SolidWorks Simulation tries to interpret how you want to go about analyzing the geometry by how it was created, but you always have control over that by changing its behavior; a right-click on the body in SW Sim you can choose "Treat as (Solid)," for example. I think that once you understand what it is doing then you can know better about how to create your analysis-ready geometry.
If you create X, then SW Sim will think you want to do it as Y:
X= extruded solid bodies; Y= solid mesh
X= sheet metal solid bodies; Y= shell mesh (thickness automatically defined)
X= surface bodies; Y= shell mesh (manual thickness definition required)
X= weldments; Y= beams (automatically defined cross-sectional properties)
It makes sense because solid bodies typically are stout complex shapes typically best handled by a solid mesh, but if instead it's a solid of a long extrusion that you want to analyze as a beam, then you can change it to treat it as a beam. You can also select a surface of a solid extrusion and define it as a shell mesh with a manually defined offset (in 2011 at least). Sheet metal bodies typically are thin and thus have a high aspect ratio, so they are best handled by a shell mesh; again if you don't want this you can treat it as a solid. And the other types follow the same idea...
Now I haven't answered your exact question based on your example model, and to answer it on a model so small and simplified would not do it justice, so I will answer based on how your geometry might actually be. First it would be incorrect to do this model entirely as beams where the geometry was done in the weldment environment; the fillet welds cannot be modeled as beams and in fact should not be modeled in the simulation at all. It is my feeling that a full beam analysis model is most useful for preliminary mock up of a design where you want to work out the placement, shape and sizing of welded support structures.
I would handle your problem instead as shells for what would be, I'm guessing, long thin plates. My preference is to model these as surface bodies done at the mid-plane of each body (this is the theoretical definition of a shell element); extend the surface bodies so that the edge touches the face of another surface. Again the welds would not be modeled at all, but with a shell mesh you can define edge weld connectors to join them. Edge weld connectors are useful for properly sizing welds by determining the forces and moments at their connections which are used in a post-processing calculation to figure out the weld size requirement. In the edge weld connector property manager, you specify its type, welding standard, electrode material, required safety factor and estimated weld size. Post-processing of the edge weld connector is done by creating a Weld Check Plot, right-click on the result folder and make this selection.
The edge weld connector calculation is based on FE-Weld by Michael Weaver at Weaver Engineering. More can be read about it (PDF): "Determination of Weld Loads and Throat Requirements Using Finite Element Analysis with Shell Element Models — A Comparison with Classical Analysis."
If you are just starting out with SW Simulation, then I recommend the instructor led training available through your VAR. If there is something specific that you'll want to accomplish with Simulation, like the above, please find out beforehand who the instructor will be and ask them to prepare material to show because it may not be part of the standard class. Doing this before the class starts helps so that the instructor can be sufficiently prepared. You can also prepare yourself for training by going through the tutorials, linked through the Help menu in SW (make sure you have Sim add-in enabled and a model open). Alternatively you can launch the tutorials directly from: "C:\Program Files\SolidWorks Corp\SolidWorks\lang\english\cwonlinetutorial.chm" There are a lot of good tutorials on mixed meshes, shells and beams, and some connectors, but nothing I saw on edge weld connectors. Fortunately, I did a presentation at SWWorld 2010 that included an example using edge weld connectors and Gabi Jack had blogged about it.
Thank you for your detailed response. I will be working through it (and the links) more thoroughly and trying out some of your suggested methods when I get the time.
I know that weld simulation is full of pitfalls given the variability of weld depth, thermal effects on the weld and parent material etc. etc. I do quite a lot of simulations of welded fabrications but have always created an assembly and used bonded contact sets. I always state the caveat "assumes perfect full-thickness welds".
I looked at weldments because I wanted a more realistic simulation based on the type of weld because I needed to consider fatigue. As you will know, a full thickness weld is treated very differently from a fillet weld in fatigue calculations. I only have SW Premium so have to estimate fatigue life by reducing stress to a level dependant on the required number of cycles. This is fine if I can rely on the stress results from my simulations. From past experience, I don't think my assembly simulation method has been too far off the mark and I have not yet seen a failure. It is likely that in some designs I may have been able to use less material, but that is a lesser consideration.
Another reason for investigating weldments is that for the assembly type simulations, I have to supress the weld preparations to give a full thickness effect. Big chamfers for a full thickness weld leaves a very small area for contact and is therefore unrealistic.
Thank you again for taking the time - it is much appreciated.
Is there still any difference between an extruded solid, swept solid, or structural member? How is the neutral axis defined in 2011?
I find this topic interesting. I personally have a challenge with neutral axis, and weldements. I have designed a structural steel structure, which when I launch it on simulation, it does not kt connect all my members, where I have beams connected to each other. I realized also that this is happening where my beams neutral axis are not symmetrical. I tried to redefine my neutral axis but I cannot get it to the centre where it would align and be symmetrical with the rest of the connecting beams. This gives me soo much of frustration because Solidworks just keep on crushing now when I try to edit connections. I can upload the file should you require for analysis of my challenge