@TrippyLighting wrote:
If you create the sketch for component 2 on the geometry of component 1 then that creates a relationship between the two components (as @chrisplyler has pointed put in his screencast). So when you change component 1 it still might change component 2.
Yes. I failed to mention this in my screencast, but EVEN IF you don't create any in-sketch relationships (intentionally or otherwise), you have still the relationship created by the fact that you began the sketch using a face of geometry instead of a stand-alone plane. Since you associated the sketch to a face of geometry, the sketch will MOVE with that face of geometry.
So in the case of this thread, the Steel component would move up and down if you change the thickness of the Aluminum component. It wouldn't get messed up, but it would always stay on that face.
Now sometimes that's what you want, so no problem. But sometimes it isn't what you want, so you should be aware of how that works. If you don't want that to happen, you make a new plane offset from the origin instead of based on a geometry face, and you start your sketch on that plane instead of on that face.
To TRULY keep components unrelated, I prefer to build each one on its OWN origin, and not necessarily "in place" where it belongs in the assembly. Build it completely unrelated to any other component. Then use an assembly Joint to put it in the right place/orientation. Now in this way, the component isn't dependent on anything else in the assembly. It could be exported out and used in a totally different assembly file, and only require a new Joint be defined. If you try that with your Steel component, with it's sketch location depending on a face of another component, then you can imagine that it would go screwy if you tried to export it out to exist on its own. It would be wondering where the heck its sketch belonged.
