Split a 3D Curve

[florian_wenzel]

Hi,

i try to Split a 3D Curve.

I took a similar Scrip for Split2D Curve, which works for 2D curves, but my Goal is to Split a 3D Curve.

I use the  SDKInventorAddIn in Visual Studio

Public Sub SampleCommandFunction()
Dim partDoc As PartDocument
partDoc = g_inventorApplication.ActiveDocument

Dim spline As Object
spline = g_inventorApplication.CommandManager.Pick(SelectionFilterEnum.kSketch3DCurveFilter, "Select 3d spline")

' Get the spline geometry from the entity.
Dim splineCurve As BSplineCurve
splineCurve = spline.Geometry

' Determine the parameter value for geometric midpoint of the curve.
Dim curveEval As CurveEvaluator
curveEval = splineCurve.Evaluator
Dim startParam As Double
Dim endParam As Double
Call curveEval.GetParamExtents(startParam, endParam)
Dim midParam As Double
Call curveEval.GetParamAtLength(startParam, spline.Length / 2, midParam)

' Split the curve.
Dim curve1 As BSplineCurve
Dim curve2 As BSplineCurve
Call splineCurve.Split(midParam, curve1, curve2)

' Create new sketch curves using the extracted splines.
Dim splineSketch As Sketch3D
splineSketch = spline.Parent
Call splineSketch.SketchFixedSplines.Add(curve1)
Call splineSketch.SketchFixedSplines.Add(curve2)

' Delete the original curve.
spline.Delete
End Sub

I can select a Curve, but without any Result.

Actually my Goal is to Split the Curve with equal Length and also choose the quantity, but first only in Middle

Any Suggestion.

Thanks

[nedeljko.sovljanski · Accepted solution]

If you run your code as addin then there should be try catch block around execute method. That means your you will not crash inventor but your addin will stop work. I put your code in macro and this lines throwing exceptions

Call splineSketch.SketchFixedSplines.Add(curve1)
Call splineSketch.SketchFixedSplines.Add(curve2)

[nedeljko.sovljanski]

As I can see in documentation

https://help.autodesk.com/view/INVNTOR/2022/ENU/?guid=GUID-C30FAF86-6494-4170-AFD7-0D98E686159D

there is no SketchFixedSplines property in Sketch3D object. There is SketchFixedSplines3D but that is only returns values.

https://help.autodesk.com/view/INVNTOR/2022/ENU/?guid=GUID-EE6B2929-6F1A-4E34-A742-D34618B74C67

[florian_wenzel]

Thanks, you right.

I try with SketchFixedSplines3D

[nedeljko.sovljanski · Accepted solution]

Only Include() method can add new Sketch3D but inout parameter is 

Input object to copy into the sketch. In a part context, valid input includes Edges, 3d sketch entities and planar sketch entities

You are trying to add BSplineCurve.

For this problem (how to convert) only @adam.nagy can help you.

[adam.nagy · Accepted solution]

Not sure what Inventor version you are using but in 2022 SketchFixedSplines3D.Add() seems to work fine:

Sub SplitSpline()
  Dim sp As SketchControlPointSpline3D
  Set sp = ThisApplication.ActiveDocument.SelectSet(1)
  
  Dim sk As Sketch3D
  Set sk = sp.Parent
  
  Dim bs As BSplineCurve
  Set bs = sp.Geometry
  
  Dim minp As Double
  Dim maxp As Double
  Call bs.Evaluator.GetParamExtents(minp, maxp)
  
  Dim midp As Double
  Call bs.Evaluator.GetParamAtLength(minp, sp.Length / 2, midp)
  
  Dim c1 As BSplineCurve
  Dim c2 As BSplineCurve
  Call bs.Split(midp, c1, c2)
  
  Call sk.SketchFixedSplines3D.Add(c1)
  Call sk.SketchFixedSplines3D.Add(c2)
  
  Call sp.Delete
End Sub

[florian_wenzel]

Ok, it works!

[florian_wenzel]

Looks good, 

the only small problem is , that all Curves are still there.

But this is not a big problem, you can choose the Curves what you need.

Then you can make a Works Surface at End of Curve.

Great!

[florian_wenzel]

Public Sub SampleCommandFunction()
Dim partDoc As PartDocument
partDoc = g_inventorApplication.ActiveDocument

Dim spline As Object
spline = g_inventorApplication.CommandManager.Pick(SelectionFilterEnum.kSketch3DCurveFilter, "Select 3d spline")

' Get the spline geometry from the entity.
Dim splineCurve As BSplineCurve
splineCurve = spline.Geometry

' Determine the parameter value for geometric midpoint of the curve.
Dim curveEval As CurveEvaluator
curveEval = splineCurve.Evaluator
Dim startParam As Double
Dim endParam As Double
Call curveEval.GetParamExtents(startParam, endParam)
Dim midParam As Double
Call curveEval.GetParamAtLength(startParam, spline.Length / 2, midParam)

' Split the curve.
Dim curve1 As BSplineCurve
Dim curve2 As BSplineCurve
Call splineCurve.Split(midParam, curve1, curve2)

' Create new sketch curves using the extracted splines.
Dim splineSketch As Sketch3D
splineSketch = spline.Parent
Call splineSketch.SketchFixedSplines3D.Add(curve1)
Call splineSketch.SketchFixedSplines3D.Add(curve2)

' Delete the original curve.
spline.Delete
End Sub

[florian_wenzel]

Hi,
im using Inventor 2022 and Visual Studio with SDK. Then i modify the VBA to VB.NET - it works 🙂
i didint refresh the Site before, so i even dont saw you Answers, sorry for this.
It was the moment which i was trying the Function.
Thanks very much!