Change the Plane of a Sketch Example (VB.NET)

'----------------------------------------------------------------------------
' Preconditions: Verify that the specified template exists.
'
' Postconditions:
' 1. Creates a new part document with a sketch of a spline.
' 2. Changes the plane of the sketch Top Plane to the Front Plane.
' 3. Examine the FeatureManager design tree and graphics area.
'----------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System

Partial Class SolidWorksMacro

    Dim Part As ModelDoc2
    Dim skSegment As SketchSegment
    Dim boolstatus As Boolean


    Sub main()

        Part = swApp.NewDocument("C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2017\templates\Part.prtdot", 0, 0, 0)

        boolstatus = Part.Extension.SelectByID2("Top Plane", "PLANE", -0.0494443883882606, 0.010829578664819, 0.0187336739521956, True, 0, Nothing, 0)
        Part.SketchManager.InsertSketch(True)

        Dim pointArray As Object
        Dim points(11) As Double

        points(0) = -0.0696700449874595
        points(1) = -0.0205096087491173
        points(2) = 0
        points(3) = -0.0349133034431539
        points(4) = 0.0151865041882777
        points(5) = 0
        points(6) = 0.0183177421652422
        points(7) = 0
        points(8) = 0
        points(9) = 0.060902578651959
        points(10) = 0.0336608082523681
        points(11) = 0
        pointArray = points

        skSegment = Part.SketchManager.CreateSpline((pointArray))
        Part.SketchManager.InsertSketch(True)

        boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("Top Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)
        boolstatus = Part.DeSelectByID("Top Plane", "PLANE", 0, 0, 0)

        ' Select sketch and new plane for the sketch
        boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)
        ' Change the plane of the sketch
        boolstatus = Part.Extension.ChangeSketchPlane(1, Nothing)
        boolstatus = Part.EditRebuild3()

        Part.ShowNamedView2("*Isometric", 7)
        boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", 0, 0, 0, True, 0, Nothing, 0)

    End Sub


    Public swApp As SldWorks


End Class