Confused about "Save As Copy" in parts and drawings

[Ralph2]

I am confused on the Save as Copy and hope someone can set me straight.

I have a part and make a drawing of it. The shop is happy but wants an additional version as well (add another hole..). So I open my part, Save As > Save as copy and open. All is well, my original stays and I make my changes in the new copy.
Now, how can I have my drawing also pick up this new version without having to start all over with a blank drawing?

I hope my explanation makes sense..
Thank you for your time.
Ralph
SW14 x64 on Windows7

 

[Updraft]

Ralph,

Save as Copy should be used for when you want two distinctly different parts, i.e., Part No. 1 and Part No. 2. It sounds like your shop is asking for a simple revision and maybe their reason is to add a tooling or fixture hole. If this hole is acceptable in the finished part then you would be best served by creating a revision to the original part and its drawing. If you need to keep this revision separate from the original then you should look into the use of Configurations. If you are unfamiliar with configs then read up on them in SWX Help and in the Tutorials under Basic Techniques -> Design Tables.

- - -Updraft

 

[ctopher]

I agree with Updraft.
Make a config.
Is the hole part of the part, or for mfg purposes? If for mfg, make a config.
If a change to the part, change the original part and roll the revision.

Chris, CSWA
SolidWorks 14
SolidWorks Legion

 

[Dievant]

Save both the part and drawing as a copy then close out of both files and go into Solidworks explorer. Find your newly copied drawing on the left panel and select it. A tab at the top of the main panel should open called references, select it. A file name should show up and should have the name of your original part. Right click on in and select replace. Another box should open up, browse to find your newly copied part, hit ok and everything should be good to go, open up your new drawing and add the dimensions to your new hole and you're ready to go.

 

[DiegoLGraves]

Ralph, an additional version of this part would indicate needing a different part number. For this using pack and go is your best bet.

If you are making a tabulated part such as xxx-xxxx-001, xxx-xxxx-002 part numbers, configurations in the part file could be your best approach, using the same drawing for both items.

This is my approach. Diego

 

[TWJR]

Basically, "save as" will change the name and/or folder of the file, and update references to any higher level assemblies or drawings. If this is your goal, make sure these higher level objects are in session so the references in these file(s) get updated.
"Save as copy" makes a copy with the new name and/or folder, which is independent of anything else.
"Save as copy and open" is same as above, but also opens the new part in your current Solidworks session.

 

[ctopher]

Yes, if drawings and assemblies are to update during "save as", the dwgs and assy's need to be open.
"Save as copy" will not update any referenced dwgs or assy's.
Too many users get this confused.

Chris, CSWA
SolidWorks 14
SolidWorks Legion

 

[CorBlimeyLimey]

If a distinct and separate part and drawing are required;
Open the original drawing
Do a Saves as copy & open to the new name
Close the original drawing
From within the new drawing, open the part
Do a Save as copy and open to the new name
Close the original part.

The new part and drawing are now ready to be edited to suit.

 

[Ralph2]

Wow.. Thanks to all those that replied. I now have a number of things to try and see what I can make work. My example of "adding a hole" was generic. What brought this to a problem was the shop makes a split collar, bolted together that aligns two shafts. The sizes of the shafts vary so I am constantly asked to make a new drawing.. but as the only thing that changes is the diameter there had to be a better way than starting from scratch each time with a new drawing..
With all your help I think I can simplify my work big time.
Thank you

 

[Jboggs]

Ralph2:
"how can I have my drawing also pick up this new version without having to start all over with a blank drawing?"
A coworker showed me this and it is SO EASY! Save a copy of your original drawing giving it the same name as the modified part. If you then open that newly saved drawing file normally it will still refer back to your original part. But instead after you click OPEN and select that new drawing file, but before you open it, click the REFERENCES button. You will see a dialog box that will allow you to "point" that drawing to your modified part. It will open up with all the views and dimensions from the original drawing intact but showing the modified part. Works really well.

 

[DiegoLGraves]

All good suggestions. I'd still recommend pack and go as the simplest and cleanest way within SW to create the new drawing and part. It's definitely worth learning to use whether it becomes your default method or not.

Diego