Private Sub Form_Load()
    Dim objApp As SolidEdgeFramework.Application
    Dim objDoc As SolidEdgePart.PartDocument
    Dim objBaseProfile As SolidEdgePart.Profile
    Dim objBaseProfileArray(1 To 2) As SolidEdgePart.Profile
    Dim objBaseModel As SolidEdgePart.Model
    Dim objProfile As SolidEdgePart.Profile
    Dim objLine As SolidEdgeFrameworkSupport.Line2d
    Dim objRefAxis As SolidEdgePart.RefAxis
    Dim objCrossSection As SolidEdgeFrameworkSupport.Circle2d
    Dim objCSArray(1 To 2) As SolidEdgePart.Profile
    Dim objHelixCutout As SolidEdgePart.HelixCutout
    Dim objHCItem As SolidEdgePart.HelixCutout
    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
    ' *** creating the base feature
    ' creating a circular profile for the base extruded protrusion feature and validating it
    Set objBaseProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objDoc.RefPlanes(1))
    Call objBaseProfile.Circles2d.AddByCenterRadius(x:=0, y:=0, Radius:=0.05)
    lngStatus = objBaseProfile.End(ValidationCriteria:=igProfileClosed)
    If (lngStatus <> 0) Then
        MsgBox "Profile for the base feature is not closed"
        Exit Sub
    End If
    ' creating the base extruded protrusion feature
    Set objBaseProfileArray(1) = objBaseProfile
    Set objBaseModel = objDoc.Models.AddFiniteExtrudedProtrusion(NumberOfProfiles:=1, _
                                                                 ProfileArray:=objBaseProfileArray, ProfilePlaneSide:=igSymmetric, ExtrusionDistance:=0.1)
    objBaseProfile.Visible = False
    ' *** creating a helix cutout feature
    ' creating a circular cross-section and a reference axis
    Set objProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objDoc.RefPlanes(2))
    Set objLine = objProfile.Lines2d.AddBy2Points(x1:=0, y1:=0.05, x2:=0, y2:=-0.05)
    Set objRefAxis = objProfile.SetAxisOfRevolution(LineForAxis:=objLine)
    Set objCrossSection = objProfile.Circles2d.AddByCenterRadius(x:=0.025, y:=-0.05, Radius:=0.01)
    Set objCSArray(1) = objProfile
    ' creating the helix cutout feature and validating it
    Set objHelixCutout = objDoc.Models(1).HelixCutouts.AddFinite(HelixAxis:=objRefAxis, _
                                                                 AxisStart:=igEnd, NumCrossSections:=1, CrossSectionArray:=objCSArray, _
                                                                 ProfileSide:=igRight, Height:=0.1, Pitch:=0.025, NumberOfTurns:=5, HelixDir:=igRight)
    objProfile.Visible = False
    If (objHelixCutout.Status <> igFeatureOK) Then
        MsgBox "AddFinite method of the HelixCutouts object fails"
    End If
    ' getting an item from the helix cutouts collection object
    Set objHCItem = objDoc.Models(1).HelixCutouts.Item(1)
    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objBaseProfile = Nothing
    Set objBaseProfileArray(1) = Nothing
    Set objBaseModel = Nothing
    Set objProfile = Nothing
    Set objLine = Nothing
    Set objRefAxis = Nothing
    Set objCrossSection = Nothing
    Set objCSArray(1) = Nothing
    Set objHelixCutout = Nothing
    Set objHCItem = Nothing
End Sub