Linking Drawing Views to new CATPart

[Lea75]

Hi guys, could someone tell me if it is possible to automate and how it would be the code for linking the views of a drawing to a new CATPart?

I have tried with this code but it does not work for me. I'm not sure if that property is read-only or I'm writing something wrong.

For j = 3 To odrawingviews.Count
Set odrawingviews.Item(j).GenerativeBehavior.Document.Parent.FullName = oPartDocument.FullName
Next j

Thank you in advance for any tip

 

[itsmyjob]

should look into DrawingView.DrawingViewGenerativeLinks.AddLink

you can find that in the object map from CAAV5Automation.chm file ... in your [catia]Code\Bin folder

Eric N.
indocti discant et ament meminisse periti ​

 

[tesak]

Hi,
it is also important to delete existing links, so your code should look like the one below:

Option Explicit

Sub LinksReplace()
    Dim myDrawing As DrawingDocument
    Set myDrawing = CATIA.Documents.Item(1)
    
    Dim mySheet As DrawingSheet
    Set mySheet = myDrawing.Sheets.Item(1)
    
    Dim myPart As Document
    Set myPart = CATIA.Documents.Item(2)
    
    Dim i As Integer
    Dim currView As DrawingView, viewLinks As DrawingViewGenerativeLinks
    For i = 3 To mySheet.Views.Count
        Set currView = mySheet.Views.Item(i)
        Set viewLinks = currView.GenerativeLinks
        
        viewLinks.RemoveAllLinks
        viewLinks.AddLink myPart.Product
    Next
End Sub

Replace Documents indexes [CATIA.Documents.Item(x)] as you need in regards to your open documents and it should work.



Tesak

http://scripts4all.eu/txtoncurve/

- Text along a curve for Catia V5

 

[Lea75]

Thank you both. It works fine, but I have a problem.
It also loose links to dimensions
I have a stardard drawing (with all dimensions) linked to a stardard Part (that can change its shape) and it can be saved in different folders, so I need to point the drawing to different paths, but I can't loose the dimensions.
Is there any way to avoid it?
Regards

 

[tesak]

I don't think so. If you replace one part by another, links to dimensions are lost as well. You can however reconnect them with Re-route Dimensions command.

Tesak

http://scripts4all.eu/txtoncurve/

- Text along a curve for Catia V5

 

[Lea75]

If I do it manually I don't loose the dimension links.
CATParts are copies from the same original CATPart. Just change some dimensions among them.

 

[Costin Ruja]

You might get this behaviour using part templates. In the menu defining the part template you can instantiate also other documents (drawings of the part). However, i think you need 2 separate licences, PKT an KT1 if I remember correctly.

Best regards,
Costin Ruja