Great post Gordon! This (3D CAD) is all like trying to eat an elephant...
As you mentioned (& others) you might be better off designing all the individual parts & then later creating an assembly file with all the parts in it. I wouldn't worry too much about using the simulation & collision detections if you're just trying to learn the software, get the basic workflow down first. I'm a Pro-E/Creo user & when I was learning to use the software (at work, designing tooling...) I bought a couple books (SDC publications, many years ago, I'm not sure if these are available for Alibre, but I'm still "old school) & would rather have a book in front of me rather trying to pick out all the commands in a YouTube video. I also started drawing up "proven designs" (Very simple ones), mostly Elmers engines or simple oscillators just to figure out how to use the software, one part at a time. I then figured out how to do the simulations, ETC. Because a model with lots of parts gets very ugly if you screw up the "assembly connections" & will make you want to give up (but don't). After doing some simple models, you will see what is required to set up BOM's & create some good working drawings.
After you've gotten to this stage, you'll probably have built some engines (I know you're a good designer).
&, after you've reached this point you'll start pushing the software a little more.
I "Think" Alibre (& other softwares) have this function, but you can create a new part within the context of an assembly to use existing geometry as references. The reference was made earlier in this post about if you change the "size of a crankshaft journal" you would have to remember to accordingly change its diameter. Well, If I create the bearing in the assembly context (This becomes it's own stand-alone part) of the assembly, & use the crankshaft diameter as a reference, I use that diameter & offset it by say .001" off that dia. for the bearing, that bearing will update accordingly & ALWAYS give a clearance of .001". If I change that dia. (Crankshaft) by 100" or .003" (extreme example, but it works), it will always maintain a .001" clearance.
Constraints are REQUIRED. In my last example, if you did not use them, you would find a lot of problems, especially "downstream". Parts MUST be FIXED, with the exception of "mechanism" parts. This technique also works for bolt patterns in assemblies. A couple of examples, if I assemble a crosshead part to my cylinder (That already has the bolt pattern, & orient it correctly, I can (in the assy. mode), "activate" my cylinder & use the bolt pattern to create the tapped holes in the cylinder (using the axes of the crosshead). If done correctly in the crosshead & the holes were created using a "pattern", I only need to create ONE hole in the cylinder & then use "Ref. pattern" to copy the holes EXACTLY to the crosshead. This doesn't matter if it's 6 holes or 60, it will ALWAYS follow the "Pattern" of the crosshead & I don't need to do the math.
'cept maybe the tapped hole size...
Importing ACAD 2D sketches into 3D has always been a bugger for me, lack of "good" geometry (open ends, non constrained. polylines...). I've given up doing that & just re-create it in my 3D sketcher.
Another note about creating the 2D sketches to create 3D geometry... don't over complicate sketches. If I create a piston, I "Revolve" my piston dia. & that's it...I create the ring grooves as another revolve feature (this all goes back to constraint's & dependincies. For instance, if I want to modify the ring grooves from the piston, I just need to edit that particular feature without touching the piston sketch.
Phewww...
Don't be overwhelmed Gordon, but start with the easy stuff.
Plenty of well qualified help here to help you on your journey...
JoHn