I would strongly recommend the Pack and Go operation (with the drawing or assembly open, File > Pack and Go). That allows you to copy the assembly or drawing to a new folder, along with all the files that are referenced by it, and you can re-name files as part of the process. In addition to drawings, you might find that it works better than your current workflow for assemblies.
Just make sure that after the Pack and Go you close the original file and then open the new one to make changes. It's a common mistake (or at least it was for me starting out) to forget that and make un-intended changes to the original.
I tried this and it does not seem to work for the way I am trying to accomplish this. I simply get "copies" of the views of the drawing that I used the pack and go feature but they do not include the one or two updated parts for the new part number. As far as using this feature for assemblies I found it to be a little more time consuming. I may not have explained the process I am currently using very well.
At the risk of getting off on a tangent...
What I will do is open an assembly (one that is a similar version of the one I am trying to create) and for any component that I want to change out I right click on it, select "replace components". SW will then replace the component with all the mates still in tact. Then I will choose Smart Team>Save As...and the rest of the process of saving is just like normal. At a speed of less than 10 seconds per replaced part I can recreate entire assemblies and assign them new assembly numbers.
I am wondering if there is simply no way to accomplish this with a drawing since the views on them are simply reflections of a part or assembly. It seems as if there would have to be a way to drop the views onto the drawing and then find a way behind the scenes to change what assembly number they are linked to (thus allowing the parts I've replaced to be updated on the drawing).
You can change which model a drawing is referencing. Close the drawing, go to File > Open, and browse to the drawing. Highlight it (single click or hover, depending on your folder options settings), but don't open it. Click on the References button near the bottom right. That will take you to a dialog box where you can change the referenced assembly.
Or, using SolidWorks Explorer, browse to the drawing, click on it to highlight it, choose the References tab, and RMB on the file you want to change.
I am not familiar with smart team, but with just SW, I would open both the assembly and the drawing, then save-as the assmebly (save as copy UNCHECKED), then save-as the drawing (save as copy UNCHECKED). then you can make changes to both without affecting the originals, and they would be associated.
we use this workflow with EPDM extensively.
If you are manually adding stuff to your drawings, what about adding that stuff to the drawing sheet template?
It's an interesting thought but unfortunately will not help me. I need the drawings and item numbers in the annotations to be linked to specific part numbers. Generic information is minimal on the prints, a single note. Otherwise everything else is a view of a specific part number and therefore needs to be linked back to an original model.
What you want will work exactly the way you describe it.
Check out the old drawing.
Save the drawing as
Save the assembly as
Make your changes.
When you do the save-as on the assembly, any open files that reference it will point to the new file name. As long as you have the drawing open, it will work just the way you want.
John, I'm surprised SmarTeam doesn't handle cloning the drawing at the same time that you create the new assembly.
However, this is easy to address.
What you're going to do is make a copy of the drawing that already exists for the assembly you copied and rename it. Then, go into SolidWorks, go to the open dialog box and browse to the drawing and click on it (don't open it).
In the open dialog box at the bottom right, there's a button that says 'references.' Click that and a dialog box will appear displaying a list of models used in the drawing. Presumably, one of them is the assembly you copied from. Double-click on the path to that and browse for a replacement assembly. Select your newly created assembly and you'll be returned to the references dialog which will show an updated path for the assembly component. Click OK to close the references dialog box.
You'll still be in the file open dialog box and the new drawing will still be selected. At this point, click the 'Open' button. Don't browse, click on another part. Changing the references this way only works if you immediately open the file you modified.
If you do that, the drawing will load referencing the new assembly.
As far as SolidWorks is concerned, drawings are at the end of the referetial chain-that is, you can't reference a SolidWorks drawing in another SolidWorks document, so therefore you don't have to jump through the same hoops when renaming SLDDRW files that you do with models. I don't know if this is the case in SmarTeam.
But that should give you something to try.
That was definitely what I was looking for. I was able to do this and it worked great. I only had to change the balloons on the two parts I was changing out but otherwise all of the anootations and their links stayed in tact. Thanks for the help!