How to hide features in assemblies?

Unfortunately there is not a good way to do it. I usually either make a sub-assembly to do my welding and then a top level to do my machining or, if my machining is complicated, I will use assembly for welding and merge all my components in to a single part to do the machining.

Neither way is an ideal solution.

We do use the merge method a lot since we do a significant amount of post welding machining that would be 'difficult', to say the least, using assembly features.

I prefer making 2 assemblies/drawings; one for the welded assembly and the second for the machining.

My reasoning is that we can sub-out the weldment to one shop and then have the machining done in-house or some mixture of where each level is done.

It has worked out well in the past, once I convinced engineering management to accept the 2 drawings as the preferred way to structure the drawings.

I'm not sure if this is possible, but perhaps you could make an assembly family table, add the features you want to exclude, then use the appropriate version of the assembly for the particular view you are making. I.e. the workflow is:

(1) Make the family table instances, turning on/off features as needed.

(2) Create the drawing.

(3) "Add Model" for the instance you want to use in a particular view.

(4) Create the view, it should reflect the configuration you want.

(5) If you want another view, "Add Model" the next instance, or "Set Model" to the one you already have included in the drawing, create the view, etc.

It's kind of clunky, but it works. You might have to align adjacent views if you want them to be related the way they would be if you were only using one model.

I haven't come across a way to have an assembly represented both ways in a single file. Assembly cuts result in hidden family tables, so I always am amused when blanket rules against using them come up. Family tables or not, there will have to be multiple assemblies involved to get the desired result.

I agree with the approaches that Stephen and Ben have suggested. To calculate the appearance of multiple states there need to be multiple models. I assume the reason that assembly simplified reps do not include assembly cuts is that the book-keeping would result in making family tables of family tables - the original cut is added via a dynamic family table for each component and hiding it would require a family table of each of those where it's suppressed. Explicit access to the hidden family tables would end up in the ordinary family table structure anyway, so you'd still be stuck.

You can merge the welded parts together into a single prt. file. In this part, you can do the machining as well as make a simp rep, since it's a part file.

You will find the merge function on: Model tab > component > component operations > Bolean Operation

NB! You will need to make a (empty) part file first and assemble it in the main assembly, so that all the assembly parts can be merged into the new empty part file wich you will be using from now on.

Not sure if that helps any, but just wanted to add that you can make your assembly level cut visible as a feature in the sub-component part being cut (see the "Intersect" tab in the definition of the assembly level extrude feature).

Then in that part, you can define a simplified rep which has the cut feature excluded...