Insert Extruded Reference Surface Example (VB.NET)

'----------------------------------------------------------------------------
' Preconditions: Verify that the specified Part template exists.
'
' Postconditions:
' 1. The FeatureManager design tree contains Surface-Extrude1.
' 2. The Surface Bodies folder contains:
'    * Surface-Extrude[1]
'    * Surface-Extrude[2]
'    * Surface-Extrude[3]
'---------------------------------------------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System.Runtime.InteropServices
Imports System

Partial Class SolidWorksMacro

    Dim Part As ModelDoc2
    Dim boolstatus As Boolean
    Dim longstatus As Long

    Sub main()

        Part = swApp.NewDocument("C:\ProgramData\SolidWorks\SolidWorks 2012\templates\Part.prtdot", 0, 0, 0)
        swApp.ActivateDoc2("Part1", False, longstatus)
        Part = swApp.ActiveDoc
        Dim myModelView As ModelView
        myModelView = Part.ActiveView
        myModelView.FrameState = swWindowState_e.swWindowMaximized
        Part.SketchManager.InsertSketch(True)
        boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -0.03891024234798, 0.02968528649877, 0.0003646590412283, False, 0, Nothing, 0)
        Part.ClearSelection2(True)
        Dim vSkLines As Object
        vSkLines = Part.SketchManager.CreateCornerRectangle(-0.05517876768764, 0.008130204900836, 0, -0.02399076855985, -0.0155939995639, 0)
        Part.ClearSelection2(True)
        vSkLines = Part.SketchManager.CreateCornerRectangle(-0.003731897331531, 0.008130204900836, 0, 0.0285223581767, -0.02998846069981, 0)
        Part.ClearSelection2(True)
        Dim skSegment As SketchSegment
        skSegment = Part.SketchManager.CreateCircle(0.053579, 0.013995, 0.0#, 0.06819, 0.018462, 0.0#)
        Part.ClearSelection2(True)
        Part.SketchManager.InsertSketch(True)
        Part.ShowNamedView2("*Trimetric", 8)
        Part.ClearSelection2(True)
        boolstatus = Part.Extension.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 0, Nothing, 0)

        Dim myFeatMr As FeatureManager
        myFeatMr = Part.FeatureManager

        ' Create a blind surface extrude of 10 mm in two directions from the selected sketch in a direction normal to the selected sketch plane
        myFeatMr.FeatureExtruRefSurface2(False, False, False, 0, 0, 0.01, 0.01, False, False, False, False, 0.01745329251994, 0.01745329251994, False, False, False, False, False, False, False, False)

    End Sub


    Public swApp As SldWorks


End Class