Extracting piece parts for detail within complete assy dwg

[mbostonsprint]

I have a relatively simple assembly for which I am making a drawing, consisting of a half-dozen parts. I would like to have the complete drawing set as a single document with multiple sheets, but it isn't clear to me how I get back to the initial dwg setup dialog when I add a sheet to the dwg, where I would like to extract the piece parts individually and add their dimensional details. The add-sheet button at the bottom doesn't bring up the initial dialog where I can select full assembly or a part. Any guidance on how this can be accomplished?

[ToddHarris7556]

Once you place the view on the sheet, you have access to the model tree where you can control visibility of individual components within the assembly. 

[ToddHarris7556]

HA! OK, I apologize..... I just realized that when you control the model tree visibility, it affects the entire drawing - every sheet! This is.... horrible. 

To be honest, I haven't yet found Fusion drawings to be usable. I use Desktop Connector to bring Fusion models into Inventor for drawings. 

[ToddHarris7556 · Accepted solution]

OK.... apologies again - I realized the part I was missing:

When you create a new sheet and place the view, in the Drawing View dialog, make sure that you select Create New Reference. This makes the new instance independent of the other sheets/views. You can then toggle visibility as originally stated. 

Happy to have forgotten/rediscovered this.

[mbostonsprint]

Thanks for the input, much appreciated. It works, but I have to say, it's quite cumbersome if there are a number of parts in an assembly. It's an "opt-out" approach rather than "opt-in", and has to be done on each successive sheet if this is the approach one needs to take to keep the parts collection within a single document.

In the "Create Drawing" dialog that appears when you select "New Drawing", there is a choice of Full Assy or "pick the part you want". This would be a more convenient arrangement if it can be made to work.

[ToddHarris7556]

Could not agree more.

Having the drawing tied to one model is a big restriction. There are two main options:

1) Separate drawings for every part. This is workable in many cases. We produce a general arrangement/overview drawing, and then breakout drawings that go to every department for fabrication. The weakness is there's no good equivalent for an AutoCAD sheet set - i.e. when you just want to be able to print a drawing set. We end up using Adobe Acrobat to assemble a whole bunch of sheets into one PDF to send to the client. 

2) One big container assembly, and then suppress parts as needed. At least that way, they're all able to be in the same drawing, but it introduces the challenges that you describe. 

Which..... is one of the primary reasons we still use Inventor to produce drawings.

[TimeraAutodesk]

Another option that will help, is that you can right click on any component (or selection of components) in the model environment and select "Create Drawing", then add that view selection to an existing drawing on an existing sheet, or a new sheet (the drawing needs to be open at the time this occurs).