Private Sub Form_Load()
    Dim objApp As SolidEdgeFramework.Application
    Dim objDoc As SolidEdgePart.PartDocument
    Dim objRefPlane As SolidEdgePart.RefPlane
    Dim objProfiles(1 To 3) As SolidEdgePart.Profile
    Dim objLines As SolidEdgeFrameworkSupport.Lines2d
    Dim objRelations As SolidEdgeFrameworkSupport.Relations2d
    Dim objLine(1 To 4) As SolidEdgeFrameworkSupport.Line2d
    Dim objBaseLines As SolidEdgeFrameworkSupport.Lines2d
    Dim objBaseProfile(1 To 2) As SolidEdgePart.Profile
    Dim objBaseRelns As SolidEdgeFrameworkSupport.Relations2d
    Dim objModel As SolidEdgePart.Model
    Dim objLoftCuts As SolidEdgePart.LoftedCutouts
    Dim objLoftCut As SolidEdgePart.LoftedCutout
    Dim lngStatus As Long
    Dim xOrigin As Double, yOrigin As Double
    Dim OriginArray(1 To 3) As Variant
    Dim Origin(1 To 2) As Double
    Dim SectionTypes(1 To 3) As Long
    Dim i As Integer
    Dim lngCnt 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
    ' Draw the Base Profile
    Set objBaseProfile(1) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:= _
                                                                objDoc.RefPlanes(1))
    Set objBaseLines = objBaseProfile(1).Lines2d
    Call objBaseLines.AddBy2Points(x1:=0, y1:=0, x2:=0.1, y2:=0)
    Call objBaseLines.AddBy2Points(x1:=0.1, y1:=0, x2:=0.1, y2:=0.1)
    Call objBaseLines.AddBy2Points(x1:=0.1, y1:=0.1, x2:=0, y2:=0.1)
    Call objBaseLines.AddBy2Points(x1:=0, y1:=0.1, x2:=0, y2:=0)
    ' Define Relations among the Line objects to make the Profile closed
    Set objBaseRelns = objBaseProfile(1).Relations2d
    Call objBaseRelns.AddKeypoint(Object1:=objBaseLines(1), Index1:=igLineEnd, Object2:= _
                                  objBaseLines(2), Index2:=igLineStart)
    Call objBaseRelns.AddKeypoint(Object1:=objBaseLines(2), Index1:=igLineEnd, Object2:= _
                                  objBaseLines(3), Index2:=igLineStart)
    Call objBaseRelns.AddKeypoint(Object1:=objBaseLines(3), Index1:=igLineEnd, Object2:= _
                                  objBaseLines(4), Index2:=igLineStart)
    Call objBaseRelns.AddKeypoint(Object1:=objBaseLines(4), Index1:=igLineEnd, Object2:= _
                                  objBaseLines(1), Index2:=igLineStart)

    ' Check for the Profile Validity
    lngStatus = objBaseProfile(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:=objBaseProfile, _
                                                             ProfilePlaneSide:=igRight, _
                                                             ExtrusionDistance:=0.1)
    objBaseProfile(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 a Lofted Cutout object
    ' Create a new reference plane.
    Set objRefPlane = objDoc.RefPlanes.AddParallelByDistance( _
                      ParentPlane:=objDoc.RefPlanes(2), Distance:=0.1, _
                      NormalSide:=igRight, Local:=True)
    ' Create a new profile set and profile to use for the first section.
    Set objProfiles(1) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:= _
                                                             objRefPlane)
    ' Get the model space origin relative to profile space.
    Call objProfiles(1).Convert3DCoordinate(x3d:=0, y3d:=0, z3d:=0, _
                                            x2d:=xOrigin, y2d:=yOrigin)
    ' Save the coordinates to define the start point for this profile.
    Origin(1) = 0.03
    Origin(2) = 0.03
    OriginArray(1) = Origin
    ' Set a reference to the Lines2d and Relations2d collections on the profile.
    Set objLines = objProfiles(1).Lines2d
    Set objRelations = objProfiles(1).Relations2d
    ' Draw 4 lines for the Rectangular profile graphics.
    Set objLine(1) = objLines.AddBy2Points(x1:=0.03, y1:=0.03, x2:=0.07, _
                                           y2:=0.03)
    Set objLine(2) = objLines.AddBy2Points(x1:=0.07, y1:=0.03, _
                                           x2:=0.07, y2:=0.07)
    Set objLine(3) = objLines.AddBy2Points(x1:=0.07, y1:=0.07, _
                                           x2:=0.03, y2:=0.07)
    Set objLine(4) = objLines.AddBy2Points(x1:=0.03, y1:=0.07, _
                                           x2:=0.03, y2:=0.03)
    ' Connect the lines with relationships
    Call objRelations.AddKeypoint(Object1:=objLine(1), Index1:=igLineEnd, Object2:= _
                                  objLine(2), Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objLine(2), Index1:=igLineEnd, Object2:= _
                                  objLine(3), Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objLine(3), Index1:=igLineEnd, Object2:= _
                                  objLine(4), Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objLine(4), Index1:=igLineEnd, Object2:= _
                                  objLine(1), Index2:=igLineStart)
    ' End and validate the profile.
    lngStatus = objProfiles(1).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox (" Invalid Profile")
    End If
    ' Turn off the display of the profile.
    objProfiles(1).Visible = False
    ' Create a new reference plane.
    Set objRefPlane = objDoc.RefPlanes.AddParallelByDistance( _
                      ParentPlane:=objDoc.RefPlanes(2), Distance:=0.05, _
                      NormalSide:=igRight, Local:=True)
    ' Create a new profile set and profile to use for the first section.
    Set objProfiles(2) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objRefPlane)
    ' Get the model space origin relative to profile space.
    Call objProfiles(2).Convert3DCoordinate(x3d:=0, y3d:=0, z3d:=0, _
                                            x2d:=xOrigin, y2d:=yOrigin)
    ' Save the coordinates to define the start point for this profile.
    Origin(1) = xOrigin
    Origin(2) = yOrigin
    OriginArray(2) = Origin
    ' Draw a circle.
    Call objProfiles(2).Circles2d.AddByCenterRadius(x:=0.05, y:= _
                                                    0.05, Radius:=0.015)
    ' End and validate the profile.
    lngStatus = objProfiles(2).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Invalid Profile")
    End If
    ' Turn off the display of the profile.
    objProfiles(2).Visible = False
    ' Create a new reference plane.
    Set objRefPlane = objDoc.RefPlanes.AddParallelByDistance( _
                      ParentPlane:=objDoc.RefPlanes(2), Distance:=0, _
                      NormalSide:=igRight, Local:=True)
    ' Create a new profile set and profile to use for the first section.
    Set objProfiles(3) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:= _
                                                             objRefPlane)
    ' Get the model space origin relative to profile space.
    Call objProfiles(3).Convert3DCoordinate(x3d:=0, y3d:=0, z3d:=0, _
                                            x2d:=xOrigin, y2d:=yOrigin)
    ' Save the coordinates to define the start point for this profile.
    Origin(1) = 0.03
    Origin(2) = 0.03
    OriginArray(3) = Origin
    ' Set a reference to the Lines2d and Relations2d collections on the profile.
    Set objLines = objProfiles(3).Lines2d
    Set objRelations = objProfiles(3).Relations2d
    ' Draw 4 lines for the Rectangular profile graphics.
    Set objLine(1) = objLines.AddBy2Points(x1:=0.03, y1:=0.03, x2:=0.07, _
                                           y2:=0.03)
    Set objLine(2) = objLines.AddBy2Points(x1:=0.07, y1:=0.03, _
                                           x2:=0.07, y2:=0.07)
    Set objLine(3) = objLines.AddBy2Points(x1:=0.07, y1:=0.07, _
                                           x2:=0.03, y2:=0.07)
    Set objLine(4) = objLines.AddBy2Points(x1:=0.03, y1:=0.07, _
                                           x2:=0.03, y2:=0.03)
    ' Connect the lines with relationships
    Call objRelations.AddKeypoint(Object1:=objLine(1), Index1:=igLineEnd, Object2:= _
                                  objLine(2), Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objLine(2), Index1:=igLineEnd, Object2:= _
                                  objLine(3), Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objLine(3), Index1:=igLineEnd, Object2:= _
                                  objLine(4), Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objLine(4), Index1:=igLineEnd, Object2:= _
                                  objLine(1), Index2:=igLineStart)
    ' End and validate the profile.
    lngStatus = objProfiles(3).End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Invalid Profile")
    End If
    ' Turn off the display of the profile.
    objProfiles(3).Visible = False
    For i = 1 To 3
        SectionTypes(i) = igProfileBasedCrossSection
    Next
    ' Build up an array of the origin positions.
    Set objLoftCut = objDoc.Models(1).LoftedCutouts.AddSimple(NumSections:=3, CrossSections:=objProfiles, _
                                                              CrossSectionTypes:=SectionTypes, Origins:=OriginArray, _
                                                              MaterialSide:=igLeft, StartTangentType:=igNone, _
                                                              EndTangentType:=igNone)

    ' Check the Status of the Feature
    If objLoftCut.Status <> igFeatureOK Then
        MsgBox ("AddSimple method of LoftedCutouts object failed")
    End If
    ' Create a LoftedCutouts collection object
    Set objLoftCuts = objModel.LoftedCutouts
    ' Get the Count property
    lngCnt = objLoftCuts.Count
    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objRefPlane = Nothing
    Set objProfiles(1) = Nothing
    Set objProfiles(2) = Nothing
    Set objProfiles(3) = Nothing
    Set objLine(1) = Nothing
    Set objLine(2) = Nothing
    Set objLine(3) = Nothing
    Set objLine(4) = Nothing
    Set objRelations = Nothing
    Set objLines = Nothing
    Set objBaseProfile(1) = Nothing
    Set objBaseLines = Nothing
    Set objBaseRelns = Nothing
    Set objModel = Nothing
    Set objLoftCuts = Nothing
    Set objLoftCut = Nothing
End Sub