Private Sub Form_Load()
    Dim objApp As SolidEdgeFramework.Application
    Dim objDoc As SolidEdgePart.PartDocument
    Dim objProf2 As SolidEdgePart.Profile
    Dim objProf1 As SolidEdgePart.Profile
    Dim objProf3 As SolidEdgePart.Profile
    Dim objProfile(1 To 2) As SolidEdgePart.Profile
    Dim objExtCut As SolidEdgePart.ExtrudedCutout
    Dim objExtProt1 As SolidEdgePart.ExtrudedProtrusion
    Dim objExtProt2 As SolidEdgePart.ExtrudedProtrusion
    Dim objModel As SolidEdgePart.Model
    Dim objLines As SolidEdgeFrameworkSupport.Lines2d
    Dim objRelns As SolidEdgeFrameworkSupport.Relations2d
    Dim objRefPln As SolidEdgePart.RefPlane
    Dim lngStatus As Long
    ' Report errors
    Const PI = 3.14159265358979
    ' Create/get the application with specific settings
    On Error Resume Next
    Set objApp = GetObject(, "SolidEdge.Application")
    If Err Then
        Err.Clear
        Set objApp = CreateObject("SolidEdge.Application")
        Set objDoc = objApp.Documents.Add("SolidEdge.PartDocument")
        objApp.Visible = True
    Else
        Set objDoc = objApp.ActiveDocument
    End If
    'Draw the Base Profile
    Set objProfile(1) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objDoc.RefPlanes(3))
    Set objLines = objProfile(1).Lines2d
    Call objLines.AddBy2Points(x1:=0, y1:=0, x2:=0.08, y2:=0)
    Call objLines.AddBy2Points(x1:=0.08, y1:=0, x2:=0.08, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0.08, y1:=0.06, x2:=0.064, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0.064, y1:=0.06, x2:=0.064, y2:=0.02)
    Call objLines.AddBy2Points(x1:=0.064, y1:=0.02, x2:=0.048, y2:=0.02)
    Call objLines.AddBy2Points(x1:=0.048, y1:=0.02, x2:=0.048, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0.048, y1:=0.06, x2:=0.032, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0.032, y1:=0.06, x2:=0.032, y2:=0.02)
    Call objLines.AddBy2Points(x1:=0.032, y1:=0.02, x2:=0.016, y2:=0.02)
    Call objLines.AddBy2Points(x1:=0.016, y1:=0.02, x2:=0.016, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0.016, y1:=0.06, x2:=0, y2:=0.06)
    Call objLines.AddBy2Points(x1:=0, y1:=0.06, x2:=0, y2:=0)
    ' Define Relations among the Line objects to make the Profile closed
    Set objRelns = objProfile(1).Relations2d
    Call objRelns.AddKeypoint(Object1:=objLines(1), Index1:=igLineEnd, Object2:=objLines(2), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(2), Index1:=igLineEnd, Object2:=objLines(3), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(3), Index1:=igLineEnd, Object2:=objLines(4), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(4), Index1:=igLineEnd, Object2:=objLines(5), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(5), Index1:=igLineEnd, Object2:=objLines(6), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(6), Index1:=igLineEnd, Object2:=objLines(7), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(7), Index1:=igLineEnd, Object2:=objLines(8), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(8), Index1:=igLineEnd, Object2:=objLines(9), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(9), Index1:=igLineEnd, Object2:=objLines(10), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(10), Index1:=igLineEnd, Object2:=objLines(11), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(11), Index1:=igLineEnd, Object2:=objLines(12), Index2:=igLineStart)
    Call objRelns.AddKeypoint(Object1:=objLines(12), Index1:=igLineEnd, Object2:=objLines(1), Index2:=igLineStart)
    ' Check for the Profile Validity
    lngStatus = objProfile(1).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Profile not closed")
    End If
    'Create the Base Extruded Protrusion Feature
    Set objModel = objDoc.Models.AddFiniteExtrudedProtrusion(NumberOfProfiles:=1, _
                                                             ProfileArray:=objProfile, ProfilePlaneSide:= _
                                                             igRight, ExtrusionDistance:=0.05)
    objProfile(1).Visible = False
    ' Check the status of Base Feature
    If objModel.ExtrudedProtrusions(1).Status <> igFeatureOK Then
        MsgBox ("Error in the Creation of Base Protrusion Feature object")
    End If
    'Create 2nd ExtrudedProtrusion Feature object
    Set objRefPln = objDoc.RefPlanes.AddParallelByDistance(ParentPlane:=objDoc.RefPlanes(2), _
                                                           Distance:=0.08, NormalSide:=igRight)
    Set objProf2 = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objRefPln)
    Call objProf2.Circles2d.AddByCenterRadius(x:=-0.025, y:=0.03, Radius:=0.025)
    ' Check if the Profile is closed
    lngStatus = objProf2.End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Profile not closed")
    End If
    Set objExtProt1 = objModel.ExtrudedProtrusions.AddFinite(Profile:=objProf2, _
                                                             profileSide:=igRight, ProfilePlaneSide:=igRight, Depth:=0.04)
    objProf2.Visible = False
    If objExtProt1.Status <> igFeatureOK Then
        MsgBox ("AddFinite Method of ExtrudedProtrusions object failed")
    End If
    'Create 3rd ExtrudedProtrusion Feature object
    Set objRefPln = objDoc.RefPlanes.AddParallelByDistance(ParentPlane:=objDoc.RefPlanes(2), _
                                                           Distance:=0.12, NormalSide:=igRight)
    Set objProf3 = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objRefPln)
    Call objProf3.Circles2d.AddByCenterRadius(x:=-0.025, y:=0.03, Radius:=0.015)
    ' Check if the Profile is closed
    lngStatus = objProf3.End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Profile not closed")
    End If
    Set objExtProt2 = objModel.ExtrudedProtrusions.AddFinite(Profile:=objProf3, _
                                                             profileSide:=igLeft, ProfilePlaneSide:=igRight, Depth:=0.03)
    objProf3.Visible = False
    If objExtProt2.Status <> igFeatureOK Then
        MsgBox ("AddFinite Method of ExtrudedProtrusions object failed")
    End If
    '******** Create an ExtrudedCutout object
    ' Create a Circular Profile
    Set objRefPln = objDoc.RefPlanes.AddParallelByDistance(ParentPlane:=objDoc.RefPlanes(2), _
                                                           Distance:=0.01, NormalSide:=igRight)
    Set objProf1 = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objRefPln)
    Call objProf1.Circles2d.AddByCenterRadius(x:=-0.025, y:=0.03, Radius:=0.005)
    ' Check if the Profile is closed
    lngStatus = objProf1.End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Profile not closed")
    End If
    'Create the ExtrudedCutout feature
    Set objExtCut = objModel.ExtrudedCutouts.AddThroughAll(Profile:=objProf1, _
                                                           profileSide:=igLeft, ProfilePlaneSide:= _
                                                           igRight)
    objProf1.Visible = False
    If objExtCut.Status <> igFeatureOK Then
        MsgBox ("AddThroughAll Method of ExtrudedCutouts object failed")
    End If
    ' Reorder the Cutout object before ExtrudedProtrusion_3
    Call objExtCut.Reorder(TargetFeature:=objExtProt1, InsertBefore:=False)

    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objProf1 = Nothing
    Set objProf2 = Nothing
    Set objProf3 = Nothing
    Set objProfile(1) = Nothing
    Set objProfile(2) = Nothing
    Set objExtCut = Nothing
    Set objExtProt2 = Nothing
    Set objExtProt1 = Nothing
    Set objLines = Nothing
    Set objModel = Nothing
    Set objRelns = Nothing
    Set objRefPln = Nothing
End Sub