I use DBWorks today and make a new part based on an old one( where this is preferred) with the "save as" command. Unfortunately do I only get the part, it do not copy the linked drawing. So I have to make a new one.......
Is there a way to create a new part from an old part including the old drawing? (In a simple way...)
I'll be most thankful to any comments on this one :)
Regards Gunnar Storheim
Hi Gunnar
We use DBWorks and AFAIK there is no way to include the drawing when saving a part/assembly.
The workaround that we use is to save the part/assembly first to the new number (save as copy checked) then save the drawing to the new number.
Then in DBWorks highlight the drawing and you will see the original part/assembly referenced. RMB on this part/assembly and select "rename/replace>mark as document to be replaced."
Then select the new part/assembly which was created from the save as, and RMB and select "rename/replace>mark as replacing document."
You will then see a dialogue box showing where the part/assembly is used. You just select the new drawing that was created in the save as.
Hope this is clear enough and hope it helps.
FrankG
I don't know about DBWorks, but here is one way to create a part and drawing file at the same time.
Open the original drawing (original.slddrw), Save-As new drawing file name (new.slddrw), before you select OK, click on the Reference button, assign a new part file name (new.sldprt) i.e. New Path dialogue box, relocate the part file if necessary using Browse, click OK, can also relocate the drawing file if necessary using the Save in box, click OK
You now have a new drawing and part file
Kman
Hi Gunnar
I have the same problem with Smarteam. The work around I use and this should also be the same for DBworks as it is a Solidworks routine nothing to do with DBW or SMT. Open the origonal drawing that is to be copied and do File SaveAs (do not SaveAs copy) to your new number. The drawing on screen should now have your new number showing on the title bar. Right click on a drawing view and open the part or assembly (this will be the part or assembly associated with the origonal drawing). With the model active (do not close the new drawing) do a file SaveAs (do not SaveAs copy), ignore the replace warning prompts. Go back to your new drawing and it should be registering the new model number. No file hunting involved.
Regards
Brian
It's even easier. Open both the part and the drawing. Save the part with the new name/location. It will give you a warning. Now save the drawing with its new name/location.
Jerry Steiger Tripod Data Systems
Excellent! Kman
"Kman" skrev i melding news: snipped-for-privacy@corp.supernews.com...
But it don't work with DBWorks....... ;)
Gunnar Storheim Seaproof Solutions
Gunnar,
I suspect you have the dataentr.lst option set on DBWorks save/saveas option set. This command overwrites the SW save and saveas function. Turning this option off will allow SW to perform the required steps needed to link your drawing using the steps illustrated by other contributors. When complete - turn on the dataentr.lst option. I would consider this a batch process of legacy data.
Cheers,
Len K. Mar, PEng. President E-data Solutions
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.