Copying Drawing From Similar Part, but Different File 3

[MattP]

I have an assembly that I completed the design on and do not anticipate making any changes to. I have another assy to design that is very similar with some dimensional changes. I decided not to make another assy configuration to avoid headaches. I decided to make all assy and part files read-only so that if a change was necessary, I would be forced to save it as another file. The parts that don't change would keep the same file name and the drawing would already be done.

NOW,its time to work up the drawings for the part/assy's that have changed. Is there a way to copy the original drawing format, views, dimensions, BOM, etc and change the reference model file?


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[ctopher]

Are you making new part numbers for the dwgs using the existing parts, or new p/n's all around?

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
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[MadMango]

We do this all the time. We save a copy of the standard part & drawing into a different folder using new file names (our file names are the same as our part numbers). Then we open the newly created drawing... since it's now lost it's reference, SW will flag us to find it. We then point to the new part and everything works perfectly, and the new drawing is associated to the new part.

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[MattP]

Interesting. If the drawing is able to lose the reference and have you point it in the right direction, is it possible to just change the reference from one model to another and have everything in the same folder?

ctopher: I am not sure if this answers your question or not, but for the parts that differ from the first assy to the next, I save as a new part number. The parts that stay the same, keep the old part number and are shared between the two assemblies.


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[CorBlimeyLimey]

If you have SW Explorer, it is also very easy to do. If you open the Top Level Assy drawing & do a copy, you can save whatever parts you need to a new folder and all references to the TL drawing are maintained. Once saved the new parts can be renamed, also using SW Explorer, so that new references are created.
Any part drawings can be simply copied into the new folder (using Windows) and as MadMango explained, the refs can be relinked upon opening them.


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[mncad]

You can also bring up the Open screen in SW, browse to your existing drawing, highlight the name and right click, now you can copy the file, browse to your new location and paste the file. Rename the file as needed then hightlight the file name and click the reference box in the Open screen. In the reference box that comes up double click the file name and browse to your new assembly. Close that screen and then open the file. The drawing should update completely to the new assembly. This is all done inside of the open screen in SW.

mncad


mncad

 

[MattP]

Brilliant! Thanks for the replys. All were helpful. mncad, what you described is exactly what I was looking for and it works like a charm.

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[ctopher]

Sorry for the delay, I leave at 3:45 PT.
I use SW Explorer for this, same as CBL.

Chris
Sr. Mechanical Designer, CAD
SolidWorks 05 SP3.1 / PDMWorks 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716