Component Occurrence Visibility in Drawing View

[tdant]

Hello All,

I'm trying to turn off visibility for all part occurrences named "break representation" in a drawing document. Here's what I've come up with so far:

Sub HideBreakRepresentationsInDrawing()
    
    Dim Counter As Integer
    Counter = 0
    
    If ThisApplication.Documents.Count <> 0 Then
        Dim Doc As DrawingDocument
        Set Doc = ThisApplication.ActiveDocument
    Else
        Call MsgBox("No open documents")
        Exit Sub
    End If
    
    Dim Sheets As Sheets
    Set Sheets = Doc.Sheets
    
    'recurse all sheets in drawing document
    Dim Sheet As Sheet
    For Each Sheet In Sheets
        Dim Views As DrawingViews
        Set Views = Sheet.DrawingViews 'recurse views here
        
        'recurse all drawing views in sheet
        Dim View As DrawingView
        For Each View In Views
            'assumes the drawing view references an assembly
            If View.ReferencedDocumentDescriptor.ReferencedDocumentType = kAssemblyDocumentObject Then
                Dim RefDoc As AssemblyDocument
                Set RefDoc = View.ReferencedDocumentDescriptor.ReferencedDocument
            
                'recurse all components in assembly referenced by view
                Call recurseOccurrences(RefDoc.ComponentDefinition.Occurrences, Counter)
            End If
        Next
    Next
    
    Call MsgBox(Counter)
End Sub

Function recurseOccurrences(Occurrences As ComponentOccurrences, Counter As Integer)
    Dim Occurrence As ComponentOccurrence
    For Each Occurrence In Occurrences
        If Occurrence.DefinitionDocumentType = kAssemblyDocumentObject Then
            'found assembly, find subparts
            Call recurseOccurrences(Occurrence.SubOccurrences, Counter)
        ElseIf Occurrence.DefinitionDocumentType = kPartDocumentObject And InStr(LCase(Occurrence.Name), "break representation") Then
            'do something to a part
            Occurrence.Visible = False
            Counter = Counter + 1
        End If
    Next
End Function

My counter returns 34, so I know the script is finding what I want it to find, but none of the part occurrences are affected. Does ComponentOccurrence.Visible = False not work in the drawing environment or something?

[MechMachineMan]

Somewhat correct.

The call you are making is changing the ASSEMBLY DOCUMENT, not the Drawing Document.

I think to make that work there are 2 steps you can take:

1. Use a Design View in your drawing views that is neither Master, nor Locked.

2. Ensure the Views are set to be Assosciative to Design view (the chain link in the edit view window).

There is not really a ton of support for changing visibility of specific occurrences in drawings through api otherwise.

[tdant]

I need to avoid changing the assembly document if at all possible. So basically, there's no way to control drawing document occurrence visibility from the API? That seems weird.

[MechMachineMan · Accepted solution]

No.

It seems Autodesk's supported workflow is to use Design View Reps from the assembly to control occurrence visibility in ALL cases.

Being able to change it in a drawing is a simple override to allow users to still get the job done if they don't understand the preferred workflow. If they were to add-in API control to all of the overrides that would just allow improper workflow to proliferate.

[Anonymous]

Hi together,

also this is an old thread i would answer for others who read this in future.

It is possible to change the visibility of occurences in drawing views.

Just use the

DrawingView.SetVisibility(Occurence, True/False)

switch

It has to be done for each drawing view on the sheet(s)

This method was introduced in Inventor 11

Greetz