Link to drawing file / part file

3D Design Volume Model
1

I would like to change the name of a part file, the problem is that when I open the drawing file, the part disappears and I can't recreate the link with the new part file name (under SW2012). On older versions, SW offered me to tell him the new file name, but not anymore. How can I do this? Thank you

2

Hi@phil.bea

Have you updated your parts files?

See this link Everything is said

http://www.forum-cao-3d.fr/solidworks-mise-en-plan/vues-non-visible-apres-changement-nom-de-plan-t11614.html

@+ ;-)

3

If it does not ask you to search for the part, the message has been ignored.

To put the message back go to Tools, Option, Messages/Errors/Warning and check the message that starts with "Could not find the file ... "

You can also give back the reference without forcing SolidWorks to display this message by doing file, open, select the drawing, click on the reference button and double click on the link to the part then point to the renamed or moved part.

9 Likes
4

Hello

There has already been a question dealing with this topic.

http://www.lynkoa.com/forum/3d/changer-les-references-d-une-mise-en-plan

You will find all the additional answers to your problem.

But fthomas has given you the essentials.

 

Kind regards

1 Like
5

You can also use solidworks to "reknit" broken links.

1 Like
6

You can also use solidworks to "reknit" broken links.

1 Like
7

 


This is a fairly classic mistake.
You have renamed your room from windows explorer, big mistake!, if I may say so.

So your drawing, which used to point to your room named "x", still points to "x", except that "x" no longer exists because your room is now called "y".

I hope you follow me. 

Several solutions are available to you:

First, when you open your drawing, you should get a message like: Unable to find the C:\ users\...\name file of your old parts. 
-Do you want to look for it yourself or 
- Delete the component
You can then search for it manually

If you don't see an error message, you can do the following: 
From Solidworks File > Open > point to your > drawing and click the "Reference" button> you can then double-click on the name of your old part and hover over the new name.

Other methods, from your "empty" drawing: File> Look for the references > and double-click again on the name of your old part, to point to the name of the new one. 

Basically, renaming parts or drawings or assemblies for that matter, is the same thing as moving these elements in windows, the result is that Solidworks is lost, and it no longer knows how to find the elements.

THE SOLUTION :arrow: IS SOLIDWORKS EXPLORER

To rename or move, or repoint the right references, the solution is to do it via Solidworks Explorer, which will "keep all the references" automatically, whatever the manipulations. :mrgreen: 


You'll find out for next time!
 
8

And if you tried, to do file/open/ click on your drawing, and click on references which is next to open.

 

And from there you select the part in question.

 

 

 

9

Hello 

 

I'm coming back to this subject because I have a reference problem

But for me it is the other way around.

When I open the drawing, I can from there open up the part that's in the drawing.

But when I open the room, there are no links to the drawing...

Do you know what to do?

The drawing is in the same folder as the part

I use EPDM but updating the references doesn't change anything...

thank you in advance

2 Likes
10

Hello @bricesk_2

When we are in a drawing, and we open the model of a view, SW will look for the 3D model in relation to its "Reference" (a complete path). It can therefore look in a completely different folder than the folder where the drawing is stored.

On the other hand, when you are on a 3D, foo.sldprt or foo.sldprt, and you ask to open the drawing, SW opens the file foo.slddrw which is in the folder where the 3D is saved.

So if your 3D and 2D don't have exactly the same name (except for the extension), SW won't open the drawing. The same applies if the drawing is not in the same folder.

In other words, the reference exists from 2D to 3D, but not from 3D to 2D.

11

Thank you very much

 

I had put spaces in the MEP

Now it works 

 

Thank you

 

12

 bricesk_2: 

"Hello, I'm coming back to this subject because I have a reference problem

But for me it is the other way around.

When I open the drawing, I can from there open up the part that's in the drawing.

But when I open the room, there are no links to the drawing...

Do you know what to do?

The drawing is in the same folder as the part

I use EPDM but updating the references doesn't change anything...

thank you in advance"

 

Hello, I'm reviving the subject

We have the same problem. When you open a 3D (with EPDM) under solid and you want to access the drawing quickly (Right click: open the drawing), it does not find the drawing.

And yet:

- The 3D and the plan have the same name

- They are in the same EPDM folder

- It worked previously

It doesn't happen all the time but it's still common here.

Is it coming from the files not rebuilt? Changes of state? 

Do you have an idea? 

 

 

 

13

Hello

I'm reviving the subject a bit.

I've renamed different parts of an assembly (using solidworks->rename), but I'm still losing sight in the drawing.

I tried to get "search for references" but I can't change the link by double clicking...

A solution? Is it due to the 2020 SP1.0 version?

Thank you for your answers.

14

It makes do file/open/choose the drw file/"reference" button/double click on the name of the file to be searched/choose the new file

1 Like