Insert Extruded Reference Surface Example (VB.NET)

'----------------------------------------------------------------------------
' Preconditions:
' 1. Verify that the specified part template exists.
' 2. Open the Immediate window.
'
' Postconditions:
' 1. Creates Surface-Extrude1 in the FeatureManager design tree.
' 2. Expand the Surface Bodies folder to verify that it contains:
'    * Surface-Extrude[1]
'    * Surface-Extrude[2]
'    * Surface-Extrude[3]
' 3. Inspect the Immediate window.
'---------------------------------------------------------------------------
Imports SolidWorks.Interop.swconst
Imports SolidWorks.Interop.sldworks
Imports System.Runtime.InteropServices
Imports System
Imports System.Diagnostics
 
Partial Class SolidWorksMacro
 
    Dim Part As ModelDoc2
    Dim selMgr As SelectionMgr
    Dim surfExtrudeFeat As Feature
    Dim surfExtrude As SurfExtrudeFeatureData
    Dim boolstatus As Boolean
    Dim longstatus As Integer
 
    Sub main()
 
        Part = swApp.NewDocument("C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2016\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)
 
        Part.ClearSelection2(True)
        selMgr = Part.SelectionManager
 
        ' Get Surface-Extrude1 data
        boolstatus = Part.Extension.SelectByID2("Surface-Extrude1", "BODYFEATURE", 0, 0, 0, False, 0, Nothing, 0)
 
        surfExtrudeFeat = selMgr.GetSelectedObject6(1, -1)
        surfExtrude = surfExtrudeFeat.GetDefinition
 
        surfExtrude.AccessSelections(Part, Nothing)
 
        Debug.Print(surfExtrudeFeat.Name)
        Debug.Print("  Depth:")
        Debug.Print("    Forward direction: " & surfExtrude.GetDepth(True))
        Debug.Print("    Reverse direction: " & surfExtrude.GetDepth(False))
        Debug.Print("  End condition as defined in swSurfaceExtendEndCond_e:")
        Debug.Print("    Forward direction: " & surfExtrude.GetEndCondition(True))
        Debug.Print("    Reverse direction: " & surfExtrude.GetEndCondition(False))
        Debug.Print("  Reverse offset enabled:")
        Debug.Print("    Forward direction? " & surfExtrude.GetReverseOffset(True))
        Debug.Print("    Reverse direction? " & surfExtrude.GetReverseOffset(False))
        Debug.Print("  Translate surface setting enabled:")
        Debug.Print("    Forward direction? " & surfExtrude.GetTranslateSurface(True))
        Debug.Print("    Reverse direction? " & surfExtrude.GetTranslateSurface(False))
        Debug.Print("  Surface extruded in both directions? " & surfExtrude.BothDirections)
        Debug.Print("  Extrusion reversed? " & surfExtrude.ReverseDirection)
 
        surfExtrude.ReleaseSelectionAccess()
 
    End Sub
 
 
    Public swApp As SldWorks
 
 
End Class