Adding Centerlines from work features

[garrettfulghum]

Hello everyone,

Im currently almost finished with an automated dimension program for drawings based on Work-planes in the model. It does work, however I cant seem to access work-planes from inside a sub Component Occurrence within the main assembly. Here's What I have:

Public shared function CreateLinearDimensionV2(ViewName as string, WorkPlane1 As String, WorkPlane2 As String, Optional SubOccurenceName As string = Nothing)
InvApp = Marshal.GetActiveObject("Inventor.Application")
        Dim oDoc As Inventor.DrawingDocument

        Dim DrawingView As Inventor.DrawingView
        Dim oSheet As Sheet
        Dim DimOffsetHeight As Decimal = 1

        Try
            oDoc = InvApp.ActiveDocument

            oSheet = oDoc.ActiveSheet
            DrawingView = DrawingViewScan(oSheet, ViewName)
        Catch ex As Exception
            Console.WriteLine("Drawing Document not open.")
            Return False
        End Try
        '
        Dim oSubDoc As AssemblyDocument
        oSubDoc = DrawingView.ReferencedDocumentDescriptor.ReferencedDocument

        Dim oOcc1 As Inventor.WorkPlane
        Dim oOcc2 As Inventor.WorkPlane

        Dim Line1 As Centerline
        Dim Line2 As Centerline
        If (SubOccurenceName IsNot Nothing) Then
            'If user has given a sub name then try and find the occurence and get the work planes
            Dim oPartDoc1 As ComponentOccurrence
            Try
                oPartDoc1 = oSubDoc.ComponentDefinition.Occurrences.ItemByName(SubOccurenceName)
            Catch
                Console.WriteLine("Unable to find SubOccurence.")
                Return False
            End Try
            oOcc1 = oPartDoc1.Definition.WorkPlanes.Item(WorkPlane1)
            oOcc2 = oPartDoc1.Definition.WorkPlanes.Item(WorkPlane2)
        Else
            'If no sub part is specified just get the planes in the main assembly
            oOcc1 = oSubDoc.ComponentDefinition.WorkPlanes.Item(WorkPlane1)
            oOcc2 = oSubDoc.ComponentDefinition.WorkPlanes.Item(WorkPlane2)
        End If


        Line1 = oSheet.Centerlines.AddByWorkFeature(oOcc1, DrawingView)  'Program breaks when SubOccurenceName is provided
        Line2 = oSheet.Centerlines.AddByWorkFeature(oOcc2, DrawingView)
 .   .   .

 So here's the break down, when I give 'SubOccurenceName' a sub assembly it then finds the work-planes I provided in that occurrence, then program breaks at the creation of the center lines. (Gives a useless error... as always)  It definitely finds the work-planes It just has to be something with the Center-lines. It works great when the planes are in the context of the main assembly (Where 'SubOccurenceName' is nothing)! 

Im thinking its probably something simple I just cant figure it out!

Any Help would be appreciated, Thanks!

[garrettfulghum · Accepted solution]

Alright! I figured it out! Apparently I just needed to call the planes as a workplaneproxy! Super simple like i thought!

Dim oAsmPlane1 As WorkPlaneProxy
    Call oPartDoc1.CreateGeometryProxy(oOcc1, oAsmPlane1)

    Dim oAsmPlane2 As WorkPlaneProxy
    Call oPartDoc1.CreateGeometryProxy(oOcc2, oAsmPlane2)

Then I just replaced the plane in the centerlines.addbyworkfeature:

Line1 = oSheet.Centerlines.AddByWorkFeature(oAsmPlane1, DrawingView)