Shell Elements vs Sold Elements 3

[mudmud35]

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,

 

[rb1957]

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.

 

[EdR]

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.

 

[UcfSE]

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

 

[mudmud35]

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.

 

[mudmud35]

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.

 

[mudmud35]

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

 

[rb1957]

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

 

[40818]

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.

 

[corus]

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

 

[mudmud35]

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.

 

[mudmud35]

rb1957:

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

 

[mudmud35]

Corus:

Thank you very much for the answer.

 

[ThomasH]

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

 

[GBor]

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

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

 

[prost]

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!

 

[mudmud35]

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.

 

[mudmud35]

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.

 

[mudmud35]

Here is the picture you asked for.

 

[crisb]

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