Now for top 3 different cases, though the stress are aprox similar, but the Plots are kind of different.
I suspect that the difference in the stress gradient is in part do to the mesh quality and in part due to a non-ideal geometry for shell elements, rather than a difference between solid and shell elements. Results from linear and quadratic triangle elements are notoriously poor, and require a high density mesh to get decent results when compared against tets. Shell elements should also be limited to, in general, geometry in which the thickness dimension is at least 1/10th of the shortest non-thickness dimension; in your example, this does not look to be the case. Finally, a true comparison needs to be made against a converged set of results.
So Please let me know as we are sure that solid mesh is perfect solution but which is the best option to choose for mixed mesh.
I wouldn't say that solid elements are 'perfect', they just contain more information that shell elements. Shell elements make an assumption about quantities through the thickness (such as stress) whereas solid elements don't. This is why shell elements are usually limited to 'thin' structures.
I always go for connected surface and solid face. As bonding option is automatically taken when two faces are coincident. But the issue with it is whole strcuture height changes.
There will be slight variations in the results, as you're changing the placement of the elements with respect to the result of the structure, but it's typically not that large as the geometry with shell elements on it should be 'thin'.
But in case of distant faces, we have to provide manually contact option but structure height remain same. So please let me know ur suggestion.
It really depends on the geometry of the structure, what you're simulating, and the results that you're after. If you feel that the offset of 1/2 the thickness of the part is large enough to cause significant error, then you should be asking if shell elements are appropriate. Also keep in mind that you can model an object using solid geometry and still mesh it with shell elements (such as an object made using the sheet metal add-in), so (I think) a default bonded contact will still remain valid even after you've compressed to the mid-surface. Also keep in mind that a bonded connection between solid and shell elements are inherently inaccurate, due to the multi-point constraint equations that the software package sets up to resolve the nodal compatibility issues that exist between the two element types.
Also when we use bolt connection between this kind of arrangement i always get this warning message, should I ignore that. Please advice.
No, you shouldn't ignore it; that error was put in there for a reason. There's be several other posts on this form site about this error that are worthwhile to read.
i'm trying to synthesize your questions
i think you're asking:
1. can you compare shell and solid solutions > the answer is yes, if they are setup the same, and look at displacement to start, worry about stresses later, remember that shells report stresses differently, effect of singularities..etc.
2. is the solid solution the "right solution" > less approximations/assumptions maybe, but from a simulation accuracy, if shell is setup the same and you follow "the rules", they will be the same
3. where do you put the shell > look at the information i've linked below. to match the solid, the shell should be a long the middle. so unless you create the surface yourself, to get it to match you need to use the offset option. but again for shells we assume they are very thin, so the offset is minimal.
4. bolt error > you should not ignore it, read up on it in the solidworks KB. you need a different approach if you need to use bolts.