Update all views in a sheet to turn on Associative check box

[GeorgK]

Hello together,

is there a solution to turn on associative check box in a drawing? How to get the ActiveDesignViewRepresentation name?

Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.ActiveDocument
Dim oSheet As Sheet
Dim oDrawView As DrawingView

For Each oSheet In oDrawDoc.Sheets
For Each oDrawView In oSheet.DrawingViews
Representation = oDrawView.ActiveDesignViewRepresentation
If Representation <> "" Then

'  How to get the name
'oDrawView.SetDesignViewRepresentation(Representation, True)
End If
Next
Next

 

 Thank you

Georg

[steveh3]

Both lines appear to be erroring... I attempted to delete both either/or...

[steveh3]

Now this...

[NachoShaw]

The nuances of VBA. you need to change the 'Set' to 'Call'. You're not setting anything, you're calling the function with parameters

Call oDrawView.SetDesignViewRepresentation("Default", True)

[NachoShaw]

your code should be

Dim app As Application: Set app = ThisApplication
Dim oDrawDoc As DrawingDocument: Set oDrawDoc = app.ActiveDocument
Dim oSheet As Sheet

For Each oSheet In oDrawDoc.Sheets
        Dim oDrawView As DrawingView
        For Each oDrawView In oSheet.DrawingViews
            If oDrawView.ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
                Call oDrawView.SetDesignViewRepresentation("Default", True)
            End If
        Next
Next

[steveh3]

Thanks.

I see what the this code is doing now.

Call oDrawView.SetDesignViewRepresentation("Default", True)

It's almost what we looking for. 

So, it does check the box for Associative, but I don't want it to change the View Rep.

Can it read the view rep and then toggle it?

[NachoShaw]

Ok. This will get the name of the current view rep in the view then set the association to true using the SetDesignViewRepresentation function

Dim app As Application: Set app = ThisApplication
Dim oDrawDoc As DrawingDocument: Set oDrawDoc = app.ActiveDocument
Dim oSheet As Sheet

For Each oSheet In oDrawDoc.Sheets
        Dim oDrawView As DrawingView
        For Each oDrawView In oSheet.DrawingViews
            If oDrawView.ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
                Dim name As String: name = oDrawView.DesignViewRepresentation
            
                Call oDrawView.SetDesignViewRepresentation(name, True)
            End If
        Next
Next

you could also add a condition to check the current viewrep and update it to what you need if it was incorrect

Dim app As Application: Set app = ThisApplication
Dim oDrawDoc As DrawingDocument: Set oDrawDoc = app.ActiveDocument
Dim oSheet As Sheet

For Each oSheet In oDrawDoc.Sheets
        Dim oDrawView As DrawingView
        For Each oDrawView In oSheet.DrawingViews
            If oDrawView.ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
                Dim name As String: name = oDrawView.DesignViewRepresentation
                
                If Not name = "Default" Then
                name = "Default"
                End If
            
                Call oDrawView.SetDesignViewRepresentation(name, True)
            End If
        Next
Next

[NachoShaw]

and finally, if you need to toggle the associative on / off (which is the definition of toggle), you can toggle it like this

Dim app As Application: Set app = ThisApplication
Dim oDrawDoc As DrawingDocument: Set oDrawDoc = app.ActiveDocument
Dim oSheet As Sheet

For Each oSheet In oDrawDoc.Sheets
        Dim oDrawView As DrawingView
        For Each oDrawView In oSheet.DrawingViews
            If oDrawView.ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
                Dim name As String: name = oDrawView.DesignViewRepresentation
                
                If Not name = "Default" Then
                name = "Default"
                End If
                
                Dim Assoc As Boolean: Assoc = oDrawView.DesignViewAssociative

                Call oDrawView.SetDesignViewRepresentation(name, Not Assoc)
            End If
        Next
Next

[steveh3]

That's it...seems to be working!!!

If we want to add in views that are .iams or .ipn's

possible to put an OR in the statement....

If oDrawView.ReferencedDocumentDescriptor.ReferencedDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then

If so...what's the syntax for .ipn's here?

DocumentTypeEnum.kAssemblyDocumentObject

[NachoShaw]

Hi

I would do a Select Case

Select Case oDrawView.ReferencedDocumentDescriptor.ReferencedDocumentType
   Case DocumentTypeEnum.kAssemblyDocumentObject
   'assembly code here

   Case DocumentTypeEnum.kPresentationDocumentObject
   'presentation code here

   Case DocumentTypeEnum.kPartDocumentObject
   'part code here

End Select

[steveh3]

Having problem with the Views that are referring to an .ipn.

Statement works fine as a "kAssemblyDocumentObject"

But, when I change it to a kPresentationDocumentObject

It bugs out...

Best,

[NachoShaw]

Hey

Good news & bad news...

Good News

you can change the associative type like this

oDrawView.PresentationViewAssociative = True

Bad News

Presentation views are different to part & assembly views as in, they dont directly show the view rep but instead, show the list of snapshot views in the presentation file. If you need to change the view rep, the underlying file would need to be opened and the view rep change at file level in the snapshop view.

Heres the bad news; there is a function in a DrawingView that is supposed to get the name of the current snapshot view in the drawingview which you would need to correct update the viedwrep of the snapshot in the presentation file however, its been flagged as bug and is currently not working. I found a thread from about 3 yrs ago explaining this so im assuming its yet another one of those things autodesk doesnt care about.

to get around it, you will need the name of the view so that you can -

open the underlying presentation file

1. edit the snapshot
2. change the viewrep
3. save and close it
4. update the drawing sheet
5. associate the view

thanks

[steveh3]

@NachoShaw 

Thanks for all the help!!!

Finally got it working.

It toggles on "Associative" for all views in an .idw's that refer to an .iam or .ipn

Ignores ipt views.

Combined it with an iLogic script that runs the VBA before it saves.

Best,

[NachoShaw]

great news.

why dont you combine all of the VBA witrh iLogic, seems pointless using both and iLogic supersedes VBA

[steveh3]

Just using the iLogic to trigger the VBA to run on only idw's.

Before a save, a trigger runs the iLogic which tells the VBA to run.

'This runs the VBA to check the Associative box on all Assembly views
	InventorVb.RunMacro("ApplicationProject", "Module3", "ViewAssoc3")

Possible to do this otherwise?