Private Sub Form_Load()
    Dim objApp As SolidEdgeFramework.Application
    Dim objDoc As SolidEdgepart.PartDocument
    Dim objBaseProfile As SolidEdgepart.Profile
    Dim objBaseProfArray(1 To 2) As SolidEdgepart.Profile
    Dim objBase As SolidEdgepart.Model
    Dim objCSinkHoleData As SolidEdgepart.HoleData
    Dim objRP As SolidEdgepart.RefPlane
    Dim objCSinkHoleProfile As SolidEdgepart.Profile
    Dim objCSinkHole As SolidEdgepart.Hole
    Dim dblCSDiameter As Double
    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 an extruded protrusion base feature
    ' creating a circular 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:=0.1)
    lngStatus = objBaseProfile.End(ValidationCriteria:=igProfileClosed)
    If (lngStatus <> 0) Then
        MsgBox "Profile for the base feature is not closed"
    End If
    ' creating the extruded protrusion and validating it
    Set objBaseProfArray(1) = objBaseProfile
    Set objBase = objDoc.Models.AddFiniteExtrudedProtrusion(NumberOfProfiles:=1, _
                                                            ProfileArray:=objBaseProfArray, ProfilePlaneSide:=igSymmetric, ExtrusionDistance:=0.05)
    objBaseProfile.Visible = False
    If (objBase.ExtrudedProtrusions(1).Status <> igFeatureOK) Then
        MsgBox "AddFiniteExtrudedProtrusion method of models object fails"
    End If
    ' *** creating a Counter-Sunk Hole using the Holedatacollection object
    ' creating the hole data for a counter sunk hole
    Set objCSinkHoleData = objDoc.HoleDataCollection.Add(HoleType:=igCountersinkHole, _
                                                         HoleDiameter:=0.01, CountersinkDiameter:=0.02, CountersinkAngle:=100, BottomAngle:=0)
    ' creating a profile for the counter sunk hole and validating it
    Set objRP = objDoc.RefPlanes(1)
    Set objCSinkHoleProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objRP)
    Call objCSinkHoleProfile.Holes2d.Add(xcenter:=0, ycenter:=0.05)
    lngStatus = objCSinkHoleProfile.End(ValidationCriteria:=igProfileClosed)
    If (lngStatus <> 0) Then
        MsgBox "Profile for the counter sunk hole is not closed"
    End If
    ' creating the counter sunk hole on the base feature and validating it
    Set objCSinkHole = objBase.Holes.AddThroughAll(Profile:=objCSinkHoleProfile, _
                                                   ProfilePlaneSide:=igLeft, Data:=objCSinkHoleData)
    If (objCSinkHole.Status <> igFeatureOK) Then
        MsgBox "AddFinite method of the Holes object fails"
    End If
    objCSinkHoleProfile.Visible = False
    ' reading and modifying the counter sink diameter of the countersunk hole
    dblCSDiameter = objCSinkHoleData.CountersinkDiameter
    objCSinkHoleData.CountersinkDiameter = dblCSDiameter + 0.005
    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objBaseProfile = Nothing
    Set objBaseProfArray(1) = Nothing
    Set objBase = Nothing
    Set objCSinkHoleData = Nothing
    Set objRP = Nothing
    Set objCSinkHoleProfile = Nothing
    Set objCSinkHole = Nothing
End Sub