Change reference part in sheet or drawing

paul_bunnell

I had a nearly finished drawing then made a change to the model that created two new parts out of some "scrap" area of the first part.  The drawing views all reference "part 1" but when I changed the model, one of the scrap parts became "part 1" and the main object became "part 2." 

When I went back to the drawing I figured "no problem, I'll just edit which part from the studio the view is referencing" but as far as I can tell, that is not possible.  Am I missing something? 

If what I am looking to do is not possible, I would say as a general feature request, any option that can be selected when something is created should be editable after it has been created.

NeilCooke

The drawing is of the body created by Part 1, so if the body for Part 1 changes as in your case, the drawing will update to reflect that. It looks like you are just trimming off the end pieces to make the chamfers bigger? You should edit your original sketch or use Move Face to make the shape you need so that the original body remains. Make your doc public and post the URL if you want more help.

It would not be possible to switch which part the drawing references because each edge/vertex reference would be different and the dimensions would not know where to go.

MBartlett21

@NeilCooke
Is there a possibility of being able to edit the internal ID of parts

konstantin_shiriazdanov

mbartlett21 said:

Is there a possibility of being able to edit the internal ID of parts

At least would be good to be able to select which side of splitting surface keeps the original body and which creates new. As it is now it is really some dark area.

paul_bunnell

The context, in case it helps helps, this is a woodworking project I want to give to some students.  The two "side" pieces were originally going to be waste, but then I decided to use the scraps to create a tent-shaped roof for the boat.  I modeled them the way they would be actually be cut out of a 2x4 and intended to position them using an assembly. 

Here's what the original model and drawing looked like.

Note that the boat is "part 1" in this version but in the broken version "part 1" is the side piece.

This is what the drawing originally looked like

So the goal is to change the now-broken-drawing-refernce to "part 2" so that it restores all the original dimensions. 

The easiest fix would be to revert the main model and make the side pieces in a separate part studio. Nor is this a ton of dimensions to redo, but I could imagine people needing to split a more complicated part into two pieces (perhaps something that is being molded and needs to be split in order to get it out of the mold more easily).  There should be a way for the user to update the drawing reference rather than redoing it from scratch.  @NeilCooke 's point is well taken that altering a drawing reference has the potential to invalidate all the dimension in the drawing, but in this case, the dimensions were already rendered invalid and changing the sketch reference would restore them.  That's something the user should have the ability to do.

Here's a link to the document.

Beshari_Jamal1

I ran to the same problem, I ended up copying a subassembly to put in a larger assembly and didn't feel like redoing all the drawings dimensioning all over again, so voila  

right-clicking then clicking on sheet properties -> right-clicking on sheet tree origin gives you a chance to replace the root part ID, I tried it and salvaged 80% of my dimensions

Shubham_Mishra

Beshari_Jamal1 said:

I ran to the same problem, I ended up copying a subassembly to put in a larger assembly and didn't feel like redoing all the drawings dimensioning all over again, so voila  

right-clicking then clicking on sheet properties -> right-clicking on sheet tree origin gives you a chance to replace the root part ID, I tried it and salvaged 80% of my dimensions

Thanks! I ran into the same kind of problem, I updated my model and now it's two separate parts which doesn't go separately on sheet, it's a composite part, this solution has saved a lot of time! It's not first time, I never knew this!
Thanks a lot!