Model to Drawing Association

[dlarz]

Is there a way to change model association in a drawing feature tree (SolidWorks 2004)? The new company that I'm working for likes to change file names for existing models that are revised. I've saved both model and drawing under the revised filename but can't seem to figure out how to get the drawing feature tree association to update. Any help???

Thanks - Dave.

 

[Bgoldstein]

Not that I agree with changing filenames with revisions (we use PDM here), but you can use SolidWorks Explorer (located in the tools menu) to rename files. SW explorer will make sure that all assemblies (only in that directory or its subdirectories, I think!) that refer to the renamed part have their references updated.

 

[MElam]

From your message it sounds like the files have already been renamed in Windows explorer, and the new drawing is looking at the old part.

If that is correct, try this:
1. In the Open dialog box, select the new drawing.
2. BEFORE HITTING THE OPEN BUTTON, select the button that says "References..."
3. You will get a dialog box listing the files the drawing is referencing. Double-click on the old model, browse to the new model, and select Open.
4. Select OK in the References dialog.
5. Now select the Open button.
The drawing should open and update to see the new model.

For future renaming, use SWx Explorer.

 

[Mandrake22]

Another way is to "save as" the original drawing and click the references button. Change the appropriate file names as MElam says, then change the drawing name to the new one. At this point, you will have a new duplicate of the original model and drawing. Edit the newly named model to suit and your new drawing for it will also change. The amount of drawing "tweaking" will range from none to fairly extensive depending on how much you change the part.
A word to the wise is to make sure you are editing the newly named model and not the original version. Don't even ask me how I know!

 

[dlarz]

Thanks to all - it seems all answers are directed to SW Explorer. I'll keep that in mind although I accidentally found another method that seems to work.

Originally I opened the model and immediately did a "save as" and checked the "copy" box with the new revision extension. I accidentally saved one of the models, which incidentally had the drawing opened, without checking the "copy" box. All references in the drawing updated to the newly named model. I simply then saved the drawing as a copy with the rev extension updated and all appears to have associated correctly. Funny how things work out sometimes!

So... here's the algorithm that I found works best for me:

1 Open the Drawing.
2 Open the Model.
3 "Save as" the Model (without checking the "copy" box).
4 Switch to the Drawing and "save as" and "copy" to the same filename given to the model.

Any comments???

Dave

 

[Mandrake22]

You are doing one extra step compared to my example. If you "save as" from the drawing, you are creating both a new drawing and model in one step.

 

[TheTick]

Just a comment, not a criticism:

If you use SW Explorer to rename files, you don't duplicate any files. Also, SW Explorer can look for links you might miss, like in-context references.