Shell Elements vs Sold Elements
Shell Elements vs Sold Elements
(OP)
I was analyzing a buried pipe particularly 10NPS sch40 w/ 10.75 OD and wall thickness .365. Software used ANSYS10. I started modeling this pipe using SOLID95. Ran the analysis, The MAX. Stress intensity was 37000 psi represented by a stress concentration at a small area.
I discussed the results with my professor and he suggested using Shell elements instead or in other words he uses Shell elements in such a problem.
I replaced SOLID95 with SHELL93 and run the analysis. To my surprise the Stress intensity was cut by 50% and the MAX stress intensity value was 11000psi.
Could anyone help me understand?
1- Why the big difference. Since I was told that the 37000psi value is actually the PEAK stress?
3- How could I decide what element to choose to solve the following problem?
Any further explanation that would help me understand this better would be very much appreciated. Thanks,
I discussed the results with my professor and he suggested using Shell elements instead or in other words he uses Shell elements in such a problem.
I replaced SOLID95 with SHELL93 and run the analysis. To my surprise the Stress intensity was cut by 50% and the MAX stress intensity value was 11000psi.
Could anyone help me understand?
1- Why the big difference. Since I was told that the 37000psi value is actually the PEAK stress?
3- How could I decide what element to choose to solve the following problem?
Any further explanation that would help me understand this better would be very much appreciated. Thanks,





RE: Shell Elements vs Sold Elements
RE: Shell Elements vs Sold Elements
3. Can't answer this either since getting good results from FEM solutions requires experience, judgement, a background in mechanics, knowledge of the loading, etc.......also lots of FEM problems solved.. I'm certain that a large number of people following this forum can get good results using either type of element (as well as a few types you didn't mention i.e. axisymmetric) so there is really no way to give you an answer to "which should I choose"
Ed.R.
RE: Shell Elements vs Sold Elements
RE: Shell Elements vs Sold Elements
I discussed it with my professor because I am the only ANSYS user in our engineering Dept. and my director who was the expert has resigned. So in general the only other source of knowledge in this area is my professor since he is also an engineering Consultant.
RE: Shell Elements vs Sold Elements
thanks for the reply. Well in either case ihad very refined meshes.
Do be more specific. I am designinghan underground burried pipe. 10" NPS Jacket pipe 1ft long, consiting of two 3" NPS core pipes. The Jacket pipe Completely fixed on both sides
The stress concentration occured at the point between the core pipe and the support plate.
The only other comment that was given to me was that the pipe had a very thin wall and therefore there was no need in using a SOLID Element. Not sure if that was case.
RE: Shell Elements vs Sold Elements
When you say more information. Could you let me know what you are looking for to help you understand the problem.
Becasue I was trying to understand for such a problem, using SOLID Elements is not suited for modeling a 10NPS pipe with a wall Thikness of .365 and therefore the correct element to use is Shell93
RE: Shell Elements vs Sold Elements
RE: Shell Elements vs Sold Elements
As EdR said, you could (if you wanted to) get reasonable results using either solid or shell elements, though it would be a lot more work to get your solid FE to give results that get close to the truth. your Prof is right in using shells.
Your tube circumference is 33.77", and you would need at least 3 solid elements through the thickness,(so 0.125"), so for every 1/8" length of pipe you would need 810 solid elements. Dont know how long your pipe is but you would end up with lots of elems. Stick with shells, they work better for this application.
RE: Shell Elements vs Sold Elements
corus
RE: Shell Elements vs Sold Elements
This is what I heard from my previous Boss before he left but he didn't have the time to explain it. Meaning the need to use 3 SOLID elements at the thickness.
You see this is the thing I am trying to understand from an FEA stand point. Because I know very well if my model and Bc's are wrong then my results are wrong.
So when you say that I need three element. Did you calculate the Aspect ratio before coming up with this conclusion and if so how did you come up with [.125"] per element.
RE: Shell Elements vs Sold Elements
No it did not have TET elemnt. The only element used were Brick shaped elements.
RE: Shell Elements vs Sold Elements
Thank you very much for the answer.
RE: Shell Elements vs Sold Elements
It is easy to think that just because it looks good (as solids often do) the results are better.
As for the "three elements". Consider the number of integration points you get through the thickness with one vs three (to four) elements. If there is bending present one element will probably not reflect that.
I agree with with the other post, step away from the FEA and consider what happens.
Good Luck
Thomas
RE: Shell Elements vs Sold Elements
You are looking at solid elements with 3 degrees of freedom vs. planar elements with 6 degrees of freedom. ThomasH eluded to this with his statement that I'll go one step farther and say that a single solid element through the thickness won't show bending because a solid element does not transfer rotational degrees of freedom...only translational. I suppose if you are using TETs, there may be some possibilities, but they have other restrictions.
As for the 0.125" element size, I suspect Corus simply divided your thickness by 3. It would be 0.1225", so it may be a typo. If you use an aspect ratio of no greater than 4 to 1, you can reduce the nubmer of elements, but without knowing more about the geometry and the peak stresses that you are seeing, I would be reluctant to recommend doing this in the area about which you are concerned.
Garland E. Borowski, PE
Borowski Engineering & Analytical Services, Inc.
Lower Alabama SolidWorks Users Group
Magnitude The Finite Element Analysis Magazine for the Engineering Community
RE: Shell Elements vs Sold Elements
As many have said above, you still haven't given enough information; we're not being evasive, the problem is that this behavior you are seeing could be many different things. Stress concentrations have many causes from numerical to geometry to material. Maybe answer a few more questions? You said 'brick elements'--how many nodes? 8, 20? 27? Also, is the Poisson ratio near 0.5? Next, could you supply a picture of the 3D solid mesh with the stresses plotted? Also supply a picture of the mesh with loads and constraints. Be careful to blank out features that might be proprietary. I've never used it; others on this eng-tips.com forum use files.engineering.com to help with file transfers. It would really help to show us some pictures!
RE: Shell Elements vs Sold Elements
You are completely correct. Even though I have taken two advanced graduate courses in FEA Theory, most of my experience is academic and the last time I used ANSYS was 10yrs ago. But I do not have proper FEA mentoring. I am trying hard to do it on my own and unfortunately there are no FEA experts at the place I work accept to call ANSYS tech support which sometimes gets me no where!
Thanks a lot for all the replies, I know this place is not a class, but your answers are very helpful. I will take your answers and try to understand every one of them and get to the bottom of my problem.
RE: Shell Elements vs Sold Elements
I will check and try to load a picture of the model. Let me check. I completely understad that w/o seeing the model everyone could guess the answer and the problem.
RE: Shell Elements vs Sold Elements
RE: Shell Elements vs Sold Elements
RE: Shell Elements vs Sold Elements
Looks like a nice clean mesh, so it doesn't look as if there are geometric singularities. What about material singularities due to differences in materials? Can't see the loads or constraints, what about those?
OK, how is this loaded? pressurized? what else? You pointed out the location of stress concentration--geometry looks symmetric-is this 37201 psi located precisely as shown, but really the stress is about 37200 all around the inner rim at the same radius as this 37201 psi?
Also, do you have any confidence in this value of 37201? One way to check is to increase the mesh density substantially (must be someway to do that automatically in ANSYS), run it again, what's the answer? close to 37201 or not (less than 10%)?
RE: Shell Elements vs Sold Elements
RE: Shell Elements vs Sold Elements
The applied load is a evenly distributed load applied lateraly on both the 3" pipes.
The 10" is fixed on both side in all directions.
I included both plots one for the SOLID95 and the other for the SHELL93. Material same for all. Poison RATIO is 0.3.
RE: Shell Elements vs Sold Elements
RE: Shell Elements vs Sold Elements
the solid model seems to be detecting the stress peak where the tube reacts against the diaphragm.
the shell model not only misses this but also detects a stress peak somewhere else, remote from the tubes ... that seems a bit questionable.
i recall that the remote ends of the model are fixed ... do both models react the same load here (which i think is artifical, ie just something to get the model going). if it is real (like a plane of symmetry) there should be no in-plane reaction ... maybe model a 10" span with two diaphragms
if the job is as "simple" as this, why not some hand calcs (as suggested above). consider the tube is a beam on many supports, with a distributed load ... this should give you an idea as to the reactions (between the tube and the diagphragm) ... should be pretty darn close to UDL*10".
then you might have more confidence in your model, and/or model the different elements separately.
a question about the "real world" ... how does the tube/diaphragm interface transfer load ... under contact i'd expect to see the unloaded diameter shrink slightly (lose contact with the diaphragm) which might be being restrained in your model.
RE: Shell Elements vs Sold Elements
RE: Shell Elements vs Sold Elements
RE: Shell Elements vs Sold Elements
I'd like to add a comment on the location of the peak stresses and their location.
As other have said, the stress plot obtained using shell elems is a bit questionable.
However, there is maybe a little "glitch" also in the 3D model's plot, related to Ansys' use and not directly to FE theory.
I see that you left "PowerGraphics" active both in the shell and in the solid model. Whether with shells this doesn't make any difference, with solids this can be crucial especially where "peak stress" concentrations occur: in fact, PowerGraphics transfers to the "visible", outer, surface the results of the external nodes only; this will emphasize the stress concentrations at the external surface due to geometric singularities (sharp corners, common edges between angled surfaces, triple corners, etc...). On the opposite, "POWER,OFF" will use all nodal results and will plot a sort of "averaged" value at the exterior. Read the manual for further explanation (and in better English than mine...). This has already been pointed out by others ("Did you use averaged or non-averaged results"...).
Though "POWER,ON" may seem better because conservative, in reality in many cases it can be largely over-conservative (and unrealistic!), and it seems to me that yours is one of these cases.
In my opinion, your BCs may or not be questionable, but IF you used the same for the two models they are out of cause. One warning, though: in the shell model, the equivalent of the "fixed" restraints on the outer tube is not only a set of restrained translational DOF but a "Full-DOFs" restraint, including the rotations.
Regards
RE: Shell Elements vs Sold Elements
The inner plate is welded to both inner 3 inch pipes and to the outer 10 inch pipe.
RE: Shell Elements vs Sold Elements
RE: Shell Elements vs Sold Elements
The BC's are the same on both Solid and Shell models. You are correct in the Shell model the BC's will also include the ROT restraints and they are also fixed.
You see this is an underground buried pipe. So if that is the case the Assumption would be, there is no motion of the pipe either inntgranslation and rotational even though I am sure there is through long period of time but not for the instance.
RE: Shell Elements vs Sold Elements
It is possible to see that you have a geometric singularity there if you run the FE solution with this number of elements, then make the mesh much denser (say by subdividing each element into 8 elements for the 3D solid elements), run it again. If you have the horsepower, make the mesh denser yet again by 8. Compare the maximum stress against the number of elements, you'll see that the maximum stress keeps going up (if there was no singularity, you normally might expect a jump in max. stress from mesh 1 to mesh 2, then mesh 3 gives you nearly same max. stress level as mesh 2).
I meshed up a simpler structure, just a pipe connected to a diaphragm, connected to a bigger pipe, with and without fillets at the intersections of the diaphragm with the two pipes; if I didn't model the fillets, my maximum stress did not converge, indicating the problem had a nasty singularity at the intersection of the diaphragm with the internal pipe. If I did model the fillets, the max. stress did converge very well, indicating the problem was now smooth.