How to handle broken references when modifications to a part studio cause named parts to be renamed

james_howard360

Working in a part studio with 3 parts whose geometry is interdependent. All part are used as derived parts in other part studios and in assemblies of the same document. A named part that we'll call 12345 needs modifications that involve split and boolean operations. On boolean, OnShape creates a new part called 'Part 2', and 12345 is lost. No big deal, I can rename it, but then everywhere 12345 was used is a broken reference. Renaming 'Part 2' back to 12345 does not fix the references. How can I tell OnShape to keep the reference, or how can I quickly update it across several other part studios and assemblies?

konstantin_shiriazdanov

This Assign identity feature may help. Though I don't know if it works with part names, but at least it works for automatic substitution of assembly references when you change part selection in the identity feature. It's what @lana gave me when I argued that I needed a persistent identity container, so this is probably some intermediate solution to this problem from OS.

ilya_baran

It may be possible to change the order of parts in the boolean so that 12345 is not lost -- for a boolean union, the part identity stays with the first part selected.

S1mon

@ilya_baran

This concept of ID being driven by the order of the references is one that I've known for so long I almost forget that I had to learn it. It was painfully true when using surfacing in Pro/E, and there are similar issues in Solidworks and Onshape. It seems like something that should be more emphasized in training and documentation. In a perfect world you don't really have to think about it, but the reality is that feature trees blow up when you make changes. If you don't have the right mental model of what's going on internally, it's easy to do things that are very "brittle".

In general, I've learned to try and keep all of my references to a minimum and make them to the most immutable thing that makes sense for capturing design intent.

EvanReese

in this case I agree that just re-ordering the boolean queries, but wow I didn't know about the Assign identity feature! It seems really powerful, and maybe a little dangerous if used willy-nilly. I tried it out and got some cool results, but also strange ones too. For example, If I assign a new ID to a sketch curve, then try to extrude it, I can't anymore because the extrude feature can't find the sketch plane. I did, however, get ruled surface working for both, and a split across the resulting face doesn't fail when I switch between them. This could open up some cool options for me.