replace model in drawings? 4

[Brad82]

Is there a way to replace the model in a drawing? I had to make a new variation of an old design and hoped that I could save a copy of the original drawing under a new name and then replace the model. I have done this in Pro/E but cannot find out how to do this in Solidworks.

 

[PDMAdmin]

Do the "source" and "destination" models have the same filename? If they do, simply copy the "destination" model into your working directory (overwriting the "source" model) and load the drawing. If they don't, you need to do the following:

1) Move the "destination" model into a different directory.

2) With the drawing open in SolidWorks, expand one of the drawing views until you see the "source" model. RMB on it and select "Open part."

3) With the part open, select "File / Save As" and enter the filename of the "destination" model. Make sure the option "Save as Copy" is not checkmarked.

4) Close the part. Save the drawing and close it. Copy the "destination" model from the other directory in step 1 into your working directory.

5) Open the drawing back up. You should be looking at the same drawing with the "destination" model in it.

 

[Brad82]

I believe that I follow you, but let me give some more info. I want to keep the original model and the associated drawings because these are still going to be used. For my new variation, I created a new folder on my drive and saved the original part model and its drawing to this new folder under a new filename. When I saved them to the new folder, I did have the Save As Copy box checked. I have already revised the new part model. I now just want to be able to use my drawing layout with the new model. The drawing in my new folder is still referencing the original part model that resides in the original folder. Will this work:

-Move my revised part model to a third folder.
-Open the renamed drawing, then open the part from a drawing view as you described in Step2.
-follow your steps 3 through 5

If I do this, will my original drawing in the original folder remain unchanged as I want?

 

[TateJ]

When in the OPEN FILE dialog box... click REFERENCES & then browse to the file you want your new drawing to open. I do this all the time.

Windows 2000 Professional / Microsoft Intellimouse Explorer
SolidWorks 2006 SP02.0 / SpaceBall 4000 FLX
Diet Coke with Lime / Dark Chocolate
Lava Lamp
www.Tate3d.com​

 

[dgowans]

Brad82,

You want to change the references of the new (copied) drawing:

Close any open documents.
Get into the File, Open form and highlight your new drawing, and hit the References button.
In the referenced Documents form that opens, browse to and select your new, revised part. Hit OK on this form and open the drawing.

Voila!!!!

 

[Brad82]

The references button worked like a charm. Thanks.

 

[dogarila]

You should thank TateJ for his valuable post.

 

[EngJW]

Wow, I just tried it and it works- I could have saved a few hours a week ago. Add another star.

 

[beachcomber]

Aonother way is to use Solid Works Explorer.
Start SE Explorer and open your original drawing.
In the file list on the left you should see your original model referenced to it.
Now RMB on the drawing in the list and select Copy.
The system assigns a new name for the copy using the current filename with "Rev2" tagged on the end.
You can change the path, filename and suffix here if you wish.
I would make sure you already have your new directory created if you want to set a new path.
If you want to copy the models at the same time click the "Copy Children" option.
You can deselect any you don't want to copy - probably standard parts like screws etc.
When you hit Apply a new drawing will be created with the new filename and the new models already linked to it.
Go to Open and locate the new file to see it.

You will need to be careful if you are doing it with complex assembly structures, but for simple stuff it's really easy and well worth a look.

Pity it's not as powerfull as Solid Edge's Revision Manager.

bc.