Insert Extruded Reference Surface Example (VBA)

This example shows how to insert an extruded surface into a model.

'----------------------------------------------------------------------------
' 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]
'---------------------------------------------------------------------------
Option Explicit

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim boolstatus As Boolean
Dim longstatus As Long

Sub main()

    Set swApp = Application.SldWorks
    Set Part = swApp.NewDocument("C:\ProgramData\SolidWorks\SolidWorks 2012\templates\Part.prtdot", 0, 0, 0)
    swApp.ActivateDoc2 "Part1", False, longstatus
    Set Part = swApp.ActiveDoc
    Dim myModelView As SldWorks.ModelView
    Set myModelView = Part.ActiveView
    myModelView.FrameState = swWindowState_e.swWindowMaximized
    Part.SketchManager.InsertSketch True
    boolstatus = Part.Extension.SelectByID2("Front Plane", "PLANE", -0.03891024234798, 0.02968528649877, 3.646590412283E-04, False, 0, Nothing, 0)
    Part.ClearSelection2 True
    Dim vSkLines As Variant
    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 SldWorks.SketchSegment
    Set skSegment = Part.SketchManager.CreateCircle(0.053579, 0.013995, 0#, 0.06819, 0.018462, 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 SldWorks.FeatureManager
    Set 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