Not sure which way I would start either... Might help if you grouped things in to folders in the feature manager tree... i.e. things that only are for one config. all go in one folder, with the parts common to all configs in a seperate folder. That way as you configure parts to suppress based on the configuration they will be easier to find. Everything in this folder should either be suppressed or unsuppressed.
That will help alot...good luck stay sane!
How you proceed should be determined by your documentation standards.
If your two different uprights are controlled by a common revision-like the dash numbers in a tabulated drawing, you are probably better off creating them as configurations of the same file. If they are seperate part numbers, revised seperately, then you should create seperate files for them.
With regard to your weldment: First, I'd recommend doing the weldment tutorials and then using what you learn to define your frame.
However, if you're already progressed in your project and committed to doing it as an assembly I recommend inserting your existing and off-the-shelf components into a blank assembly. Use mates to establish the known relationships between those components in the final design (minimum clearances, alignments, contact, etc.) Use envelopes so that you can position moving componets at the beginning and end of their ranges without affecting the mass-properties or BOM
Following that, create a 3D sketch that defines where everything that's not already securely mated goes. You can then mate the remaining components directly to the entities of the sketch. Create planes and axes from the sketch entities to assist in defining where your components land.
Now create new parts in the context of the assembly using a combination of the existing components and the armature sketch to define your new geometry.
For assemblies made of complex components with lots of features, I'll create those as a multi-body part and save the individual bodies out to seperate files when I'm done.
Weldments are usually made of simple parts with few features so it's probably a good idea to have only one body in a given part file.
Finally, you're going to insert the componets that are 100% dependent on the new geometry for their locations-things like fasteners, hardware and the like.
At some point, for the sake of re-usuability you should go ahead and break the external relationships between the components and the top level assembly and replace those with relations to sketch and reference geometry within the individual part files. We do that before releasing documents for production.
Hope it helps.
holly cow, i have two base frames, one is suqare the other is offset. i have two sets of uprites, one is 2x2 structural l and the other are bent sheet metal. then all the other brackets get put on. i need a drawing to send to the fabricator to get quotes on 1; using the structural vs bending, 2; welding the entire assembly or bolting it together, basically i need a drawing for each configuration. right now im trying it starting with one of the common brackets. i was able to configure the model with the two different base frames and the two uprites. i thought i had it untill i atarted putting in the other brackets, then the mates get turned off and things can move. so with the two frames and uprites im good. i dont know why adding other parts is causing problems.
so whats happening now is when i add a part, i have to go to each configuration and either fix the mates or put new ones in. is this normal or am i doing something wrong?
there is an option when you create new configurations to suppress new mates...
I find it sometimes helps to put in all of the common parts and mates. then create one configuration and those mates and components. then go on to the next configuration.
hope that helps...I'm responding on my phone so soory if it's brief.