Extract Centerline of free form tube

Scene: a non-descript grey fabric covered box that currently contains a workstation running NX and 2 coworkers

Coworker: Hey, I need to measure the length of this tube I have...

NXJournaling: No problem, here's a journal that lets you select a tube and adds up the lengths of the defining sections

Coworker: actually, it is from an imported part; there are no defining objects in the file...

NXJournaling: Ok, assuming it is made of straights and bends, we can extract lines from the cylindrical faces then...

Coworker: Well, it doesn't have straight sections or simple bends so much... it seems to be made of B-surfaces

NXJournaling: oh, I see... well... hmmm

NXJournaling: Let me introduce you to Frank Swinkels. He is a regular contributor at the GTAC languages forum and also at the eng-tips Siemens NX forum and he likes to write and share the type of code that can get you out of situations like this.

He has given us permission to reproduce some code he originally posted in the GTAC forum in answer to the request for extracting the centerline of an unparameterized free form tube. The code works the following way:

1. The user is prompted to select a B-surface face.
2. Collect the B-surface data, make sure the surface is closed in the U direction. Use the V direction surface data to help generate the tube centerline.
3. At each point of interest along the length of the tube, generate equally spaced points around the circumference (U direction) of the tube. The average of these points determines the center point of the tube cross section.
4. Construct a studio spline through these points which will closely approximate the centerline of the tube.




Notes

This journal will only work with NX 8 or above.

I encourage you to step through the code to see what is going on, I can almost guarantee that you will learn something.

The code demonstrates the use of the AskFaceProps function and a couple of vector functions that may come in handy. Also, there is a subroutine for creating a through points studio spline. Pass in an array of points and the desired degree and the spline will be created. That's a good piece of reusable code to have on hand...


The Code

Download the code and a sample part.

'Author: Frank Swinkels
'for use only with NX 8.5 or above
'Create approximate centerline of B-surface "tube"
'user will be prompted to select B-surface, a 'through points' studio spline will be created along the centerline
 
'  modified June 19, 2014 to include creating the bsurface and allow for faces with other then 0 to 1 parameters 
' (typically cylinders or extended cylinders)
'
' modified June 24 to change for selecting apply or OK
' 
'  NXJournaling.com
'    Report length of selected tube.
 
Option Strict Off
Imports System
Imports NXOpen
Imports NXOpen.UF
Imports NXOpenUI
Imports NXOpen.Features
Imports System.IO
 
Module CableCentreline
 
    Dim s As Session = Session.GetSession()
    Dim ufs As UFSession = UFSession.GetUFSession()
    Dim workPart As Part = s.Parts.Work
    Dim lw As ListingWindow = s.ListingWindow
    Sub Main()
        Dim no_pts As Integer = Nothing
        Dim pos1 As Integer = Nothing
        Dim junk3(2) As Double
        Dim junk2(1) As Double
        Dim periodic1 As Boolean = False
        Dim theFace As Face = Nothing
        Dim totalLength As Double = 0
        Dim response1 As Selection.Response = Selection.Response.Cancel
        Dim type1 As Integer = Nothing
        Dim subtype1 As Integer = Nothing
        Dim bsurface1 As UFModl.Bsurface = Nothing
        Dim extractedfeat1 As Feature = Nothing
        Dim extractedbodyfeat1 As BodyFeature = Nothing
        Dim extractedbody1() As Body = Nothing
        Dim faces() As Face
        Dim testface As Face
        lw.Open()
        While select_a_face("Select a tube extracted face or dumb solid face", theFace) = Selection.Response.Ok
 
 
            'response1 = select_a_face("Select a tube extracted face or dumb solid face", theFace)
            'If response1 = Selection.Response.Cancel Or response1 = Selection.Response.Back Then GoTo end1
            ' check that it is a bsurface
            Try
                ufs.Modl.AskBsurf(theFace.Tag, bsurface1)
                testface = theFace
            Catch ex As Exception
                createExtractedBSurface(theFace, extractedfeat1)
                extractedbodyfeat1 = DirectCast(extractedfeat1, BodyFeature)
                extractedbody1 = extractedbodyfeat1.GetBodies
                faces = extractedbody1(0).GetFaces
                ufs.Modl.AskBsurf(faces(0).Tag, bsurface1)
                testface = faces(0)
            End Try
 
            Dim noPolesV As Integer = bsurface1.num_poles_v
            Dim noPolesU As Integer = bsurface1.num_poles_u
            Dim poles1(,) As Double = bsurface1.poles
            Dim knotsU() As Double = bsurface1.knots_u
            Dim knotsV() As Double = bsurface1.knots_v
            Dim orderU As Integer = bsurface1.order_u
            Dim orderV As Integer = bsurface1.order_v
            Dim ptno As Integer = Nothing
            Dim params(1) As Double
            Dim pnt0(2) As Double
            Dim pnt1(2) As Double
            Dim pnt2(2) As Double
            Dim pnt3(2) As Double
            Dim vec0(2) As Double
            Dim vec1(2) As Double
            Dim vec2(2) As Double
            Dim vec3(2) As Double
            Dim rads(1) As Double
            Dim tolerance1 As Double = 0.001
            Dim magnitude1 As Double = Nothing
            Dim degree3 As Integer = orderV - 1
            Dim pointtag As Tag = Tag.Null
            Dim ArrayOfPoints(-1) As Point
            Dim uparm() As Double = {0.0, 0.25, 0.5, 0.75}
            Dim delta1 As Double
            Dim sum1 As Double = Nothing
            Dim distance1 As Double = Nothing
            Dim cnt1 As Integer = 0
            Dim tempcpt(2) As Double
            Dim coordinates1 As Point3d
            Dim temptag As Tag = Tag.Null
            ' tube bsurf u around tube, v along the tube
            Dim vparm(noPolesV - 1) As Double
            vparm(0) = 0.0
            vparm(noPolesV - 1) = 1.0
            Dim lengths(noPolesV - 2) As Double
            sum1 = 0.0
            cnt1 = 0
            For i As Integer = noPolesU To noPolesU * noPolesV - 1 Step noPolesU
                pnt1(0) = poles1(i, 0)
                pnt1(1) = poles1(i, 1)
                pnt1(2) = poles1(i, 2)
                pnt2(0) = poles1(i - noPolesU, 0)
                pnt2(1) = poles1(i - noPolesU, 1)
                pnt2(2) = poles1(i - noPolesU, 2)
                ufs.Vec3.Distance(pnt1, pnt2, distance1)
                lengths(cnt1) = distance1
                cnt1 += 1
                sum1 += distance1
            Next
            delta1 = 0.0
            For i As Integer = 0 To noPolesV - 2
                delta1 += lengths(i)
                vparm(i + 1) = delta1 / sum1
            Next
            Dim uvminmax(3) As Double
            ufs.Modl.AskFaceUvMinmax(testface.Tag, uvminmax)
            Dim total2 As Double = uvminmax(3) - uvminmax(2)
            Dim delta2 As Double = total2 / (noPolesV - 1)
            Dim zero1 As Double = uvminmax(2)
            For i As Integer = 0 To noPolesV - 1
                If i = 0 Then
                    vparm(i) = zero1
                Else
                    vparm(i) = vparm(i - 1) + delta2
                End If
 
            Next
            For i As Integer = 0 To noPolesV - 1
                params(0) = uparm(0)
                params(1) = vparm(i)
                ufs.Modl.AskFaceProps(testface.Tag, params, pnt0, junk3, vec0, junk3, junk3, junk3, rads)
                ufs.Vec3.Unitize(vec0, tolerance1, magnitude1, vec0)
                params(0) = uparm(1)
                ufs.Modl.AskFaceProps(testface.Tag, params, pnt1, junk3, vec1, junk3, junk3, junk3, rads)
                params(0) = uparm(2)
                ufs.Modl.AskFaceProps(testface.Tag, params, pnt2, junk3, vec2, junk3, junk3, junk3, rads)
                params(0) = uparm(3)
                ufs.Modl.AskFaceProps(testface.Tag, params, pnt3, junk3, vec3, junk3, junk3, junk3, rads)
                ufs.Vec3.Add(pnt0, pnt1, tempcpt)
                ufs.Vec3.Add(pnt2, tempcpt, tempcpt)
                ufs.Vec3.Add(pnt3, tempcpt, tempcpt)
                tempcpt(0) /= 4.0
                tempcpt(1) /= 4.0
                tempcpt(2) /= 4.0
                coordinates1 = New Point3d(tempcpt(0), tempcpt(1), tempcpt(2))
 
                ReDim Preserve ArrayOfPoints(i)
                ArrayOfPoints(i) = workPart.Points.CreatePoint(coordinates1)
            Next
 
            periodic1 = False
            Dim myStudioSpline As Features.StudioSpline
            myStudioSpline = CreateStudioSplineThruPoints(ArrayOfPoints, degree3)
            Dim tubeLength As Double = 0
            For Each tempCurve As Curve In myStudioSpline.GetEntities
                tubeLength += tempCurve.GetLength
            Next
            totalLength += tubeLength
            lw.WriteLine("section length: " & tubeLength.ToString)
            lw.WriteLine("total length: " & totalLength.ToString)
            lw.WriteLine("")
        End While
end1:
    End Sub
    Public Sub createExtractedBSurface(ByVal face1 As Face, ByRef extractedfeat1 As Feature)
        Dim nullFeatures_Feature As Features.Feature = Nothing
        Dim extractFaceBuilder1 As Features.ExtractFaceBuilder
        extractFaceBuilder1 = workPart.Features.CreateExtractFaceBuilder(nullFeatures_Feature)
        extractFaceBuilder1.ParentPart = Features.ExtractFaceBuilder.ParentPartType.WorkPart
        extractFaceBuilder1.Associative = True
        extractFaceBuilder1.FixAtCurrentTimestamp = True
        extractFaceBuilder1.HideOriginal = False
        extractFaceBuilder1.Type = Features.ExtractFaceBuilder.ExtractType.Face
        extractFaceBuilder1.InheritDisplayProperties = False
        extractFaceBuilder1.SurfaceType = Features.ExtractFaceBuilder.FaceSurfaceType.PolynomialCubic
        Dim added1 As Boolean
        added1 = extractFaceBuilder1.ObjectToExtract.Add(face1)
        extractedfeat1 = extractFaceBuilder1.Commit
    End Sub
    Function select_a_face(ByRef prompt As String, ByRef face1 As Face) As Selection.Response
        Dim mask(0) As Selection.MaskTriple
        With mask(0)
            .Type = UFConstants.UF_solid_type
            .Subtype = 0
            .SolidBodySubtype = UFConstants.UF_UI_SEL_FEATURE_ANY_FACE
        End With
        Dim cursor As Point3d = Nothing
        Dim response1 As Selection.Response = Selection.Response.Cancel
        select_a_face = Nothing
        response1 = UI.GetUI.SelectionManager.SelectTaggedObject(prompt, "Select the Face", _
            Selection.SelectionScope.AnyInAssembly, _
            Selection.SelectionAction.ClearAndEnableSpecific, False, _
            False, mask, face1, cursor)
        If response1 = Selection.Response.ObjectSelected Or _
            response1 = Selection.Response.ObjectSelectedByName Then
            Return Selection.Response.Ok
        ElseIf response1 = Selection.Response.Back Then
            Return Selection.Response.Back
        Else
            Return Selection.Response.Cancel
        End If
    End Function
 
    Public Function CreateStudioSplineThruPoints(ByRef points() As Point, ByVal degree3 As Integer) As Features.StudioSpline
        Dim markId9 As Session.UndoMarkId
        markId9 = s.SetUndoMark(Session.MarkVisibility.Visible, "Studio Spline Thru Points")
        Dim Pcount As Integer = points.Length - 1
        Dim nullFeatures_StudioSpline As Features.StudioSpline = Nothing
        Dim studioSplineBuilderex1 As Features.StudioSplineBuilderEx
        studioSplineBuilderex1 = workPart.Features.CreateStudioSplineBuilderEx(nullFeatures_StudioSpline)
        studioSplineBuilderex1.OrientExpress.ReferenceOption = GeometricUtilities.OrientXpressBuilder.Reference.ProgramDefined
        studioSplineBuilderex1.Degree = degree3
        studioSplineBuilderex1.OrientExpress.AxisOption = GeometricUtilities.OrientXpressBuilder.Axis.Passive
        studioSplineBuilderex1.OrientExpress.PlaneOption = GeometricUtilities.OrientXpressBuilder.Plane.Passive
        studioSplineBuilderex1.MatchKnotsType = Features.StudioSplineBuilderEx.MatchKnotsTypes.None
        Dim knots1(-1) As Double
        studioSplineBuilderex1.SetKnots(knots1)
        Dim parameters1(-1) As Double
        studioSplineBuilderex1.SetParameters(parameters1)
        Dim nullDirection As Direction = Nothing
        Dim nullScalar As Scalar = Nothing
        Dim nullOffset As Offset = Nothing
        Dim geometricConstraintData(Pcount) As Features.GeometricConstraintData
        For ii As Integer = 0 To Pcount
            geometricConstraintData(ii) = studioSplineBuilderex1.ConstraintManager.CreateGeometricConstraintData()
            geometricConstraintData(ii).Point = points(ii)
            geometricConstraintData(ii).AutomaticConstraintDirection = Features.GeometricConstraintData.ParameterDirection.Iso
            geometricConstraintData(ii).AutomaticConstraintType = Features.GeometricConstraintData.AutoConstraintType.Tangent
            geometricConstraintData(ii).TangentDirection = nullDirection
            geometricConstraintData(ii).TangentMagnitude = nullScalar
            geometricConstraintData(ii).Curvature = nullOffset
            geometricConstraintData(ii).CurvatureDerivative = nullOffset
            geometricConstraintData(ii).HasSymmetricModelingConstraint = False
        Next ii
        studioSplineBuilderex1.ConstraintManager.SetContents(geometricConstraintData)
        Dim feature1 As Features.StudioSpline
        feature1 = studioSplineBuilderex1.CommitFeature()
        studioSplineBuilderex1.Destroy()
 
        Return feature1
 
    End Function
 
    Public Function GetUnloadOption(ByVal dummy As String) As Integer
        'Unloads the image when the NX session terminates
        GetUnloadOption = NXOpen.Session.LibraryUnloadOption.Immediately
    End Function
 
End Module