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 objRPProfile As solidEdgePart.Profile
    Dim objLine As SolidEdgeFrameworkSupport.Line2d
    Dim objRefAxis As solidEdgePart.RefAxis
    Dim objRevProt As solidEdgePart.RevolvedProtrusion
    Dim lngCount As Long
    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 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"
        Exit Sub
    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 (objBaseModel.ExtrudedProtrusions(1).Status <> igFeatureOK) Then
        MsgBox "AddFiniteExtrudedProtrusion method of the Models object fails"
        Exit Sub
    End If
    objBaseProfile.Visible = False
    ' *** creating a Revolved Protrusion on the base feature towards the left side
    ' creating the profile for the revolved protrusion feature
    Set objRPProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objDoc.RefPlanes(3))
    Call objRPProfile.Circles2d.AddByCenterRadius(x:=0.05, y:=0, Radius:=0.015)
    Set objLine = objRPProfile.Lines2d.AddBy2Points(x1:=0, y1:=-0.05, x2:=0, y2:=0.05)
    Set objRefAxis = objRPProfile.SetAxisOfRevolution(lineforaxis:=objLine)
    lngStatus = objRPProfile.End(ValidationCriteria:=igProfileClosed)
    If (lngStatus <> 0) Then
        MsgBox "Profile for the revolved protrusion feature is not closed"
        Exit Sub
    End If
    ' creating the revolved protrusion feature and validating it
    Set objRevProt = objBaseModel.RevolvedProtrusions.AddFinite(Profile:=objRPProfile, _
                                                                RefAxis:=objRefAxis, ProfileSide:=igLeft, ProfilePlaneSide:=igLeft, _
                                                                AngleOfRevolution:=PI)
    objRPProfile.Visible = False
    If (objRevProt.Status <> igFeatureOK) Then
        MsgBox "AddFinite method of the Revolved Protrusions object fails"
    End If
    ' getting the number of revolved protrusions in the model
    lngCount = objBaseModel.RevolvedProtrusions.Count
    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objBaseProfile = Nothing
    Set objBaseProfileArray(1) = Nothing
    Set objBaseModel = Nothing
    Set objRPProfile = Nothing
    Set objLine = Nothing
    Set objRefAxis = Nothing
    Set objRevProt = Nothing
End Sub