Imports System.Runtime.InteropServices
Public Class Form1

    Private Sub Button1_Click(sender As Object, e As EventArgs) Handles Button1.Click
        Dim application As SolidEdgeFramework.Application = Nothing
        Dim documents As SolidEdgeFramework.Documents = Nothing
        Dim partDocument As SolidEdgePart.PartDocument = Nothing
        Dim objModels As SolidEdgePart.Models = Nothing
        Dim objModel As SolidEdgePart.Mode = Nothing
        Dim objAddThkFeat As SolidEdgePart.Thicken = Nothing

        Try

            Console.WriteLine("Connecting to Solid Edge.")

            ' Connect to or start Solid Edge.
            application = ConnectToSolidEdge(True)

            ' Make sure user can see the GUI.
            application.Visible = True

            ' Bring Solid Edge to the foreground.
            application.Activate()

            ' Get a reference to the documents collection.
            documents = application.Documents

            Console.WriteLine("Creating a new part document.")

            ' Create a new part document.
            partDocument = CType(documents.Add("SolidEdge.PartDocument"), SolidEdgePart.PartDocument)

            ' Always a good idea to give SE a chance to breathe.
            application.DoIdle()

            Console.WriteLine("Drawing part.")

            ' Create geometry.
            CreateAddThickenFeat(partDocument)

            Console.WriteLine("Switching to ISO view.")

            ' Switch to ISO view.
            application.StartCommand(CType(SolidEdgeConstants.PartCommandConstants.PartViewISOView, SolidEdgeFramework.SolidEdgeCommandConstants))



        Catch ex As System.Exception
#If DEBUG Then
            System.Diagnostics.Debugger.Break()
#End If
            Console.WriteLine(ex.Message)
        Finally
            Console.WriteLine("Unregistering OleMessageFilter.")

        End Try
    End Sub

    Public Shared Sub CreateAddThickenFeat(ByVal partDocument As SolidEdgePart.PartDocument)
        Dim profileSets As SolidEdgePart.ProfileSets = Nothing
        Dim profileSet As SolidEdgePart.ProfileSet = Nothing
        Dim profiles As SolidEdgePart.Profiles = Nothing
        Dim profile As SolidEdgePart.Profile = Nothing
        Dim refplanes As SolidEdgePart.RefPlanes = Nothing
        Dim relations2d As SolidEdgeFrameworkSupport.Relations2d = Nothing
        Dim relation2d As SolidEdgeFrameworkSupport.Relation2d = Nothing
        Dim lines2d As SolidEdgeFrameworkSupport.Lines2d = Nothing
        Dim line2d As SolidEdgeFrameworkSupport.Line2d = Nothing
        Dim models As SolidEdgePart.Models = Nothing
        Dim model As SolidEdgePart.Model = Nothing
        Dim aProfiles As System.Array = Nothing
        Dim objFace(0 To 2) As SolidEdgeGeometry.Face
        Dim objExFeat As SolidEdgePart.ExtrudedProtrusion = Nothing
        Dim objThkFeat As SolidEdgePart.Thicken = Nothing

        ' Get a reference to the profile sets collection.
        profileSets = partDocument.ProfileSets

        ' Add a new profile set.
        profileSet = profileSets.Add()

        ' Get a reference to the profiles collection.
        profiles = profileSet.Profiles

        ' Get a reference to the ref planes collection.
        refplanes = partDocument.RefPlanes

        ' Add a new profile.
        profile = profiles.Add(refplanes.Item(3))

        ' Get a reference to the lines2d collection.
        lines2d = profile.Lines2d

        ' UOM = meters.
        Dim lineMatrix(,) As Double = {{0, 0, 0.08, 0}, {0.08, 0, 0.08, 0.06}, {0.08, 0.06, 0.064, 0.06}, {0.064, 0.06, 0.064, 0.02}, {0.064, 0.02, 0.048, 0.02}, {0.048, 0.02, 0.048, 0.06}, {0.048, 0.06, 0.032, 0.06}, {0.032, 0.06, 0.032, 0.02}, {0.032, 0.02, 0.016, 0.02}, {0.016, 0.02, 0.016, 0.06}, {0.016, 0.06, 0, 0.06}, {0, 0.06, 0, 0}}

        ' Draw the Base Profile.
        For i As Integer = 0 To lineMatrix.GetUpperBound(0)
            line2d = lines2d.AddBy2Points(x1:=lineMatrix(i, 0), y1:=lineMatrix(i, 1), x2:=lineMatrix(i, 2), y2:=lineMatrix(i, 3))
        Next i

        ' Define Relations among the Line objects to make the Profile closed.
        relations2d = CType(profile.Relations2d, SolidEdgeFrameworkSupport.Relations2d)

        ' Connect all of the lines.
        For i As Integer = 1 To lines2d.Count
            Dim j As Integer = i + 1

            ' When we reach the last line, wrap around and connect it to the first line.
            If j > lines2d.Count Then
                j = 1
            End If

            relation2d = relations2d.AddKeypoint(Object1:=lines2d.Item(i), Index1:=CInt(SolidEdgeConstants.KeypointIndexConstants.igLineEnd), Object2:=lines2d.Item(j), Index2:=CInt(SolidEdgeConstants.KeypointIndexConstants.igLineStart), guaranteed_ok:=True)
        Next i

        ' Close the profile.
        profile.End(SolidEdgePart.ProfileValidationType.igProfileClosed)

        ' Hide the profile.
        profile.Visible = False

        ' Create a new array of profile objects.
        aProfiles = Array.CreateInstance(GetType(SolidEdgePart.Profile), 1)
        aProfiles.SetValue(profile, 0)

        ' Get a reference to the models collection.
        models = partDocument.Models

        Console.WriteLine("Creating finite extruded protrusion.")

        ' Create the extended protrusion.
        model = models.AddFiniteExtrudedProtrusion(NumberOfProfiles:=aProfiles.Length, ProfileArray:=aProfiles, ProfilePlaneSide:=SolidEdgePart.FeaturePropertyConstants.igRight, ExtrusionDistance:=0.005)

        objExFeat = model.ExtrudedProtrusions(0)
        objFace(0) = objExFeat.TopCap

        model = models.AddThickenFeature(SolidEdgePart.FeaturePropertyConstants.igLeft, 0.1, 1, objFace)
    End Sub

    ''' <summary>
    ''' Connects to a running instance of Solid Edge.
    ''' </summary>
    Private Shared Function ConnectToSolidEdge() As SolidEdgeFramework.Application
        Return ConnectToSolidEdge(False)
    End Function

    ''' <summary>
    ''' Connects to a running instance of Solid Edge with an option to start if not running.
    ''' </summary>
    Private Shared Function ConnectToSolidEdge(ByVal startIfNotRunning As Boolean) As SolidEdgeFramework.Application
        Try
            ' Attempt to connect to a running instance of Solid Edge.
            Return CType(Marshal.GetActiveObject("SolidEdge.Application"), SolidEdgeFramework.Application)
        Catch ex As System.Runtime.InteropServices.COMException
            ' Failed to connect.
            If ex.ErrorCode = -2147221021 Then ' MK_E_UNAVAILABLE
                If startIfNotRunning Then
                    ' Start Solid Edge.
                    Return CType(Activator.CreateInstance(Type.GetTypeFromProgID("SolidEdge.Application")), SolidEdgeFramework.Application)
                Else
                    Throw New System.Exception("Solid Edge is not running.")
                End If
            Else
                Throw
            End If
        Catch
            Throw
        End Try
    End Function
End Class