Imports System.Runtime.InteropServices
Public Class Add

    Private Sub Button1_Click(sender As Object, e As EventArgs) Handles Button1.Click
        Dim objApplication As SolidEdgeFramework.Application = Nothing
        Dim objpartDoc As SolidEdgePart.PartDocument = Nothing
        Dim objRedefineFaces As SolidEdgePart.RedefineFaces
        Dim objRedefineFace As SolidEdgePart.RedefineFace
        Dim objModels As SolidEdgePart.Models
        Dim objModel As SolidEdgePart.Model
        Dim objBody As SolidEdgeGeometry.Body
        Dim objFaces As SolidEdgeGeometry.Faces
        Dim objFace As SolidEdgeGeometry.Face
        Dim objEdge As SolidEdgeGeometry.Edge
        Dim ii As Integer = 0
        Dim objType As Type = Nothing
        Dim objInputFaces(0) As Object
        Dim objInputEdges(0) As Object
        Dim objTypes(0) As SolidEdgeConstants.FeaturePropertyConstants
        Dim numBoundaryEdges As Integer
        Dim objBdryEdges(1) As Object
        Dim objBdryEdgeTypes(1) As SolidEdgeConstants.FeaturePropertyConstants
        Dim objRefPlanes As SolidEdgePart.RefPlanes
        Dim objRefPlane As SolidEdgePart.RefPlane
        Dim minParams(1) As Double
        Dim maxParams(1) As Double
        Dim isUCurve(0) As Boolean
        Dim inParams(0) As Double

        Try
            ' Create/get the application with specific settings
            objApplication = Marshal.GetActiveObject("SolidEdge.Application")

            If objApplication Is Nothing Then
                ' Get the type from the Solid Edge ProgID
                objType = Type.GetTypeFromProgID("SolidEdge.Application")
                ' Start Solid Edge
                objApplication = Activator.CreateInstance(objType)
                ' Make Solid Edge visible
                objApplication.Visible = True
            End If

            ' open the document mentioned in the doc files.
            objpartDoc = objApplication.Documents.Open("C:\TestFiles\RedefineFace\Cylinder.par")

            ' For solids
            objModels = objpartDoc.Models
            objModel = objModels.Item(1)
            objRedefineFaces = objModel.RedefineFaces
            objBody = objModel.Body

            objFaces = objBody.Faces(SolidEdgeGeometry.FeatureTopologyQueryTypeConstants.igQueryPlane)
            objFace = objFaces.Item(1)
            Dim FaceId As Integer = objFace.ID
            objInputFaces(0) = objFace
            objEdge = objFace.Edges(1)
            objInputEdges(0) = objEdge
            objTypes(0) = SolidEdgePart.FeaturePropertyConstants.igNatural

            '*************** Create the redefine feature first **********************
            objRedefineFace = objRedefineFaces.Add(1,
            objInputFaces,
            1,
            objInputEdges,
            objTypes,
            SolidEdgePart.SurfaceByBoundaryPatchTopology.igSurfaceByBoundarySingle, True)

            '******************Edit the feature option to full merge *********************
            objRedefineFace.FaceMergeOption = SolidEdgePart.SurfaceByBoundaryPatchTopology.igSurfaceByBoundarySingle

            '************ Edit the feature so that instead of replacing faces new surface is created. ***************
            objRedefineFace.ReplaceFacesOnSolidBody = False

            '********** Get and Set boundary edges tangency.************************
            'We must roll to previous feature before we get/set tangency types for edges. This is because the tangency is set on edges which are present before creating 'redefine feature.
            objModel.RollToFeature(objModel.Features.Item(1), True)

            objRedefineFace.GetEdgeTangencyTypes(numBoundaryEdges,
                                                 objBdryEdges,
                                                 objBdryEdgeTypes)

            For ii = 0 To numBoundaryEdges - 1
                objBdryEdgeTypes(ii) = SolidEdgePart.FeaturePropertyConstants.igTangent
            Next ii


            'Need not send back all the edges to SetEdgeTangencyTypes. You can only send the 
            'edges for which tangency is to be changed.
            objRedefineFace.SetEdgeTangencyTypes(numBoundaryEdges,
                                                 objBdryEdges,
                                                 objBdryEdgeTypes)

            'Roll to current feature to see the changes.
            objRedefineFace.RollToFeature()

            'Set boundary edges tangency back to normal so that insert sketch etc. functions can be demonstrated.
            objpartDoc.Undo(3)

            '**************************** Insert Sketch ************************************
            objRefPlanes = objpartDoc.RefPlanes
            objRefPlane = objRefPlanes.Item(1)

            objRedefineFace.InsertSketch(objRefPlane, True)

            '******************************* Insert UV Curve *******************************
            'We must roll to previous feature before we insert UV curve. This is because the 
            'UV curve is created on input faces to redefine feature.
            objModel.RollToFeature(objModel.Features.Item(1), True)
            objBody = objModel.Body
            objFace = objBody.GetFaceByFaceID(FaceId)
            objInputFaces(0) = objFace

            objFace.GetParamRange(minParams, maxParams)
            isUCurve(0) = False
            inParams(0) = (minParams(0) + maxParams(0)) / 2

            objRedefineFace.InsertUVCurve(1, objInputFaces, isUCurve, inParams, False)

            objRedefineFace.RollToFeature()

            objRedefineFace.ReplaceFacesOnSolidBody = True

        Catch ex As Exception
            MsgBox(ex.ToString)
        End Try

    End Sub
End Class