Best FEA/modeling for solid/shell combinations

[RobertCasey]

Hello. We are a small company that designs amusement park ride structures and mechanisms. Up until now we have outsourced all our FEA work, but now we want to bring this in house. We are using SolidWorks 2006 but recently we have been investigating the upgrade to SolidsWorks 2010+Simulation. A lot of our FE models are combinations of solid and sheet metal parts, and we want to make our FE models from block and shell elements respectively. Having played with SW2010+Sim, it appears to me that it is rather weak in this area, especially when it comes to joining the parts and maintaining mesh continuity between them. To do the work properly requires split lines to be placed on the parts which can be quite labourious (I believe that another SW client that also has this issue employs a 'split line lady' to do this work full time :S).

We would still like to upgrade to SolidWorks 2010 - we looked at migrating to ProEngineer/Mechanica but we think that this would be too much of a 'year zero' issue for us with regards to modeling and draughting.

Therefore the question is if anyone has experience of an FE solution that integrates well with SW so that we can update models and have this quickly reflected in the FE model, and which is more capable than SW Sim when it comes to combining shells and solids, and which is (as always) not too expensive.

A modular system would be excellent so that additional functionality such as non-linearity can be added if and when needed. Thank you.

 

[johnhors]

Robert,

I hope that you are aware that mixing solid and shell elements is not best practice, as the two types are incompatible. They have different degrees of freedom at nodes and of course have incompatible shape/displacement functions.

Nodes of solid elements have translational degrees of freedom only, (no rotational degrees of freedom). Thus when you join shell elements along a line of nodes on the solid elements, these shell elements are free to rotate or "hinge" about the join line.

Just saying you need to be cautious and also be aware that stress results at and near the join should be dis-regarded.

http://www.Roshaz.com

 

[gwolf2]

I agree with johnhors, shell/solid stuff is for when you really know what you are doing. It's not impossible by any means but the stresses at the interfaces need a LOT of care when assessing.

 

[RobertCasey]

Thanks for the tips guys and it is indeed an effect that I have noticed with some of the results from the specialist company we use. They have never told us that there could be issues with the stresses calculated in the joints which is somewhat disappointing. It could well be a question of the blind leading the blind...

If we had the processing power we would model everything as one or the other - I tried that during our trial of SW Simulation, but to get a mesh fine enough for the thin metal plate took far too long to process given the size of the model. Its not practical with the systems that we have.

We are analysing vehicle chassis which are fabricated from bent plate members and stiffeners which are welded to various solid steel blocks. Can you suggest a better way of modelling this sort of structure?

 

[gwolf2]

The key to it is getting the stiffness of the 'lumpy bits' correct so that they attract the correct amount of load. One then uses hand calculations and/or detailed FE sub-models to find out what the stresses are. Make lots of small test models too.

 

[RobertCasey]

Would it be possible to 'embed' the nodes at the ends of shells so that they are bonded with the nodes of the solids at the interface? There will still be no rotational DOF but would the connection of the displacement DOFs provide a better way of tranferring out of plane bending into the shells?

 

[johnhors]

Robert,

What you suggest sounds reasonable and as good as any, assuming you mean that you are burying the shell elements into the solid. There is no "magic" correct solution to this problem.

http://www.Roshaz.com

 

[RobertCasey]

Yes, burying several "rows" of the shell nodes into the solid and ensuring that the nodes of the shell and solid are connected.

As you say, its not a magic fix but at least there should be no hinge between the parts.

The thing is, coming back to my original question, what would be a good package that would be able to able to do this sort of manipulation? Im sure as anything that Solidworks Sim isnt up to this sort of thing in any easy manner.

 

[gwolf2]

> Would it be possible to 'embed' the nodes at the ends of shells so that they are bonded with the nodes of the solids at the interface?

Yes, it works. What thickness do you give to the embedded shells?..................... Small test models.

As for the package which lets you fool around like this, the big, CAD- based ones which I have seen don't give you that kind of wierd flexibility. Enter PATRAN stage left, again :-( I've done loads of this stuff with it but feel reluctant to recommend it any more because it's too buggy and out of date.

FEMAP will probably do it too these days. Ask them for a 1 month limited node licence and see how you get on. You can do this for all the packages before you buy.

 

[gwolf2]

There are far too many tips and tricks with this sort of modelling to list here. We can only really guide you in the right direction and suggest strategies for your own learning path.

 

[TERIO]

ANSYS (and other codes also probably) has what it calls a solid shell element, which is a 8-node solid element (only displacement dofs) that has a special formulation that makes it work better in bending than normal solid elements and then you don't have the dof mismatch when connecting to solids elements. I haven't tried it myself, but it may be something worth looking into.

 

[RobertCasey]

Thank you for all your tips! I have booked onto an Ansys workshop and will get a 30 day free trial. I think i need to dig out my old FE university notes too...

 

[BlasMolero]

Dear RobertCasey,
Please check

http://www.realfea.com/,

you will see the list of FEMAP & NX NASTRAN distributors around the world, my suggestion is to contact with the nearest distributor to ask for a demo session of FEMAP & NX Nastran, forget at all the use of 3D solid-only FEA packages, the type of problem you describe must be setup using DOMINANT SHELL & BEAM elements, here FEMAP is really powerful, you can import the 3D CAD model and built in FEMAP the 1-D & 2-D Finite Element model based in the 3D geometry, very fast & reliable.

Best regards and good luck!,
Blas.

 

[JohnyGluebag]

PADT has posted several blurbs about solid-shell connections in there newsletter called 'The Focus':

http://www.padtinc.com/epubs/focus/2008/0066_0804/TheFocus_66.pdf#Page=1

http://www.padtinc.com/epubs/focus/default.asp

They use Ansys but you should be able to take something from it.



____________
JohnyGluebag

 

[RobertCasey]

Very interesting read, thanks! Our local Ansys agent has arranged to come to our office to demo the package using our CAD files, and especially with handing solid/shell interfaces. Looking forwards to it!