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