Replace feature with pattern and preserve mates?

[SolidKeke]

Hey,

I think this is not possible but I have to ask anyways...

I want to replace these cut-extruded holes with hole-wizard holes to be able to use pattern-driven-component-pattern in assemblies. Problem is that the part is used VERY much in previous projects and will destroy all mates. Is there any way to tell to this part that the new hole-wizard holes are actually just the same cut-extruded holes so the mates wouldn't get destroyed? Think about replacing sketch-entities in sketch, now just replacing features?

[gupta9665]

No, the face id will change.

Try one thing:

Create a copy of this file and give name to the 2 faces (remember the names exactly for each face). Create a new assembly using this new plate and add cylindrical components using the concentric mate using the 2 holes. Go back to the part and instead of the cut extrude, make the holes using the hole wizard. And then set the same face name as it was earlier. Go back to assembly and see if themate fails. If not then it might work.

[SolidKeke]

Thanks for answer Gupta9665. I gave name to all faces and edges, created copy of the part, replaced cut-extrudes with hole-wizard holes and gave same names to those faces and edges as in original cut-extrude. When I replaced the original part in assembly with the copy, all mates to edges remained correctly but concentric mates to hole's face unfortunately did not survive.

[gupta9665]

....but concentric mates to hole's face unfortunately did not survive.

[Glenn Schroeder]

If it was me, since I'm a one-man operation, I'd go ahead and change them to Hole Wizard holes, and fix the broken mates as needed (I'd fix them whenever I opened one of the existing Assemblies using this Part instead of trying to fix them all at once).

If you're in a multi-user environment you would need to make sure everyone else is aware of it, and what to do if they run into problems. Even if some complain initially I think they'll relent when they see how much better it is to be able to use the feature to drive patterns in Assemblies.

[Frank_Oostendorp]

Change the dept of the cut extruded holes from "through all" into "Blind" with a dept of 0,05mm or something very small. After that, add the hole wizard holes, but don't let them take away the original face of the first holes. It might be needed to enlarge the first holes to get these a bit oversized.

[bnemec]

Thanks for answer Gupta9665. I gave name to all faces and edges, created copy of the part, replaced cut-extrudes with hole-wizard holes and gave same names to those faces and edges as in original cut-extrude. When I replaced the original part in assembly with the copy, all mates to edges remained correctly but concentric mates to hole's face unfortunately did not survive.

That's same as what we saw trying to name geometry doesn't do what it looks like it does.

What you speak of is very normal in our day to day product dataset maintenance. We also looked into if there was any way to get this to work for all opened assemblies, but we found it does not. I just tested again to check my memory. But we're still in 2019, maybe they've added it to update mates in all open assemblies in later versions?

I did some digging in Solid Edge to expose the geometry IDs referenced in mates (relationships) was going to create an index of "geometry where used" so we knew the impact before editing the part, already had index of file where used. But they keep that geometry ID stuff hidden away, I don't recall if I gave up because I failed to find the data or gave up because we thought PDM would be worth converting to SW...