Private Sub Form_Load()
Dim objApp As SolidEdgeFramework.Application
Dim objDoc As SolidEdgePart.PartDocument
Dim objProf As SolidEdgePart.Profile
Dim objProfile(1 To 2) As SolidEdgePart.Profile
Dim objModel As SolidEdgePart.Model
Dim objExtCut As SolidEdgePart.ExtrudedCutout
Dim objLines As SolidEdgeFrameworkSupport.Lines2d
Dim objRelns As SolidEdgeFrameworkSupport.Relations2d
Dim objRefPln As SolidEdgePart.RefPlane
Dim objFeatures As SolidEdgePart.Features
Dim objExtCut1 As SolidEdgePart.ExtrudedCutout
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
'Draw the Base Profile
Set objProfile(1) = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:= _
objDoc.RefPlanes(3))
Set objLines = objProfile(1).Lines2d
Call objLines.AddBy2Points(x1:=0, y1:=0, x2:=0.08, y2:=0)
Call objLines.AddBy2Points(x1:=0.08, y1:=0, x2:=0.08, y2:=0.06)
Call objLines.AddBy2Points(x1:=0.08, y1:=0.06, x2:=0.064, y2:=0.06)
Call objLines.AddBy2Points(x1:=0.064, y1:=0.06, x2:=0.064, y2:=0.02)
Call objLines.AddBy2Points(x1:=0.064, y1:=0.02, x2:=0.048, y2:=0.02)
Call objLines.AddBy2Points(x1:=0.048, y1:=0.02, x2:=0.048, y2:=0.06)
Call objLines.AddBy2Points(x1:=0.048, y1:=0.06, x2:=0.032, y2:=0.06)
Call objLines.AddBy2Points(x1:=0.032, y1:=0.06, x2:=0.032, y2:=0.02)
Call objLines.AddBy2Points(x1:=0.032, y1:=0.02, x2:=0.016, y2:=0.02)
Call objLines.AddBy2Points(x1:=0.016, y1:=0.02, x2:=0.016, y2:=0.06)
Call objLines.AddBy2Points(x1:=0.016, y1:=0.06, x2:=0, y2:=0.06)
Call objLines.AddBy2Points(x1:=0, y1:=0.06, x2:=0, y2:=0)
' Define Relations among the Line objects to make the Profile closed
Set objRelns = objProfile(1).Relations2d
Call objRelns.AddKeypoint(Object1:=objLines(1), Index1:=igLineEnd, Object2:=objLines(2), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(2), Index1:=igLineEnd, Object2:=objLines(3), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(3), Index1:=igLineEnd, Object2:=objLines(4), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(4), Index1:=igLineEnd, Object2:=objLines(5), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(5), Index1:=igLineEnd, Object2:=objLines(6), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(6), Index1:=igLineEnd, Object2:=objLines(7), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(7), Index1:=igLineEnd, Object2:=objLines(8), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(8), Index1:=igLineEnd, Object2:=objLines(9), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(9), Index1:=igLineEnd, Object2:=objLines(10), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(10), Index1:=igLineEnd, Object2:=objLines(11), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(11), Index1:=igLineEnd, Object2:=objLines(12), Index2:=igLineStart)
Call objRelns.AddKeypoint(Object1:=objLines(12), Index1:=igLineEnd, Object2:=objLines(1), Index2:=igLineStart)
' Check for the Profile Validity
lngStatus = objProfile(1).End(ValidationCriteria:=igProfileClosed)
If lngStatus <> 0 Then
MsgBox ("Profile not closed")
End If
'Create the Base Extruded Protrusion Feature
Set objModel = objDoc.Models.AddFiniteExtrudedProtrusion(NumberOfProfiles:=1, _
profileArray:=objProfile, profileplaneSide:= _
igRight, ExtrusionDistance:=0.05)
objProfile(1).Visible = False
' Check the status of Base Feature
If objModel.ExtrudedProtrusions(1).Status <> igFeatureOK Then
MsgBox ("Error in the Creation of Base Protrusion Feature object")
End If
' Create a Circular Profile
Set objRefPln = objDoc.RefPlanes.AddParallelByDistance(ParentPlane:=objDoc.RefPlanes(2), _
Distance:=0.01, NormalSide:=igRight)
Set objProf = objDoc.ProfileSets.Add.Profiles.Add(pRefPlaneDisp:=objRefPln)
Call objProf.Circles2d.AddByCenterRadius(x:=-0.025, y:=0.035, Radius:=0.005)
' Check if the Profile is closed
lngStatus = objProf.End(ValidationCriteria:=igProfileClosed)
If lngStatus <> 0 Then
MsgBox ("Profile not closed")
End If
'Create the ExtrudedCutout feature
Set objExtCut = objModel.ExtrudedCutouts.AddFinite(Profile:=objProf, _
ProfileSide:=igLeft, profileplaneSide:= _
igRight, Depth:=0.1)
objProf.Visible = False
If objExtCut.Status <> igFeatureOK Then
MsgBox ("AddFinite Method of ExtrudedCutouts object failed")
End If
' Get the Features object
Set objFeatures = objModel.Features
' Assign the ExtrudedCutout object to another new object
Set objExtCut1 = objFeatures.Item(2)
' USER DISPLAY
' Release objects
Set objApp = Nothing
Set objDoc = Nothing
Set objProf = Nothing
Set objProfile(1) = Nothing
Set objProfile(2) = Nothing
Set objModel = Nothing
Set objExtCut = Nothing
Set objLines = Nothing
Set objRelns = Nothing
Set objRefPln = Nothing
Set objFeatures = Nothing
Set objExtCut1 = Nothing
End Sub