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when save a part as a new name, how to make drawing link to new part ?

Question asked by Zhao Hong Qiang on Sep 19, 2012
Latest reply on Sep 20, 2012 by Zhao Hong Qiang

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Hi All,
when I save a part as new name, and make some changes, I don't want to make new drawing , is there any way to save previous drawing to new drawing which link to new part ?

We have a lot of this kind of parts, customer has different module of machine, and they just make some changes and send to us. we have spent a lot of time on the drawing. if we can save part to new name and make changes, the drawing can be saved and link to new part, we can save a lot of time.

We have used other 3d software, when we save the part to antoher name, the 2d drawing will be saved as new name automatically and still remain the link. is it possible for wolidworks to do same way ?

Glenn Schroeder Sep 19, 2012 10:07 PM

Correct Answer

Hello,

There are two ways to do it that I know of; they should both come up if you do a search here for "change drawing reference". The one that I prefer is to go into SolidWorks Explorer, select the drawing, choose the References tab, then RMB on the part from the list and choose Change. I think that terminology is right, I'm at home now and don't have SolidWorks here to check.

Good luck,

Glenn

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Glenn Schroeder Sep 19, 2012 10:07 PM

Hello,

Good luck,

Glenn

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Zhao Hong Qiang @ Glenn Schroeder on Sep 19, 2012 10:55 PM

Hi Glenn, thank you very much. you are correct , I checked and it's workable. cheers !

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Mark Greenwell @ Zhao Hong Qiang on Sep 20, 2012 4:26 AM

Hi Zhao,

Another way is to open the drawing in SolidWorks then go:-

Save As -- click Reference tab at bottom -- Change the drawing and part name in the field box to the new name -- save to file location.

If you want to see a video of this let me know.

There must be something wrong with the site as it wont let me attach file to a reply, but will let me if I start a new post.

Thanks

Mark

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Jerry Steiger @ Mark Greenwell on Sep 20, 2012 12:38 PM

Mark,

Does it not let you attach a file after you select "Use advanced editor" in the upper right corner of the reply window?

Jerry Steiger

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Mark Greenwell @ Jerry Steiger on Sep 20, 2012 1:50 PM

Hi Jerry,

No tried about 3 or 4 times it looks like it starts to download then just freezes so i have to escape.

This was using the advanced editor only started to happen in last few days.

Funny that i can add a file if i start a post but not when replying to one,

Regards

Mark

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Seth Renigar @ Mark Greenwell on Sep 20, 2012 1:49 PM

Even another method (which I prefer) is to re-reference while opening the drawing. Click open. Highlight (single click) the drawing file. At the bottom of the open dialog, click references. A window pops up showing the current referenced parts (or assemblies). Double click the part (or assembly) that you want to re-reference, and simply browse to the new one you want to replace it with.

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Jeremiah Feist Sep 20, 2012 1:08 PM

my prefered method is to have the drawing and part open before you make the edits. save as the part, then save as the drawing. you now have a new drawing + part set that are linked and you can commence with the edits.

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Zhao Hong Qiang @ Jeremiah Feist on Sep 20, 2012 8:37 PM

Hi All friends, thanks for your great help .

I have tried a lot of times , and found there are several way to do this:

1. Keep part and drawing open and save them as same anohter name, the new part and drawing is linked together.

2. Just open the drawing only and save as new name, then open part and save as same name, the new part and drawing is still linked;

3. If open part only and save as new name, then open drawing and save as same name, the new drawing is linked with old part. so it need to change drawing reference in this way: open --->reference--->Ctrl + Double Click file ---> select file to be referenced --->open , then check the file reference, the new drawing is linked with new part.

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8 Replies

Glenn Schroeder Sep 19, 2012 10:07 PM
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Correct Answer
Hello,

There are two ways to do it that I know of; they should both come up if you do a search here for "change drawing reference". The one that I prefer is to go into SolidWorks Explorer, select the drawing, choose the References tab, then RMB on the part from the list and choose Change. I think that terminology is right, I'm at home now and don't have SolidWorks here to check.

Good luck,
Glenn
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- Zhao Hong Qiang @ Glenn Schroeder on Sep 19, 2012 10:55 PM
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  Hi Glenn, thank you very much. you are correct , I checked and it's workable. cheers !
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  - Mark Greenwell @ Zhao Hong Qiang on Sep 20, 2012 4:26 AM
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    Hi Zhao,
    
    Another way is to open the drawing in SolidWorks then go:-
    
    Save As -- click Reference tab at bottom -- Change the drawing and part name in the field box to the new name -- save to file location.
    
    If you want to see a video of this let me know.
    
    There must be something wrong with the site as it wont let me attach file to a reply, but will let me if I start a new post.
    
    Thanks
    
    Mark
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    - Jerry Steiger @ Mark Greenwell on Sep 20, 2012 12:38 PM
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      Correct Answer
      Mark,
      
      Does it not let you attach a file after you select "Use advanced editor" in the upper right corner of the reply window?
      
      Jerry Steiger
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      - Mark Greenwell @ Jerry Steiger on Sep 20, 2012 1:50 PM
        Mark Correct
        Correct Answer
        Hi Jerry,
        
        No tried about 3 or 4 times it looks like it starts to download then just freezes so i have to escape.
        
        This was using the advanced editor only started to happen in last few days.
        
        Funny that i can add a file if i start a post but not when replying to one,
        
        Regards
        
        Mark
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    - Seth Renigar @ Mark Greenwell on Sep 20, 2012 1:49 PM
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      Correct Answer
      Even another method (which I prefer) is to re-reference while opening the drawing. Click open. Highlight (single click) the drawing file. At the bottom of the open dialog, click references. A window pops up showing the current referenced parts (or assemblies). Double click the part (or assembly) that you want to re-reference, and simply browse to the new one you want to replace it with.
      Like • Show 0 Likes0
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Jeremiah Feist Sep 20, 2012 1:08 PM
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Correct Answer
my prefered method is to have the drawing and part open before you make the edits. save as the part, then save as the drawing. you now have a new drawing + part set that are linked and you can commence with the edits.
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- Zhao Hong Qiang @ Jeremiah Feist on Sep 20, 2012 8:37 PM
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  Correct Answer
  Hi All friends, thanks for your great help .
  
       I have tried a lot of times , and found there are several way to do this:
       1. Keep part and drawing open and save them as same anohter name, the new part and drawing is linked together.
       2. Just open the drawing only and save as new name, then open part and save as same name, the new part and drawing is still linked;
       3. If open part only and save as new name, then open drawing and save as same name, the new drawing is linked with old part. so it need to change drawing reference in this way: open --->reference--->Ctrl + Double Click file ---> select file to be referenced --->open , then check the file reference, the new drawing is linked with new part.
  Like • Show 1 Like1
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when save a part as a new name, how to make drawing link to new part ?

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