use Solid meshing (ideally there should be no bending forces (on most pressure vessels), use as large meshing as possible (? a bit uncertain, but I believe that larger meshing "spreads" the strain in the material better for a pressure vessel).
2; In properties, set adaptive settings to "none".
3; Run a check for each domed end, sylinder, part etc, seperately.
4; Pulling forces, caused by the internal pressure must be added by hand, as an addendum to/ or in the report. (This can clearly be improved)
(5; In addition; check ellipsioal ends manually).
Puuh... Open for any comments, whatsoever.
Did I understand you correctly? You do NOT reccomend using shells to model thin walled vesels R/t> 10? Even if the vessel thickness is assumed constant over the head and shell? There is sometimes some vvariation in thickness in the head but for the most part the head thickness coudl be assumed conservatively the same thcikness as the shell. Please explain.
Also, can you reccomend any reading on classifying stresses according to AME sEction VIII Div.2? This is the most difficult problem I have when I attempt to use FEA for vessel leg calcs subject to lateral and vertical accelrations. Thanks. for yoru help and contribuitions.
Hi Steve, maybe I wasn't clear in my response. Shells can be very useful for modeling thin walled pressure vessels if the geometry is truly thin walled. you won't have stress linearization on shells but we do report the membrane and bending stresses separately.
What I thought I said (or what I meant to say) was that the concept of "thin walled" vs. "thick walled" pressure vessels is a calculation consideration not a COSMOSWorks or an FEA consideration. Intuitively, a vessel that qualifies as "thick walled" wouldn't be a good shell candidate. However, some that are thin walled might not be either. You'll have to experiment if shells are an attractive opiton for performance sake. Try simplifying your model and run it both ways. Don't forget to exploit symmetry.
On Knut's model, he could have used quarter symmetry and reached the same conclusions. His calcs made some references that I couldn't follow (not being familiar with that particular code) but I did verify that the results he calculated in CW were as good as could be expected and mapped very closely to brick mesh in MSC.NASTRAN.
Last thought... it has come up in the past & relevant here so I'll bring it up. An answer that corresponds to expectations with larger elements than smaller elements is usually an accident. Either your expectations are incorrect or you've converged into a singular situation where the results being tracked are fictitious. If you are confident of your expectations and the model converges past them, take a harder look at your inputs. restraints especially.
I agree with Vince. The entire "thin wall/thick wall" is a "traditional calculation" assessment, not an FEA assement. Using shells takes you out of any ASME-type calculation as you can't show through stresses.
The new ASME BPVC Section VIII, Div 2 (Design by Analysis) has specifically addressed FEA. However, many of the specified techniques appear to be based on the old WRC 350, which is about 10 years old when we had to be a bit more stingy with meshes.
As far as the head/shell deflections, I've found them to be pretty close to hand calculations. I use hand calcs (and regular code calcs) to examine the "shell/head stresses", those away from any discontinuities. If it matches fairly closely, then I can have a fair bit of confidence with all of the discontinuities.