Reference file

[vidon]

Does anyone know if it is possible to change the reference file for a drawing? Last week I was doing two drawings at once so naturally I messed up - I finished one part, saved it, did a drawing, saved it, than I changed the part into a new part and saved it as a different file ( and yes, both files exist in the same directory ), finished the second drawing, and saved it. Then when I opened the first drawing it changed and it wont change back.Its a really complex part and I just dont have the time right now to do it all over again. I tried fiksing the problem myself but I just cant do it. Need your help. Thank you in advance.

Vid Golob
Research and developement
Iskra Tela
Slovenia

 

[ctopher]

FILE/OPEN, then select references within open window.

Chris
SolidWorks 07 4.0/PDMWorks 07
AutoCAD 06
ctopher's home (updated 04-21-07)

 

[CorBlimeyLimey]

See also;

http://www.solidprofessorstore.com/Samples/PackandGo.html

and for future reference;

http://www.solidprofessorstore.com/asksp_media/V13Q1.html

 

[SBaugh]

Working with 2 drawings that have different parts, but all you need to do is change the reference.

SW explorer works well and the file\Open works well... either one will do the trick.

I prefer the file\open because that away I know what I am pointing it to myself.

What I do is I open the drawing1 and do a file save as an change the name of the drawing1 to say for example drawing2. I close the file to be safe, and reopen Drawing2, but I just don't open it all the way. I File\Open - Highlight Drawing2 - click references - Change Part1 to Part2 and then I click open - I do a file find references to confirm I am using Part2 in Drawing 2. Then I save and work or Save and close (to be safe) and reopen Drawing2.

It quick its easy and its safe.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"
faq731-376

 

[CorBlimeyLimey]

From

http://www.solidworks.com/pages/services/FAQs/FAQ-DataManagement.html

ID : 72415

Question : How can I open a drawing and have it reference a different part than it was originally created with?

Answer : When opening the drawing, use the Open dialog. Click on the drawing name, and before you click Open, select the References button. Single click twice slowly on the part name under "New pathname" and type in the name of the replacement part. Click OK and then Open and the drawing will open and will now refer to the new part. If the part is not a modified version of the original part, it will warn that the internal IDs do not match. In such a case, the drawing might not open because the part is totally incompatible or dimensions/annotations may shift around or become dangling because the original entity references are not in the new file. If the drawing does open, you must save the drawing for this reference update to become permanent. (Please note that this procedure can also be used when opening other types of documents, such as assemblies.)

 

[vidon]

Thank you for your answers.

Vid