Change BOM structure of all assy children to Phantom

[brendan.henderson]

Hi all.

I am aware of iLogic but do not have the time to learn it (and am to old to remeber it anyway). Hoping someone can help me with what I think should be easy to code.

I have been supplied a STEP file that when imported into Inventor creates many sub-assy's and parts. All good as I need to delete some. What I need to acheive is to change the BOM structure of all sub-assy's and all their parts to Phantom. I can easily change the top level assy to Phantom.

Making the top level assy Reference is not an option because this does strange stuff in IDW's. If all files become Phantom they are excluded from a drawing Parts List nd they display just fine in the IDW.

Any takers?

[MechMachineMan · Accepted solution]

This should accomplish what you asked for. It will even make library/cc parts phantom too, so be warned.

SyntaxEditor Code Snippet

Public Sub Main()

    ' Get the active assembly. 
    Dim oAsmDoc As AssemblyDocument 
    oAsmDoc = ThisApplication.ActiveDocument 
    
    
    Call TraverseAssembly(oAsmDoc.ComponentDefinition.Occurrences, 1)

End Sub 

Private Sub TraverseAssembly(Occurrences As ComponentOccurrences, _ 
                             Level As Integer) 
    
    Dim oOcc As ComponentOccurrence 
    For Each oOcc In Occurrences 
    Try
    oOcc.Definition.BOMStructure = BOMStructureEnum.kPhantomBOMStructure
    Catch
    'MsgBox(oOcc.Name & "remains unchanged")
    End Try
        ' Check to see if this occurrence represents a subassembly 
        ' and recursively call this function to traverse through it. 
        If oOcc.DefinitionDocumentType = kAssemblyDocumentObject Then
            Call TraverseAssembly(oOcc.SubOccurrences, Level + 1) 
        End If 
    Next
End Sub

t 

[brendan.henderson]

That did the job. Many thanks too you.

[brendan.henderson]

I don't know why but now this previously working macro fails. See the picture. Anybody know how to fix this? I'm still on 2014 if that matters.

[MechMachineMan]

Hi. It's failing because the code is written in VB.net, whereas the macro feature in inventor only works for VBA. However, the vb.net is still fine for use in rules and external rules.

Adding a "Set" in front of variable declarations converts most of it over.

ie; Set oAsmDoc = ThisApplication.ActiveDocument