Generate Tractrix geometry in NX

[AndersSande]

Hi,
I've been asked if NX can generate a geometry that's is a ''tractrix''. Ref this wikipedia page:

https://en.wikipedia.org/wiki/Tractrix

The geometry is a variant of ''surface blend'' controlled by an expression. This one: x=t-\tanh(t),y=1/{\cosh(t) x=t-\tanh(t),y=1/{\cosh(t). ( from the Wikipedia page)
I'm running NX 12, but solution for newer versions is also possible.

Any suggestions?

Anders

 

[Toost]

I think that shape is/should be possible, at least as a curve.
the wikipedia page notes that a surface of revolution of this shape can be used as a loudspeaker.
Most surfaces are built from curves, The surface shape is a derivative of the curve shape-s.
are you looking to define a surface directly with this shape and skip the "curve stage" ?

Regards,
Tomas

Never try to teach a pig to sing. I wastes your time and it annoys the pig.

 

[AndersSande]

If I could have NX to make a expression controlled 'Face blend' from the given expression, I would be happy.
No need for the curve, a 'Face blend' will do the trick.

Regards,
Anders

 

[MANox]

Hello,

I was used NX Journal for create spline sililar to tractrix.
Mayby it's usefull for You:
(You must change Rk and Rm)

Imports System
Imports NXOpen

Module Horn_trackix

    Sub Main(ByVal args() As String)



        Dim theSession As NXOpen.Session = NXOpen.Session.GetSession()
        Dim workPart As NXOpen.Part = theSession.Parts.Work
        Dim displayPart As NXOpen.Part = theSession.Parts.Display
        Dim lw As ListingWindow = theSession.ListingWindow
        lw.Open()
        Dim markId1 As NXOpen.Session.UndoMarkId = Nothing
        markId1 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Visible, "Start")

        Dim nullNXOpen_NXObject As NXOpen.NXObject = Nothing
        Dim studioSplineBuilderEx1 As NXOpen.Features.StudioSplineBuilderEx = Nothing
        studioSplineBuilderEx1 = workPart.Features.CreateStudioSplineBuilderEx(nullNXOpen_NXObject)

        Dim origin1 As NXOpen.Point3d = New NXOpen.Point3d(0.0, 0.0, 0.0)
        Dim normal1 As NXOpen.Vector3d = New NXOpen.Vector3d(0.0, 0.0, 1.0)
        Dim plane1 As NXOpen.Plane = Nothing
        plane1 = workPart.Planes.CreatePlane(origin1, normal1, NXOpen.SmartObject.UpdateOption.WithinModeling)

        studioSplineBuilderEx1.DrawingPlane = plane1
        studioSplineBuilderEx1.OrientExpress.ReferenceOption = NXOpen.GeometricUtilities.OrientXpressBuilder.Reference.WcsDisplayPart
        studioSplineBuilderEx1.MovementMethod = NXOpen.Features.StudioSplineBuilderEx.MovementMethodType.View
        studioSplineBuilderEx1.OrientExpress.AxisOption = NXOpen.GeometricUtilities.OrientXpressBuilder.Axis.Passive
        studioSplineBuilderEx1.OrientExpress.PlaneOption = NXOpen.GeometricUtilities.OrientXpressBuilder.Plane.Passive
        studioSplineBuilderEx1.Extender.StartValue.RightHandSide = "0"
        studioSplineBuilderEx1.Extender.EndValue.RightHandSide = "0"
        studioSplineBuilderEx1.InputCurveOption = NXOpen.Features.StudioSplineBuilderEx.InputCurveOptions.Hide
        studioSplineBuilderEx1.MatchKnotsType = NXOpen.Features.StudioSplineBuilderEx.MatchKnotsTypes.None

        Dim Rm As Integer = 460 ' Mouth radius (mm*10) 'edit 2020.04.23
        Dim Rk As Integer = 75 ' Throat radius (mm*10) 'edit 2020.04.23

        For R As Integer = Rm To Rk Step -1

            Dim Rs As Double = Rm / 10
            Dim Rr As Double = R / 10
            Dim x As Double
            x = Rs * Math.Log((Rs + (Rs ^ 2 - Rr ^ 2) ^ 0.5) / Rr) - (Rs ^ 2 - Rr ^ 2) ^ 0.5

            'lw.WriteLine(x & ",   " & Rr)

            Dim coordinates1 As NXOpen.Point3d = New NXOpen.Point3d(0, Rr, x)
            Dim point1 As NXOpen.Point = Nothing
            point1 = workPart.Points.CreatePoint(coordinates1)
            Dim geometricConstraintData1 As NXOpen.Features.GeometricConstraintData = Nothing
            geometricConstraintData1 = studioSplineBuilderEx1.ConstraintManager.CreateGeometricConstraintData()
            geometricConstraintData1.Point = point1
            studioSplineBuilderEx1.ConstraintManager.Append(geometricConstraintData1)

        Next

        Dim nXObject1 As NXOpen.NXObject = Nothing
        nXObject1 = studioSplineBuilderEx1.Commit()
        studioSplineBuilderEx1.Destroy()


        theSession.DeleteUndoMark(markId1, Nothing)
    End Sub
End Module

Best Regards

MANok
NX12
TC10