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 objHelixProt As SolidEdgePart.HelixProtrusion
    Dim objHPItem As SolidEdgePart.HelixProtrusion
    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 the profile for the base feature and validating it
    Set objBaseProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objDoc.RefPlanes(1))
    Call objBaseProfile.Circles2d.AddByCenterRadius(x:=0, y:=0, Radius:=0.025)
    lngStatus = objBaseProfile.End(ValidationCriteria:=igProfileClosed)
    If (lngStatus <> 0) Then
        MsgBox "Profile for the base feature is not closed"
    End If
    ' creating the base extruded protrusion and validating it
    Set objBaseProfileArray(1) = objBaseProfile
    Set objBaseModel = objDoc.Models.AddFiniteExtrudedProtrusion(NumberOfProfiles:=1, _
                                                                 ProfileArray:=objBaseProfileArray, ProfilePlaneSide:=igSymmetric, ExtrusionDistance:=0.1)
    If (objDoc.Models(1).ExtrudedProtrusions(1).Status <> igFeatureOK) Then
        MsgBox "AddFiniteExtrudedProtrusion method of the Models object fails"
    End If
    objBaseProfile.Visible = False
    ' *** creating the Helix Protrusion feature with the Ref Axis and Cross Section in the same plane
    ' creating the cross-section and the 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:=0.05, y:=-0.05, Radius:=0.01)
    lngStatus = objProfile.End(ValidationCriteria:=igClosed)
    If (lngStatus <> 0) Then
        MsgBox "Cross-section for the helix protrusion feature is not closed"
    End If
    ' creating the helix protrusion and validating it
    Set objCSArray(1) = objProfile
    Set objHelixProt = objDoc.Models(1).HelixProtrusions.AddFinite(HelixAxis:=objRefAxis, _
                                                                   AxisStart:=igStart, NumCrossSections:=1, CrossSectionArray:=objCSArray, _
                                                                   ProfileSide:=igRight, Height:=0.1, Pitch:=0.05, NumberOfTurns:=2, HelixDir:=igRight)
    objProfile.Visible = False
    If (objHelixProt.Status <> igFeatureOK) Then
        MsgBox "AddFinite method of the HelixProtrusions object fails"
    End If
    ' getting a particular helix protrusion feature from the collection object
    Set objHPItem = objDoc.Models(1).HelixProtrusions.Item(1)
    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objProfile = Nothing
    Set objLine = Nothing
    Set objRefAxis = Nothing
    Set objCrossSection = Nothing
    Set objCSArray(1) = Nothing
    Set objHelixProt = Nothing
    Set objBaseProfile = Nothing
    Set objBaseModel = Nothing
    Set objBaseProfileArray(1) = Nothing
    Set objHPItem = Nothing
End Sub