Mesh singularity on non-manifold geometry

[IcarusAero223]

Hello everyone!

I'm modelling a composite wing and am exhibiting a mesh singularity at the spar web/cap connection.

Solutions I've tried:

1. Modelling softer boundary conditions through springs
2. Reducing the stiffness of the spar webs
3. Pulling out spar web surfaces and modelling BC's through idealized bolted contact

One of the options is to ignore the singularity by averaging the stress in n amount of elements before the singularity by measuring and graphing which I did, but I'm not so sure how accurate that would be as per my lack of experience.

And as you can see none of it really worked so I decided to come here and see if anyone has an answer to this little problem I have.
I'm assuming the fix might not be the modelling approach but rather geometry modification and for that I have no more ideas unfortunately.

Any help is appreciated!

 

[FEA way]

You could use submodeling or shell-to-solid coupling to model that small region with solid elements and including some fillets thus obtaining more realistic result.

 

[IcarusAero223]

You could use submodeling or shell-to-solid coupling to model that small region with solid elements and including some fillets thus obtaining more realistic result.

Thanks for the suggestion FEA way.

As the wing is supposed to be optimized later in regards to ply thicknesses and orientations, using any solid elements might not be the most ideal solution.

Could the problem be in the mesh connectivity? I did check for free edges and it seems OK at the moment.

And one important thing to mention is that the wing is fixed at the root rib.

 

[FEA way]

As the wing is supposed to be optimized later in regards to ply thicknesses and orientations, using any solid elements might not be the most ideal solution.

There are also composite sections for solid elements so you can use layups with them. This is often used e.g. when analyzing nozzle regions of composite pressure vessels.

 

[SWComposites]

And one important thing to mention is that the wing is fixed at the root rib.

that is likely the cause of the stress peaks at the spar web at the root.
but you have two lugs at the root of the spars. how exactly are you modelling that area? note: you are unlikely to get accurate stresses in those lugs with the current mesh refinement, and since the stresses in the lugs will be highly influenced by pin contact and tolerances and such, getting an accurate FEM there is near impossible. Rather you should be analyzing those lugs with classical lug hand calcs.
And if those lug are composite materials, then you better have some test data to validate any strength predictions (I've been deep into that mess before).

oh, and why are you looking at Von Mises stress for a composite material? VM is a metal yield criterion. DOES NOT work for composites. Use max fiber strain failure criteria (the composite text book lamina strength interaction criteria also DO NOT work).