Making Solidworks references more resilient

Making references to other parts is often inevitable (or else the alternative is much more work). They often cause problems, though, and after some trial and error this is what I've learned:

1. Consider using "Intersection curve" on a solid body rather than "convert entities" with a face or edge. It breaks less frequently because Solidworks can still find where the solid body intersects the sketch plane, whereas some common operations will destroy the face/edge that "convert entities" used to refer to.
2. Avoid splines. Also, the intersection of two curved surfaces or an offset of an ellipse will generally be a spline.
3. You can use "offset entities" on an entire sketch (rather than selecting sketch elements) if it is a single loop. This way, the offset still works even if you add/delete sketch elements.
4. Tongue/groove features on mating edges seem especially prone to breaking. So just don't bother with them (suppress them while you change upstream features) until you're ready to send it out to SLA or whatever.
5. If you define features for a part in the context of an assembly, make sure you that assembly always accompanies that part. As a corollary, if you decide to rename the assembly, do this in Solidworks Explorer, not "Save As...". Otherwise it's very easy for features to become out of context (looks like "-> ?").
6. Try to plan out part dependencies. If you can create one set of independent parts (that define mating surfaces, critical geometries, etc.) and one set of parts that depend only on those independent parts, you can reduce rebuild times and reduce the likelihood of crashing.
7. Fillets on complex surfaces break all the time. Don't reference fillet edges.
8. If you need to make a copy of a surface, "Knit surfaces" fixes small gaps but "Offset surfaces" does not.