×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Shell Elements vs Sold Elements
3

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,

RE: Shell Elements vs Sold Elements

well, i agree with yur prof that the geometry is better suited to 2D elements ... i imagine that you had Lots more 3D elemetns than 2D.  this indicates that your 3D mesh would be much more sensitive to stress peaks.  i don't think that inherently 3D elements give higher stresses than 2D.  if this is so (that your 3D mesh was much denser) and you found a stress peak somewhere on the strcuture, you could always refine the 2D mesh in this area.

RE: Shell Elements vs Sold Elements

1. Without more information your question cannot be answered....For example we don't know how the two problems were meshed and whether the meshing was adequate to model the problem...Also its possible that the stresses you are seeing from the shell are not on the surface but rather at internal integration points (and likewise for the solid)....etc....just be assured that if your results don't match and, since you are using ANSYS, the difference is due to something you have done, overlooked, etc...

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

Why did you discuss with your professor and not your boss or supervisor at work?

RE: Shell Elements vs Sold Elements

(OP)
UcfSE:

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

(OP)
rb1957:

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

(OP)
EdR,

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

did your 3D model include TET4s ? ... i consider these to be suspect (overly stiff)

RE: Shell Elements vs Sold Elements

If you step back a bit from the FE. If your loading is something that can easily be applied in a classical sense, then how do the FE results match up with the hand calcs?
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

Look at the stresses away from the peak and get out of the habit that many have of just looking at the maximum value. If your results are similar elsewhere away from the peak then the likelihood is that both models are correct. The solid model will be better at picking up peak stresses as it will be able to represent a stress distribution through the thickness that is not linear. Shell eleemnts can't do that.  Depending on how you are assessing the stresses, peak stresses will only be of value for assessing against fatigue damage and not against yield as is normal. If it's just a static type loading then all you need are the nominal membrane and bending stresses. At worst stresses in shell elements at a geometric discontinuiy could be classed as secondary and not primary, with a different allowable stress.   

corus

RE: Shell Elements vs Sold Elements

(OP)
40818:

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

(OP)
rb1957:

No it did not have TET elemnt. The only element used were Brick shaped elements.

RE: Shell Elements vs Sold Elements

(OP)
Corus:

Thank you very much for the answer.

RE: Shell Elements vs Sold Elements

To put it simple (and it has already been said): If you have a thinwalled pipe, use shells. If you have a thickwalled pipe, use solids.

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

mudmud35,

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

Quote:

If there is bending present one element will probably not reflect 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

I could go into a long rant about the folly of allowing finite element method novices to compute some numbers with FEA just because they can, but I won't, since that wouldn't be productive. I think still that you have a learning environment primed for disaster, as it appears to me that you do not have proper mentoring to learn how to use FEA software properly. (Almost) everyone in this forum appreciates that you are doing the best you can, and that you are smart enough at least to start asking questions about your observations and not accepting the answers blindly.

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

(OP)
prost:

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

(OP)
prost:

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

2 questions. Were the stress plots generally similar but just with a different maximum stress reported? Are you plotting smoothed or unsmoothed stresses?

RE: Shell Elements vs Sold Elements

Ah, so you know some theory but, like the rest of us, have to go back and restudy some notes to remember what you forgot! Just one comment--if you mesh this up with shells, you probably can expect the stresses to be fully three dimensional at the location you've pointed to in this figure; since shells don't do well with 3D stress states, it would seem most appropriate to use 3D solids in this mesh.

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

i'm guessing that the diaphram supporting the pipes is modelled with 2D elements like everything else, and this is concentrating the load (unnaturally) to a point (well, to a line).  I'm imagining that the smaller tubes are loaded with pressure (either internally or externally).  how real is the modelled constraint ? as modelled the tubes are welded to the diaphragm ... is this the real state of the connection ? possibly the tubes have brackets or collars on them with are attached discretely to the diaphragm ??  maybe then there is no direct connection between the diaphragm and the tubes ??? and so the model is predicting something that won't really occur.

RE: Shell Elements vs Sold Elements

OK, best I can tell from these pictures is that you have introduced a geometric singularity that might not be there in real life, but it appears to be in your model. You are pulling on those internal pipes, the pipes are pulling on what appears to be a thin diaphragm or membrane oriented perpendicular to the axial length of the pipe. The very high stress is then a numerical artifact of the mesh. What can you do about it? One thing you could do is put a fillet at the intersections of the diaphragm and the internal pipes. That might not be a good idea if the fillet doesn't actually exist! Another approach is model the pipe and diaphragm as elastic-plastic material (say Ramberg Osgood), compute the stress then with a nonlinear (plasticity) analysis.

RE: Shell Elements vs Sold Elements

thx for the pix, they explain alot ...

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

(OP)
Thank you all for all the helpful hints. I will study the responses carefully.

RE: Shell Elements vs Sold Elements

In this pipe arrangement, how is the diaphragm connected to  the internal pipes?

RE: Shell Elements vs Sold Elements

Hi,
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

(OP)
prost: Answering your last question:

The inner plate is welded to both inner 3 inch pipes and to the outer 10 inch pipe.

RE: Shell Elements vs Sold Elements

(OP)
Oh one last point I didn't add and it may not be of any importance but in case someone is asking. The wall thickness for the support plate is .25 inch.

RE: Shell Elements vs Sold Elements

(OP)
cbrn:

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

Ah, welded. The connection in your mesh doesn't look welded, that's why I tried to get this clarified. You still have a geometric singularity in which you are not taking into account the weld, which I think (I don't do welds, there are other experts) means that you are neglecting to model a very important part of your structure, the weld, in the highest stress area in the whole structure. Therefore I don't think your stresses can be considered representative of what reality is. If the weld was properly modeled, I think you'd see a big difference in your results that should be more representative of what is going on in the actual pipe structure.

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.

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources