Insert Extruded Reference Surface Example (VB.NET)

'----------------------------------------------------------------------------
' Preconditions: Verify that the specified Part template exists.
'
' Postconditions: Boss-Extrude1, Surface-Extrude1,

' and 6 Solid Bodies are in the FeatureManager design tree.
'------------------------------------
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System

Partial Class SolidWorksMacro

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

    Sub main()

        Part = swApp.NewDocument("C:\ProgramData\SolidWorks\SolidWorks 2011\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 myFeature As Feature
        Dim myFeatMr As FeatureManager
        myFeatMr = Part.FeatureManager
        myFeature = myFeatMr.FeatureExtrusion2(True, False, False, 0, 0, 0.05, 0.01, False, False, False, False, 0.01745329251994, 0.01745329251994, False, False, False, False, False, False, False, 0, 0, False)

        boolstatus = Part.Extension.SelectByID2("", "FACE", -0.03303425584835, -0.002425135081921, 0.04999999999995, False, 0, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("", "FACE", 0.01139270278031, -0.006451084779542, 0.05000000000001, True, 256, Nothing, 0)
        boolstatus = Part.Extension.SelectByID2("", "FACE", 0.05275573322768, 0.01530932615179, 0.05000000000001, True, 256, Nothing, 0)

        myFeatMr.FeatureExtruRefSurface(False, False, False, 0, 0, 0.01, 0.01, False, False, False, False, 0.01745329251994, 0.01745329251994, False, False, False, False, True, True, False, False)

    End Sub

    
    Public swApp As SldWorks


End Class