Frustrating inconsistency with "Edit in Context"

robert_mangas

Hi all, new here, new(ish) to OnShape, not really new to CAD but, er.... rusty, shall we say?


I'm working on a project for a friend and am having a really frustrating time with "Edit in Context". 

Here's the project: https://cad.onshape.com/documents/0f464fcb4e9b648fcc5a0730/w/9472cabe816bdd29cb97b119/e/81d2b98f01d766cbdbeb8c4a ; at this point I'm working on the "Update Bolted" assembly and the PS2-Updates part studio.

The assembly will be bolted, and I had tremendous early success with passing a bolt pattern from one part to another- in this image the two pairs of holes were originally made in "Transom Mount Left" (silver) and then passed to 'Extension Angle Left" (blue) via "Edit in Context".  It worked exactly as expected and generated perfectly matched holes. Cool....




Then I tried to use the same exact technique with the 4 vertically-arranged holes on the other flange, only to fail miserably.  Here's sketch 9 on the inner face of my Motor Mount Board, made by the "Use (Project/Convert)" function on the hole edges from the "Transom Mount Left"



Then I try to extrude-remove using that sketch to drill the hole pattern in the "Motor Mount Board"  Note the input requirement for "Merge Scope"; this was not a requirement for the previous hole transfer/drill operation and is the crux of the issue- I cannot select anything on the screen as my context:



The resulting error is "Extrude 11 did not regenerate properly: No merge scope selected".  

Going back to the sketch that did work, there is a clear difference between the sketches:


...but I'm not sure how I got the functional sketch on the "Face of Extrude 3" while the non-functional one wound up on "Face of Context 2" as I believe I followed the same workflow. 

Where have I gone wrong (as I so clearly have )?


Thanks in advance,
Robert

NeilCooke

It's because you have all the parts in your Part Studio hidden so there is nothing to select for the scope. It only "automatically" selected the part for merge the first time because you sketched on the face of the part. If you sketch on the face of an assembly context (ghosted item) you must select a part for the feature to merge with (you cannot cut a hole in the ghosted part, if that is what you are trying to do - you must edit that part in context).

robert_mangas

Hi NeilCooke, thanks for the fast response.   I'm sorry to say that this answer didn't help (though I'll be first to admit the error could of the 'pilot' variety).

First, the workflow for both operations was the same- edit the to-be-drilled part 'in context' and transfer the hole sketch from the previously drilled part.  Worked great the first time, not at all the second.

Second, I can find no way to "unghost" the in-context part.  I can unhide the motor mount board in the Part Studio but the in-context assembly is in a different position entirely, so that if I select the motor mount board as my scope in the part studio the extrude-remove fails because the extrusion doesn't touch it.

NeilCooke

You might have done this already but you need to go back to the assembly and right-click the part that needs the holes and create a NEW context. This will put the ghosted assembly in the correct place. 

shawn_crocker

Yes. Your assembly parts have probably moved with respect to the origin since you last created the in context reference. Neil is having you create a new one because it is safer then updating the existing one. Updating the existing one may cause your first successful in context edits to fail as they are counting on the parts in the assembly to be where they were before.

robert_mangas

Ha, that was exactly it- thank you very much!  This seems to suggest that the workflow would be then to get the entirely assembly mated before performing this sort of operation, would you agree?