Salted Fish wrote:
Is there a way to force SolidWorks not to do this? Or break the dependency? This seems completely stupid: if I make a drawing for a particular part, I want that part to always be visible even if I've hidden that part in the assembly. Why would the drawing be dependent on the assembly in this manner? What use is a drawing to me if I have to constantly open the assembly, "unhide" everything in the assembly, then reload the drawing? I find myself hiding and unhiding parts in the assembly as a way to focus on certain features and derive relationships between parts while setting up parts on machines.
Drawings are always dependent on the model, so anything you change in model would be reflected int he drawing.
For your needs, you either need to use display state or configurations in the model and then use them in the drawings. This way everything would be just like you want
First of all, you'll get some argument about your statement "This seems completely stupid". That's how Solidworks has always been. If you make a change to a model, that change will be reflected in any drawings that reference that model. I wouldn't want it to work any other way. It's not the fault of the software that it doesn't work the way you think it should.
Now that I have that out of the way, you have several options. You could use either display states or configurations, as Deepak Gupta and Brad Meador have suggested (of those two options I'd prefer display states). However, you have another option that might work better in your situation. In your Drawing, right-click on a component in an Assembly view and choose "Show/Hide > Hide Component".
That will hide that component in that drawing view, but it won't affect the model, or any other drawings or drawing views that reference the model. If you want to hide multiple components you can Ctrl+select them before right-clicking and hide them all with one operation instead of doing them one at a time.
I make configurations because sometimes (many times) I need to show how this group of parts fits together in context of the next level so I have a drawing config and I have an assembly config. The assembly config reports to the PDM.
Thanks all for the responses, looks like Display State is what I'm looking for!