Private Sub Form_Load()
    Dim objApp As SolidEdgeFramework.Application
    Dim objDoc As SolidEdgePart.PartDocument
    Dim objBaseProfile(1 To 2) As SolidEdgePart.Profile
    Dim objLine1 As SolidEdgeFrameworkSupport.Line2d
    Dim objLine2 As SolidEdgeFrameworkSupport.Line2d
    Dim objArc1 As SolidEdgeFrameworkSupport.Arc2d
    Dim objArc2 As SolidEdgeFrameworkSupport.Arc2d
    Dim objModel As SolidEdgePart.Model
    Dim objExtProtrusion As SolidEdgePart.ExtrudedProtrusion
    Dim objRelations As SolidEdgeFrameworkSupport.Relations2d
    Dim objTraceRefPlane As SolidEdgePart.RefPlane
    Dim objTraceprofile(1 To 2) As SolidEdgePart.Profile
    Dim objCSRefPlane As SolidEdgePart.RefPlane
    Dim objCSProfile(1 To 2) As SolidEdgePart.Profile
    Dim vOriginArray(2) As Variant
    Dim objCutoutProfile As SolidEdgePart.Profile
    Dim objCutout As SolidEdgePart.ExtrudedCutout
    Dim objSweptCutout As SolidEdgePart.SweptCutout
    Dim lngStatus As Long
    Dim lngTraceCurveTypes(1 To 2) As Long
    Dim lngCrossSectionTypes(1 To 2) 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
    On Error GoTo 0
    '*************** Create an Extruded Protrusion as Base feature
    'Draw the base Profile
    Set objBaseProfile(1) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objDoc.RefPlanes(1))
    Set objLine1 = objBaseProfile(1).Lines2d.AddBy2Points(x1:=0.05, y1:=0, x2:=0.05, y2:=0.15)
    Set objArc1 = objBaseProfile(1).Arcs2d.AddByCenterStartEnd(xCenter:=0.025, yCenter:=0.15, _
                                                               xStart:=0.05, yStart:=0.15, xEnd:=0, yEnd:=0.15)
    Set objLine2 = objBaseProfile(1).Lines2d.AddBy2Points(x1:=0, y1:=0.15, x2:=0, y2:=0)
    Set objArc2 = objBaseProfile(1).Arcs2d.AddByCenterStartEnd(xCenter:=0.025, yCenter:=0, _
                                                               xStart:=0, yStart:=0, xEnd:=0.05, yEnd:=0)
    ' Define Relations among the Line and Arc objects to make the Profile closed
    Set objRelations = objBaseProfile(1).Relations2d
    Call objRelations.AddKeypoint(Object1:=objLine1, Index1:=igLineEnd, _
                                  Object2:=objArc1, Index2:=igArcStart)
    Call objRelations.AddKeypoint(Object1:=objArc1, Index1:=igArcEnd, _
                                  Object2:=objLine2, Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objLine2, Index1:=igLineEnd, _
                                  Object2:=objArc2, Index2:=igArcStart)
    Call objRelations.AddKeypoint(Object1:=objArc2, Index1:=igArcEnd, _
                                  Object2:=objLine1, Index2:=igLineStart)
    ' Check for the Profile Validity
    lngStatus = objBaseProfile(1).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Base feature profile is not closed")
    End If
    'Create the Base Extruded Protrusion Feature
    Set objModel = objDoc.Models.AddFiniteExtrudedProtrusion(NumberOfProfiles:=1, ProfileArray:=objBaseProfile, _
                                                             ProfilePlaneSide:=igRight, ExtrusionDistance:=0.05)
    objBaseProfile(1).Visible = False
    Set objExtProtrusion = objModel.ExtrudedProtrusions(1)
    ' Check the status of Base Feature
    If objExtProtrusion.Status <> igFeatureOK Then
        MsgBox "Base Feature is not created properly"
    End If
    '*********Create a simple Cutout. SweptCutout will be reordered ahaead of this cutout
    Set objCutoutProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objDoc.RefPlanes(2))
    Call objCutoutProfile.Circles2d.AddByCenterRadius(x:=0.01, y:=0.025, Radius:=0.005)
    ' Check for the Profile Validity
    lngStatus = objCutoutProfile.End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox "Cutout feature profile not closed"
    End If
    ' Create a ExtrudedCutout feature
    Set objCutout = objModel.ExtrudedCutouts.AddFinite(Profile:=objCutoutProfile, ProfileSide:=igLeft, _
                                                       ProfilePlaneSide:=igRight, Depth:=0.025)
    objCutoutProfile.Visible = False
    ' Check the status of ExtrudedCutout Feature
    If objCutout.Status <> igFeatureOK Then
        MsgBox "Cutout feature failed"
    End If

    '****************** Create SweptCutout with Add method
    'Draw the Trace profile
    Set objTraceRefPlane = objDoc.RefPlanes.AddParallelByDistance(ParentPlane:=objDoc.RefPlanes(1), _
                                                                  Distance:=0.05, NormalSide:=igRight, Local:=True)
    Set objTraceprofile(1) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objTraceRefPlane)
    Set objLine1 = objTraceprofile(1).Lines2d.AddBy2Points(x1:=0.05, y1:=0, x2:=0.05, y2:=0.15)
    Set objArc1 = objTraceprofile(1).Arcs2d.AddByCenterStartEnd(xCenter:=0.025, yCenter:=0.15, _
                                                                xStart:=0.05, yStart:=0.15, xEnd:=0, yEnd:=0.15)
    Set objLine2 = objTraceprofile(1).Lines2d.AddBy2Points(x1:=0, y1:=0.15, x2:=0, y2:=0)
    Set objArc2 = objTraceprofile(1).Arcs2d.AddByCenterStartEnd(xCenter:=0.025, yCenter:=0, _
                                                                xStart:=0, yStart:=0, xEnd:=0.05, yEnd:=0)
    ' Define Relations among the Line and Arc objects to make the Trace Profile closed
    Set objRelations = objTraceprofile(1).Relations2d
    Call objRelations.AddKeypoint(Object1:=objLine1, Index1:=igLineEnd, _
                                  Object2:=objArc1, Index2:=igArcStart)
    Call objRelations.AddKeypoint(Object1:=objArc1, Index1:=igArcEnd, _
                                  Object2:=objLine2, Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objLine2, Index1:=igLineEnd, _
                                  Object2:=objArc2, Index2:=igArcStart)
    Call objRelations.AddKeypoint(Object1:=objArc2, Index1:=igArcEnd, _
                                  Object2:=objLine1, Index2:=igLineStart)
    ' Check for the Trace Profile Validity
    lngStatus = objTraceprofile(1).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Trace profile is not closed")
    End If
    ' Create a reference plane for Cross section profile
    Set objCSRefPlane = objDoc.RefPlanes.AddNormalToCurve( _
                        Curve:=objLine1, _
                        PlanePoint:=igCurveStart, _
                        OrientationPlaneOrPivot:=objDoc.RefPlanes(1), _
                        PivotOrigin:=igPivotEnd, _
                        Local:=True, _
                        ParentCurve:=objTraceprofile(1))
    ' Draw the Cross Section profile
    Set objCSProfile(1) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objCSRefPlane)
    Call objCSProfile(1).Circles2d.AddByCenterRadius(x:=0, y:=0, Radius:=0.01)
    ' Check for the Cross section Profile Validity
    lngStatus = objCSProfile(1).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Cross-section profile is not closed")
    End If
    'Create SweptCutout Feature
    lngTraceCurveTypes(1) = igProfileBasedCrossSection
    lngCrossSectionTypes(1) = igProfileBasedCrossSection
    vOriginArray(1) = 0
    Set objSweptCutout = objModel.SweptCutouts.Add(NumCurves:=1, _
                                                   TraceCurves:=objTraceprofile, TraceCurveTypes:=lngTraceCurveTypes, NumSections:=1, _
                                                   CrossSections:=objCSProfile, CrossSectionTypes:=lngCrossSectionTypes, _
                                                   Origins:=vOriginArray, SegmentMaps:=0, MaterialSide:=igLeft, StartExtentType:=igNone, _
                                                   StartExtentDistance:=0, StartSurfaceOrRefPlane:=Nothing, EndExtentType:=igNone, _
                                                   EndExtentDistance:=0, EndSurfaceOrRefPlane:=Nothing)
    objTraceprofile(1).Visible = False
    objCSProfile(1).Visible = False
    ' Check the status of SweptCutout Feature
    If objSweptCutout.Status <> igFeatureOK Then
        MsgBox "Add method of the SweptCutouts object Failed"
    End If
    'Reorder the SweptCutout feature ahead of Cutout
    Call objSweptCutout.Reorder(TargetFeature:=objExtProtrusion, InsertBefore:=False)

    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objBaseProfile(1) = Nothing
    Set objBaseProfile(2) = Nothing
    Set objLine1 = Nothing
    Set objLine2 = Nothing
    Set objArc1 = Nothing
    Set objArc2 = Nothing
    Set objModel = Nothing
    Set objExtProtrusion = Nothing
    Set objRelations = Nothing
    Set objTraceRefPlane = Nothing
    Set objTraceprofile(1) = Nothing
    Set objTraceprofile(2) = Nothing
    Set objCSRefPlane = Nothing
    Set objCSProfile(1) = Nothing
    Set objCSProfile(2) = Nothing
    Set vOriginArray(1) = Nothing
    Set vOriginArray(2) = Nothing
    Set objCutoutProfile = Nothing
    Set objCutout = Nothing
    Set objSweptCutout = Nothing
End Sub