Solid vs Shell elements for plate structures ?

[Jacques28]

I have been ask to evaluate an analysis done on a bifurcation. The analysis was done using solid-shell elements (SOLSH190 – Ansys – 8 node brick), with one element across the thickness. Apparently this element can handle bending quite well and give accurate answers

My FEA knowledge is about 5 years out of date. The type of solid elements I am use to give bad results for plate structures (especially using low order elements – with 1 element across the thickness). I know the solid mesh is quick to build from the CAD model. Making a shell mesh takes longer and more skill.

Despite the new solid-shell element I am uncomfortable with it, and don’t know whether to trust the results.

Does anyone have advice, or maybe a link to a article where they compare the accuracy to tradition shells?

 

[corus]

A single solid element through the thickness would be no good if there was through wall bending as there is only one gauss point at the centre of the element. For shell structures these elements are ok if the stress is predominantly a direct/membrane stress. Better results would be obtained with a 20 noded quadrilateral solid element or just spend more time and build a shell model. They are much easier to build than 3D solid models though it does involve more than a single click from a CAD model.

Tata

 

[crisb]

corus: I think this Ansys element is not formulated like a traditional solid element, but more like a shell element, where the corners of the "brick" are used as a lazy way of determining the shell thicknesses. Maybe someone else can enlighten us more?

http://www.kxcad.net/ansys/ANSYS/ansyshelp/Hlp_E_SOLSH190.html

 

[rb1957]

"don't know whether to trust the results" ... run your own tests ... single element, simple loads, ... results you can check with calculations

 

[Drej]

Generally speaking, it depends on the geometry of the "plate". If the structure is truly plate/shell-like then shells (or "solid" shells, like SOLSH190) will give a reasonable response in bending and usually a good pure membrane response. The further away you go from the geometry of plate/shell structures using shells or shell-like elements, then the shell will struggle in bending, usually being overly-stiff. That said, the global response (eg from a dynamic perspective) will usually be reasonable for low-order modes, but it is local strains owing to bending that suffer from accuracy using shells in this respect.

Your best bet is to test, test and test again (as said) against simple benchmarks for your structure. If in doubt - and if practicable - go with solids for bending-dominated problems that are of questionable shell geometry. If the problem is non-linear, then consider using multiple solids through-thickness, preferably hexehedrals. Three as an absolute lower limit, and anything upwards of this if possible/practicable. Avoid single order tets like the plague for stress-related problems, and always use plenty of higher order tets where possible.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[ESPcomposites]

I agree with rb1957.

Do a test to prove that the FEM can replicate the classical solution you find from a reference.

These types of special elements can work well, but can also introduce some unknown issues if you are not familiar with them.

The basic elements should work just fine. The only exception I can think is if the b/t ratio is low then the transverse shear stiffness will have an effect. It is more significant in composites though. You would need an element capable of accounting for that, but again you would first want to check the results with known solutions.

Brian

http://www.espcomposites.com

 

[JohnyGluebag]

See attached PDF, discusses the use and performance of the SOLSH190 element.

Ansys 12 allows you to layer the SOLSH190, so you can get 3 elements thick on a plate if needed and keep mesh size down (rather than using SOLID186).

How well this works I do not know, I have not gotten around to setting up some test runs.

See the benchmarks provided in the Ansys help file, they will show how the element performs compared to some hand calcs.

____________
JohnyGluebag

 

[JohnyGluebag]

oops, I do not think the attachment uploaded.
here is the link to the SOLSH190 discussion

http://www.ansys.com/events/proceedings/2006/PAPERS/22.pdf

____________
JohnyGluebag

 

[Jacques28]

Thanks everyone for your response.

Thanks especially JohnyGlueBug for the link to the paper. Very informative. Looks like Ansys are onto a good thing with the Solid shell element.

I did run my own model for the first round of analysis which were linear static. Here the contractor used Nastran with Shell elements which I could check easily with my program (Strand7).

It was discovered that the structure needed to be embedded (or partially embedded) in concrete to withstand the pressure. At this stage a new contractor was bought in and the analysis change from a linear static to a nonlinear contact analysis (using Ansys) which I afraid to say are basically beyond the abilities of my program.

 

[IDS]

At this stage a new contractor was bought in and the analysis change from a linear static to a nonlinear contact analysis (using Ansys) which I afraid to say are basically beyond the abilities of my program.

You can do a non-linear contact analysis in Strand7.

Doug Jenkins
Interactive Design Services

http://newtonexcelbach.wordpress.com/

 

[Elabbasi]

I did a search on Strand7 and it seems that it only supports point contact elements. If that is the case, then it is quite restrictive.

Regarding the original question, I personally find the SOLSH190 element to be very useful. Only slightly more expensive than traditional shell elements for thin shells and considerably more accurate for thicker shells, and cheaper than a very fine solid mesh. Just as mentioned in the interesting presentation posted by johnyGluebag.

As mentioned in the above posts, you should make your own test though. The purpose of these tests will be to verify that you are using the element correctly and that it is suitable for your model (not that it functions properly, because this is a heavily tested element with a good formulation).

Nagi Elabbasi
Veryst Engineering