Question

Changing the Model to Which a Drawing is Referenced

Asked by: kgerb

Hello All,
I run into this problem quite often in Solidworks and have not been able to come up with a good solution.  I work in a production environment and am frequently required to make changes to current products.  For example, plate A is currently 8" long and it needs to be 10" long.  No problem, take out a new part number, save the model as a different name (the new part number), change the dimension, COMPLETELY recreate the 2D drawing, and I'm done.  You probably noticed the last step is where I have issues.  Every time I save a part as a new name and make a minor change I have to completely re-do (from scratch) the drawing.  It would be SOOO nice if I could just open the old drawing, save it with a new name, and then change the model to which the drawing is referenced to the new model.  However, it doesn't appear that this can be done.  Any advice would be much appreciated.

Kyle

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Asked On
2007-09-13 at 07:20:58ID22826223
Tags

solidworks

,

drawing

,

model

,

change

Topics

SolidWorks CAD Software

,

CAD & Architecture Software

Participating Experts
4
Points
500
Comments
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Answers

 

by: dhsindyPosted on 2007-09-13 at 07:55:10ID: 19884195

Do you have admin previleges on your system?  It sounds like to me your source files are protected at the folder level.  Try saving the file in a different folder where you know you have access.

Don't you get some kind of an error message.

 

by: kgerbPosted on 2007-09-13 at 10:59:18ID: 19885747

dhsindy,
Thanks for your response.  I don't think it's a permissions issue.  I have administrative privileges to this machine so I shouldn't be restricted.  I just don't know the procedure on how to do it.  Do you know how to change the model that a drawing references?  For example if you have two almost identical models (A and B) and you have a drawing of model A.  Do you know how to get the drawing to reference or "link" to model B instead of model A?  I realize that model B essentially has to be created from model A in order for the dimensions to recognize what edges to attach to and everything.  Am I being clear or just confusing things further?  It's essentially like doing a 'Replace Components' w/in an assembly, except in a drawing.

Kyle

 

by: meintsiPosted on 2007-10-02 at 12:41:57ID: 20001427

You have 2 methods at your disposal .......

Method 1:
1. Open both the original part and its drawing in SolidWorks.
 2. Do a save-as on the part file and SolidWorks will prompt you that the drawing will now reference the new part file.
3. Click yes to accept this change.
4. Now immediatly swith the the drawing and do as "save as' there.

Two different part files, each with its own drawing.

Method 2:

1. Within the FILE - OPEN dialog box .
2. Browse to the drawing you want to copy and highlight it it so that it previews on the right.
3. Click references.
4. Double-click the left-sie file string under "New Pathname" and browse to the new part file and either double-click the new part file or highlight it and select open
5. Select OK.
6. Select OPEN.
7. Immediatlely do a "save-as' on the now open drawing under the new file name.

 

by: meintsiPosted on 2007-10-02 at 12:46:30ID: 20001455

Poor typing.
4. Now immediatly swith the the drawing and do as "save as' there.  should be
       4. Now immediatly switch to the drawing and do as "save as' there.
and
4. Double-click the left-sie file string under "New Pathname" and browse   should be
       4. Double-click the left-side file string under "New Pathname" and browse .....

In both methods above, the originals will not be changed unless you hit SAVE instead of "SAVE AS".

 

by: meintsiPosted on 2007-10-02 at 12:49:22ID: 20001478

A small mistake in the second method.

THis is for after you copy the drawing file.
FILE - OPEN - to the copied drawing which when highlighted will appear in the preview pane and then hit REFERENCES and follow above.

 

by: tool_manPosted on 2007-10-15 at 11:20:46ID: 20080239

In SW2007 I think you may be able to do what you want with Pack-and-Go. In SW2006, SolidWorks Explorer may have the ability to do what you want. It did in some previous versions. If not SW2006, close your files and copy them to another directory but before you open the new copies, temporarily rename the original directory. Once you've renamed the original directory, open the drawing-copy and save it. Now you can put the original directory back to its original name.

At this point you'll rename your new copies. Open the renamed-drawing. When you do it'll ask you if you want to find the lost model. Choose "yes". Click on the correct model.

You can check "references" under File to see if the associations are correct.

 

by: kgerbPosted on 2007-10-15 at 12:09:41ID: 20080676

meintsi,
Thank you.  I tried a variant of your suggestions and it worked.  Through windows explorer I made copies of the drawings in which I wanted to change the references.  Then, using the File-open dialogue in Solidworks, I changed the pathname to the new model.  When I opened the drawing, the new geometry was displayed.  Thanks for help!

Kyle

 

by: alexsmith2kPosted on 2008-12-01 at 10:04:13ID: 23070798

meintsi:
Both solutions work perfect...absolutely fantastic - this has been bugging me for years! Thanks very much, Alex

20120131-EE-VQP-002

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