Hello all. I will be starting a new project in the coming weeks and would like some insight into the best method for designing a complex sheet metal assembly. In the past I have typically worked with simple assemblies where there have not been more than 5-10 parts, for those types of design the bottom up approach is not too cumbersome. However, this will be considerably more complex. I have experimented with multi-body sheet metal parts and have had good success. But I think thinks could get challenging. Any thoughts on what the best approach would be. It is also worth mentioning that I will be using simulation to verify the assembly.
If you are goin tu use Simulation to verify your design (or to optimize) then I will recommend you use a Top-Down method, having all dimensions, thickness, bendind radius, etc, driven by skecthes you will be able to create a Design Study to perform an optimization or evaluate specific scenarios of your design. Our work require very large ans complex assemblies made over 90% of sheet metal parts, and that is the way we do them.
Some tips:
Do not mate any parts using part features (surfaces, edges, holes, etc.), allways mate parts into the assembly using parallel mates to two planes and coincident (part origin to a point on a sketch).
Do "referece geometry sketches" at the top level assembly, use "referece geometry sketches" at sub-assemblies (related to sketches at the top level assembly) and create sketches at the part level related to the sketches on the sub-assembly containing the part.
Link "thickness" (after unlinking the global variable automatically created by SW) to a vector or dimenssion on a sub-assembly, or assembly sketch, (also do the same with the bending radius), that way you will be able to change thickness of parts by changing a value at the assembly level (if needed to optimize the design, and to use that variable on the "Design Study" in Simulation.
Holes for fasteners joining two parts should be define on sketches at a level on top of the two parts, then convert those sketch entities into sketchs inside the part, this way if you change number of fasteners (holes), size or position, they will change on all parts joined by the same fastener.
When creating parts, try to define all sketches on planes, not on sufaces, remember that Sheet Metal surfaces move when you unfold bends.
Try to model parts using a "symetric" concep when possible (modeling half part and them doing a 'mirror" of the body).
If you are modeling large Sheet Metal parts to analyze with Simulation, model them to be able to use Shells, a solid mesh on a large sheet metal part take for ever and sometimes fail unless you use avery fine mesh which will take even more time to process.
There are many other things to consider.... but you need to start on something...