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 objRegHoleData As SolidEdgePart.HoleData
    Dim objCBoreHoleData As SolidEdgePart.HoleData
    Dim objCSinkHoleData As SolidEdgePart.HoleData
    Dim objRP As SolidEdgePart.RefPlane
    Dim objRegHoleProfile As SolidEdgePart.Profile
    Dim objCBoreHoleProfile As SolidEdgePart.Profile
    Dim objCSinkHoleProfile As SolidEdgePart.Profile
    Dim objRegHole As SolidEdgePart.Hole
    Dim objCBoreHole As SolidEdgePart.Hole
    Dim objCSinkHole As SolidEdgePart.Hole
    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 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 Regular Hole using the Holedatacollection object
    ' creating the hole data for a regular hole
    Set objRegHoleData = objDoc.HoleDataCollection.Add(HoleType:=igRegularHole, _
                                                       HoleDiameter:=0.01, BottomAngle:=90)
    ' creating a profile for the regular hole and validating it
    Set objRP = objDoc.RefPlanes.AddParallelByDistance(ParentPlane:=objDoc.RefPlanes(1), _
                                                       Distance:=0.025, NormalSide:=igRight)
    Set objRegHoleProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objRP)
    Call objRegHoleProfile.Holes2d.Add(xcenter:=0, ycenter:=0)
    lngStatus = objRegHoleProfile.End(ValidationCriteria:=igProfileClosed)
    If (lngStatus <> 0) Then
        MsgBox "Profile for the regular hole is not closed"
    End If
    ' creating the regular hole on the base feature and validating it
    Set objRegHole = objBase.Holes.AddFinite(Profile:=objRegHoleProfile, _
                                             ProfilePlaneSide:=igLeft, FiniteDepth:=0.02, Data:=objRegHoleData)
    If (objRegHole.Status <> igFeatureOK) Then
        MsgBox "AddFinite method of the Holes object fails"
    End If
    objRegHoleProfile.Visible = False

    ' *** creating a CounterBore Hole using the HoleDataCollection object
    ' creating the hole data for a counter bore hole
    Set objCBoreHoleData = objDoc.HoleDataCollection.Add(HoleType:=igCounterboreHole, _
                                                         HoleDiameter:=0.01, CounterboreDiameter:=0.02, CounterboreDepth:=0.01, BottomAngle:=0)
    ' creating a profile for the counter bore hole and validating it
    Set objCBoreHoleProfile = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objRP)
    Call objCBoreHoleProfile.Holes2d.Add(xcenter:=0.05, ycenter:=0)
    lngStatus = objCBoreHoleProfile.End(ValidationCriteria:=igProfileClosed)
    If (lngStatus <> 0) Then
        MsgBox "Profile for the regular hole is not closed"
    End If
    ' creating the counter bore hole on the base feature and validating it
    Set objCBoreHole = objBase.Holes.AddFinite(Profile:=objCBoreHoleProfile, _
                                               ProfilePlaneSide:=igLeft, FiniteDepth:=0.03, Data:=objCBoreHoleData)
    If (objCBoreHole.Status <> igFeatureOK) Then
        MsgBox "AddFinite method of the Holes object fails"
    End If
    objCBoreHoleProfile.Visible = False

    ' *** 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 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

    ' getting the number of HoleDatas in the HoleDataCollection object
    lngCount = objDoc.HoleDataCollection.Count
    ' USER DISPLAY
    ' Release objects
    Set objApp = Nothing
    Set objDoc = Nothing
    Set objBaseProfile = Nothing
    Set objBaseProfArray(1) = Nothing
    Set objBase = Nothing
    Set objRegHoleData = Nothing
    Set objCBoreHoleData = Nothing
    Set objCSinkHoleData = Nothing
    Set objRP = Nothing
    Set objRegHoleProfile = Nothing
    Set objCBoreHoleProfile = Nothing
    Set objCSinkHoleProfile = Nothing
    Set objRegHole = Nothing
    Set objCBoreHole = Nothing
    Set objCSinkHole = Nothing
End Sub