Sketch profile control

Public Sub SketchProfileControl()
    ' Create a new part document, using the default part template.
    Dim oPartDoc As PartDocument
    Set oPartDoc = ThisApplication.Documents.Add(kPartDocumentObject, _
    ThisApplication.FileManager.GetTemplateFile(kPartDocumentObject))
    
    ' Set a reference to the component definition.
    Dim oCompDef As PartComponentDefinition
    Set oCompDef = oPartDoc.ComponentDefinition
    
    ' Create a new sketch on the X-Y work plane. Since it's being created on
    ' one of the base workplanes we know the orientation it will be created in
    ' and don't need to worry about controlling it. Because of this we also
    ' know the origin of the sketch plane will be at (0,0,0) in model space.
    Dim oSketch As PlanarSketch
    Set oSketch = oCompDef.Sketches.Add(oCompDef.WorkPlanes(3))
    
    ' Set a reference to the transient geometry object.
    Dim oTransGeom As TransientGeometry
    Set oTransGeom = ThisApplication.TransientGeometry
    
    ' Draw 3 concentric circles.
    
    Dim oCircle1 As SketchCircle
    Set oCircle1 = oSketch.SketchCircles.AddByCenterRadius( _
    oTransGeom.CreatePoint2d(5, 5), 6)
    
    Dim oCircle2 As SketchCircle
    Set oCircle2 = oSketch.SketchCircles.AddByCenterRadius( _
    oTransGeom.CreatePoint2d(5, 5), 4)
    
    Dim oCircle3 As SketchCircle
    Set oCircle3 = oSketch.SketchCircles.AddByCenterRadius( _
    oTransGeom.CreatePoint2d(5, 5), 2)
    
    ' Create a profile.
    Dim oProfile As Profile
    Set oProfile = oSketch.Profiles.AddForSolid
    
    ' Modify the profile: the returned profile consists of 3
    ' paths each corresponding to a sketch circle. The desired
    ' result is that the innermost path removes material and the
    ' second path adds material. The outermost path is not needed
    ' and is hence deleted.
    Dim oProfPath As ProfilePath
    For Each oProfPath In oProfile
      If oProfPath.Item(1).SketchEntity Is oCircle3 Then
        oProfPath.AddsMaterial = False
      ElseIf oProfPath.Item(1).SketchEntity Is oCircle2 Then
        oProfPath.AddsMaterial = False
      Else
        oProfPath.Delete
      End If
    Next
    
    ' Create a base extrusion 1cm thick.
    Dim oExtrudeDef As ExtrudeDefinition
    Set oExtrudeDef = oCompDef.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, kJoinOperation)
    Call oExtrudeDef.SetDistanceExtent(1, kNegativeExtentDirection)
    Dim oExtrude As ExtrudeFeature
    Set oExtrude = oCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef)
    
    'Make the sketch visible for better visualization
    oSketch.Visible = True
End Sub