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Duplicated Drawing Shares Revision History With Original Drawing

AaronGuoAaronGuo Member Posts: 1
Hello all,

I am working with the revision system in Onshape for my drawings, and I have a drawing that is on, say, revision B. If I try to duplicate this drawing for the purposes of creating a drawing for a different size of the same part (just changing configurations of the inserted parts), then the whole revision history is also copied over. When I try to release this drawing as a separate entity from the original, Onshape tries to release it under the same drawing ID name. I can change the part number, but when I try to set the revision letter to A to start fresh, I think this causes an error that doesn't allow me to release it.

At the same time, I can't refresh the revision table on the drawing, so I would have to continue off from C, which is not what I would like. Is there any way to duplicate a drawing without it copying the revision history as well (without having to copy each sheet's components to a fresh drawing)?

Thanks in advance.


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    eric_pestyeric_pesty Member Posts: 1,493 PRO
    I think if you give it a new part number after you duplicate, it should become "separate", although the rev table might still "look" wrong until you go through the release process (I think I ran into something similar recently).
    Make sure the parts/assemblies referenced by the drawing are also given new part numbers to avoid errors.

    It should work so if it doesn't I would submit a ticket to look at your specific case.
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    tim_hess427tim_hess427 Member Posts: 648 ✭✭✭✭
    I think you're on the right track. A couple things to keep in mind:
    1. Drawings, Parts, and Assemblies all their own revision history independent of one another. 
    2. Depending on how your organization is configured, drawings and parts/assemblies may be able to use the same part number. 
    3. You may be running into a situation where you've changed the drawing part number, but the part view is actually referencing (and linked to) a released part from the original document. 
    So, yes, you should be able to change part numbers and then release the new parts. If I were troubleshooting, it would look deeper to just make sure that both the parts and the drawings have new part numbers as appropriate and that all of the drawing views are referencing the correct part versions (or workspaces).
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    shawn_crockershawn_crocker Member, OS Professional Posts: 801 PRO
    I agree with everything said above.  From my experience, if you change the drawing part number from the release dialog, and then manually change the rev label to A, sometimes it helps the release reset itself by hitting apply.  Apply is different from refresh as you made reference to.  Apply actually forces new rows into all the items configured properties table or if not configured, into the items default properties.  You maybe experiencing issue because you have changed the part number but have not fully applied it before attempting release.  That said, I would still tread with caution after apply the changes.  I find quite often, after applying, the revision label will jump back to the way it was (c or whatever).  I then have to change it back to A and apply again.  I have never had it happen twice in a row.

    Another thing to consider is your part that the drawing is referencing.  If you had created a part number for the part before having enabled configurations, every time you change the reference config in the drawing and then attempt a release, onshape will try to use that original part number that you had assigned before enabling configs.  To stop this, I copy the properties table and paste it into a sheet temporarily.  I delete the part number column from the properties table.  look at the part properties and remove the default part number you will find there.  Then put the part number column back into the properties table and paste the part numbers back in from the temporary sheet you used to store the table.  From now on, new configs will populate a blank part number in the release dialog because you define blank as the default part number.
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