Linke refused................. 6

• Dec 11, 2013

• Thread starter
• #2

CAD2015

Computer

Jan 21, 2006

2,053

Sorry, I'd like to replace part2 with part1.
It is just an example, creted as simple as possible. I would like to know the steps that must be follow in order to change the linkage of the drawing.
Thanks!

MZ7DYJ

 

 http://files.engineering.com/getfile.aspx?folder=eb579945-64aa-4de3-9c6d-31c9b3ee6019&file=Part1.CATPart

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• Dec 11, 2013

1
• #3

adminhost

Computer

Jul 30, 2007

23

If the Part your replacing does not have the same UUID as the original Part in the link, it will be refused. In Drafting, go to Edit > Links. Thats where you can change links.

 

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• Dec 11, 2013

• Thread starter
• #4

CAD2015

Computer

Jan 21, 2006

2,053

I used In Drafting, Edit > Links, but it doesn;t work!
How could I change the UUID?
Thanks

MZ7DYJ

 

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• Dec 11, 2013

1
• #5

itsmyjob

Mechanical

Apr 11, 2002

2,375

you don't.

only way to change the link is with scripts but dimesions will lose links... search forums for more info

Eric N.
indocti discant et ament meminisse periti ​

 

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• Dec 13, 2013

• Thread starter
• #6

CAD2015

Computer

Jan 21, 2006

2,053

Thanks a lot!

MZ7DYJ

 

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• Dec 17, 2013

4
• #7

drewmumaw

Computer

May 20, 2013

288

@mz7dyj
You can't change the drawing view links manually via Edit > Links, but you can do it with a vba script as itsmyjob recommended. See code below and attached images.

Code:

Sub CATMain()

Dim drawingDocument1 As DrawingDocument
Set drawingDocument1 = CATIA.ActiveDocument

Dim drawingSheets1 As DrawingSheets
Set drawingSheets1 = drawingDocument1.Sheets

Dim drawingSheet1 As DrawingSheet
Set drawingSheet1 = drawingSheets1.ActiveSheet

Dim drawingViews1 As DrawingViews
Set drawingViews1 = drawingSheet1.Views

Dim drawingView1 As DrawingView
Set drawingView1 = drawingViews1.ActiveView

Dim viewLinks1 As DrawingViewGenerativeLinks
Set viewLinks1 = drawingView1.GenerativeLinks
viewLinks1.RemoveAllLinks

Dim partDocument1 As Document
Set partDocument1 = CATIA.Documents.Item("square.CATPart")

Dim viewBehavior As DrawingViewGenerativeBehavior
Set viewBehavior = drawingView1.GenerativeBehavior
viewBehavior.Document = partDocument1
viewBehavior.Update

End Sub

Regards,
Drew Mumaw

http://www.drewmumaw.com/

http://www.textsketcher.com/

 

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• Dec 18, 2013

• Thread starter
• #8

CAD2015

Computer

Jan 21, 2006

2,053

Thanks!

MZ7DYJ

 

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• Dec 19, 2013

• #9

KevinDeSmet

Computer

Apr 29, 2008

302

It's pretty sad, yeah. I know one company who wants every .CATPart stored underneath a .CATProduct, and then the drawings get made with links to the .CATProduct. This way the system does not complain about "refusing the document" with the same UUID .CATProduct being re-used and the .CATParts get unique UUID assignments.

It's an awful workaround, and I wouldn't recommend it.

Does that macro work as well as it sounds?

 

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• Dec 19, 2013

• #10

itsmyjob

Mechanical

Apr 11, 2002

2,375

relinking with macro does not relink annotations or dimensions... all links between drawing element and projected 3D will be lost (according to my testing way back then)

Eric N.
indocti discant et ament meminisse periti ​

 

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• Dec 21, 2013

• #11

hims1980

Aerospace

Jul 9, 2012

54

Thanks, itsmyjob & drewmumaw, was really searching for this type of solution to edit the link of a cat drawing.

Till now i was also getting the message of link refused, but now it is solved.

Just one more question ,will it work for complicated & bulky cat products & cat parts ?


Regards,

Himanshu

 

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• Dec 21, 2013

• #12

drewmumaw

Computer

May 20, 2013

288

@hims1980
I don't know. You'll have to test it. To be honest, I don't use it too much. If CATIA doesn't allow you to relink drawing views manually because of the "Link refused" error message then it makes me apprehensive to do it programmatically. I only use it out of necessity. It might retain ghost links, cause other problems behind the scenes, etc. I would use KevinDeSmet's suggestion of nesting components inside a shell CATProduct so that the drawing is always linked to that CATProduct. Then your subparts and subproducts can be swapped without encountering the "Link refused" error message. My two cents...

Regards,
Drew Mumaw

http://www.drewmumaw.com/

http://www.textsketcher.com/

 

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• Dec 21, 2013

• #13

ferdo

Mechanical

Jul 4, 2002

2,856

Hi,

A batch bulk solution it will be much more complicated but it can be done, you need to know what to relink exactly.

I know also a company using the solution with catproducts but only because of the pdm system, no connection with uuid.

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

https://picasaweb.google.com/103462806772634246699/

 

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• Dec 22, 2013

• #14

hims1980

Aerospace

Jul 9, 2012

54

@KevinDeSmet, but how could one store all the cat parts underneath a catproduct, because when you will check the links of a cat drawing having assembly views taken from a cat product, then in the "EDIT-LINKS" CATIA shows all the linked catp products as well as cat parts.

And how about the cat drawing to be created from a cat part & not from cat product ?

Please correct me if i have misunderstood.


Regards,

Himanshu

 

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• Dec 23, 2013

• #15

KevinDeSmet

Computer

Apr 29, 2008

302

Yeah you're right. As I said I only read that workflow, ain't never done it myself! I guess then they were unique .CATProduct files but they each had the same UUID which allowed the links to be re-linked. I guess?

 

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• Dec 23, 2013

• #16

KevinDeSmet

Computer

Apr 29, 2008

302

Ultimately, this must be some kind of brainfreeze in CATIA because I don't think very many other MCAD systems have this problem...

 

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