Private Sub Form_Load()
    Dim objApp As SolidEdgeFramework.Application
    Dim objDoc As SolidEdgePart.PartDocument
    Dim objProf As SolidEdgePart.Profile
    Dim objProfile(1 To 2) As SolidEdgePart.Profile
    Dim objExtProt As SolidEdgePart.ExtrudedProtrusion
    Dim objModel As SolidEdgePart.Model
    Dim objLines As SolidEdgeFrameworkSupport.Lines2d
    Dim objRelns As SolidEdgeFrameworkSupport.Relations2d
    Dim objRefPln As SolidEdgePart.RefPlane
    Dim objMProfile As SolidEdgePart.Profile
    Dim objL1 As SolidEdgeFrameworkSupport.Line2d
    Dim objL2 As SolidEdgeFrameworkSupport.Line2d
    Dim objL3 As SolidEdgeFrameworkSupport.Line2d
    Dim objL4 As SolidEdgeFrameworkSupport.Line2d
    Dim objRelations As SolidEdgeFrameworkSupport.Relations2d
    Dim objProfCollection As SolidEdgePart.Profiles
    Dim objMExtprot As SolidEdgePart.ExtrudedProtrusion
    Dim objProfArray(1 To 2) As SolidEdgePart.Profile
    Dim objGetProfArray(1 To 2) As SolidEdgePart.Profile
    Dim i As Integer
    Dim lngStatus As Long
    Dim lngNumProfiles 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 a Finite ExtrudedProtrusion with multiple profiles with profileplaneside \
    ' set to igRight
    Set objRefPln = objDoc.RefPlanes.AddParallelByDistance(ParentPlane:=objDoc.RefPlanes(2), _
                                                           Distance:=0.08, NormalSide:=igRight)
    Set objMProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objRefPln)
    'Draw two closed profiles and validate the same
    Call objMProfile.Circles2d.AddByCenterRadius(x:=-0.04, y:=0.05, Radius:=0.005)
    Set objL1 = objMProfile.Lines2d.AddBy2Points(x1:=-0.015, y1:=0.025, x2:=-0.015, y2:=0.035)
    Set objL2 = objMProfile.Lines2d.AddBy2Points(x1:=-0.015, y1:=0.035, x2:=-0.04, y2:=0.035)
    Set objL3 = objMProfile.Lines2d.AddBy2Points(x1:=-0.04, y1:=0.035, x2:=-0.04, y2:=0.025)
    Set objL4 = objMProfile.Lines2d.AddBy2Points(x1:=-0.04, y1:=0.025, x2:=-0.015, y2:=0.025)
    Set objRelations = objMProfile.Relations2d
    Call objRelations.AddKeypoint(Object1:=objL1, Index1:=igLineEnd, Object2:=objL2, Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objL2, Index1:=igLineEnd, Object2:=objL3, Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objL3, Index1:=igLineEnd, Object2:=objL4, Index2:=igLineStart)
    Call objRelations.AddKeypoint(Object1:=objL4, Index1:=igLineEnd, Object2:=objL1, Index2:=igLineStart)
    lngStatus = objMProfile.End(ValidationCriteria:=igProfileClosed)
    If lngStatus <> 0 Then
        MsgBox ("Profile not colsed")
    End If
    Set objProfCollection = objMProfile.Parent.Profiles
    For i = 1 To objProfCollection.Count
        Set objProfArray(i) = objProfCollection(i)
        objProfArray(i).Visible = False
    Next i
    Set objMExtprot = objModel.ExtrudedProtrusions.AddFiniteMulti(NumberOfProfiles:=2, _
                                                                  profileArray:=objProfArray, profileplaneSide:=igRight, Depth:=0.05)
    'Verify the Feature created
    If objMExtprot.Status <> igFeatureOK Then
        MsgBox "AddFiniteMulti method failed to create a feature with profileplaneside as igRight"
    End If
    'Get the profiles associated with the Feature
    Call objMExtprot.GetProfiles(numprofiles:=lngNumProfiles, Profiles:=objGetProfArray)
    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objProf = Nothing
    Set objProfile(1) = Nothing
    Set objProfile(2) = Nothing
    Set objModel = Nothing
    Set objExtProt = Nothing
    Set objLines = Nothing
    Set objRelns = Nothing
    Set objRefPln = Nothing
    Set objMProfile = Nothing
    Set objL1 = Nothing
    Set objL2 = Nothing
    Set objL3 = Nothing
    Set objL4 = Nothing
    Set objRelations = Nothing
    Set objProfCollection = Nothing
    Set objMExtprot = Nothing
    Set objProfArray(1) = Nothing
    Set objProfArray(2) = Nothing
    Set objGetProfArray(1) = Nothing
    Set objGetProfArray(2) = Nothing
End Sub