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,

 

[prost]

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%)?

 

[rb1957]

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.

 

[mudmud35]

Ok,

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.

 

[prost]

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.

 

[rb1957]

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.

 

[mudmud35]

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

 

[prost]

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

 

[cbrn]

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

 

[mudmud35]

prost: Answering your last question:

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

 

[mudmud35]

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.

 

[mudmud35]

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.

 

[prost]

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.