Copying/Moving Drawings to Different Documents?

Oliver_Lax

Hi,

I am trying to move (or copy) a number of drawings along with the referenced part studio/assembly into differnet document as part of a clean up job. However whenever I do this the moved/copied drawing loses it's reference to the moved/copied part studio or assembly. This means I cannot update the drawing if I want to change the part or assembly, which means I would have to redraw all these parts. Is there any way to:

• Re-reference drawings back to the right part studio/assembly?
• Keep the references in check when copying/moving the drawing?

Thanks!

philip_thomas

@Oliver_Lax - That should absolutely work as you describe and we just tested again here.
You are a Pro-User, please submit a support ticket and we will take a look!
Thank you.

hailong_li

Hello Oliver,

If you use 'Copy' to copy a drawing, it copies the drawing as well as the referenced part studio/assembly, which means the copied drawing has a reference to the copied part studio/assembly, not the original part studio/assembly.
If you use 'Move' to move a drawing to a different document, it moves the drawing as well as the referenced part studio/assembly to that document and it maintains the references between the drawing and the part studio/assembly. The drawing and the part studio/assembly that are being moved will no longer exist in the original document. 
It sounds like 'Move' is the command that you should use. If you find the behavior is not what you would expect, please give us more information to describe what the problems are, or you may report a bug so that we can do a further investigation on your case.

Thanks
Hailong

philip_thomas

@Oliver_Lax - That should absolutely work as you describe and we just tested again here.
You are a Pro-User, please submit a support ticket and we will take a look!
Thank you.

hailong_li

Hello Oliver,

If you use 'Copy' to copy a drawing, it copies the drawing as well as the referenced part studio/assembly, which means the copied drawing has a reference to the copied part studio/assembly, not the original part studio/assembly.
If you use 'Move' to move a drawing to a different document, it moves the drawing as well as the referenced part studio/assembly to that document and it maintains the references between the drawing and the part studio/assembly. The drawing and the part studio/assembly that are being moved will no longer exist in the original document. 
It sounds like 'Move' is the command that you should use. If you find the behavior is not what you would expect, please give us more information to describe what the problems are, or you may report a bug so that we can do a further investigation on your case.

Thanks
Hailong

brucebartlett

If you want to go a step further and have your moved drawings reference the original doc you have to change the links on the part in the drawing to reference a version in the original doc before moving. This is only if you want the part studio to remain in the original. This may be useful for example if you want to share a drawing with a vendor in a clean document, referencing a specific version without the part studios and design details. 

For document cleanup sometimes I have found I have to do a double step move as part studio end up where I don't want after moving a drawing, so I will then move them back to the original position, feels bit dangerous with links and history all getting crossed up but Onshape seem to handle this very well. 

Oliver_Lax

Thank you all for your help! I have just tried it again and it worked fine... Not sure why I was having the problem yesterday but it was almost definitely my fault. Thanks again.

romeograham

I just ran into an interesting case when moving / copying drawings.

I have a Document where I have a bunch of Drawings, Parts, Assemblies. All for tooling for a certain sized product. All my drawings reference Revisions of their parts (as has been described elsewhere as good practice).

NOW

I want to move all these parts, assemblies, and drawings out to their own document, and then make a copy, so I can start working on the tooling for a different-sized product (after creating new part numbers, and updating all Properties etc).

HOWEVER

When I Moved all the Drawings, Part Studios, and Assemblies out to their own Document - the Drawings still retain their reference to the Released parts in the Source Document (as they should!). But now, if I want to "Change to Version" in the drawings, to associate them to the local copy of the Parts, I can't. There is no option to select a Part from the local Document, only options to change Versions / Workspace in the source document.

Since we can't REPLACE references in Drawings, this means I have to import a new view of the local part, and totally recreate the drawing with the new part, then delete the original parts, update the Sheet reference etc.

As described above, when moving a drawing that references a current part from the same workspace (un-Versioned or -Released) the new drawing retains the reference to the new, local part. As far as I can tell, if the Drawing references a Revision or Version of a part, Move and Copy give the same result: the new drawing references the old part, and you cannot update it to the target reference without recreating the drawing.

TO GET AROUND THIS, THIS IS A PROPOSED WORKFLOW
Source Document

• Create a Version (to give something to come back to later) (OPTIONAL: create a Branch to work in so you don't need to do the Restore step below)
• change all Assembly and Drawing References to the Current Workspace instance of each part
• Copy / Move Drawings, Assemblies (and associated Part Studios) to new Document
• Restore Source Document to Version (only if you made a mistake...if you are successful, your drawings no longer exist in this Document, and doing a Restore would make them appear again!)

Target Document:

• Check / Ensure all references are local
• If this is a Copy: Update All Part Numbers (so that Releases don't contaminate your other document), change Properties etc
• If this is a Move: begin to work on Parts, 
• When Releasing Parts / Drawings from your new Document, you'll have to update the Drawing reference to the Revision of the part again...but you can't do this until after your first Release from this new Document. Thankfully, the Drawing's Revision History seems to be retained through the Move.

Unfortunately, most of these steps above have to be performed manually, on individual Drawings, Part Studios, Assemblies (for the most part). I don't even want to get into the manual fixes on my new Revision Tables in all the new drawings!

Is there an Improvement Request here, something like: "Move to new Document, and make sure all references are to the new local copy" or simply "Let me update the Replace parts in Drawings!"

Anyone have any other ideas on how to do this? (I am sure that I'm missing many valid reasons that it has to be this way, but looking for some improvement in workflow nonetheless).

Oh - and we need better bulk tools for this task (like a Super Pack & Go) that allows us to Create a New Document, Update Part Numbers, and manage references all in one step / interface!