Extrudebuilder_ how let user to select the sketch that created programmatically

I recorded a journal while extruding a sketch (with the "feature curves" rule); I then edited the journal to use the first sketch it finds in the part navigator instead of the originally chosen sketch. Run the code on a part file that has at least 1 sketch in it.

Since your code creates a sketch before extruding it, replace "sketchFeature1" with a reference to your sketch.

Option Strict Off
Imports System
Imports NXOpen

Module Module136
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

' ----------------------------------------------
' Menu: Insert->Design Feature->Extrude...
' ----------------------------------------------
Dim markId1 As NXOpen.Session.UndoMarkId
markId1 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Visible, "Start")

Dim nullNXOpen_Features_Feature As NXOpen.Features.Feature = Nothing

If Not workPart.Preferences.Modeling.GetHistoryMode Then
Throw (New Exception("Create or edit of a Feature was recorded in History Mode but playback is in History-Free Mode."))
End If

Dim sketchFeature1 As NXOpen.Features.SketchFeature = Nothing
Dim sketch1 As NXOpen.Sketch = Nothing

For Each tempFeat As Features.Feature In theSession.Parts.Work.Features
If TypeOf (tempFeat) Is Features.SketchFeature Then
sketchFeature1 = tempFeat
sketch1 = sketchFeature1.Sketch
Exit For
End If
Next

If IsNothing(sketchFeature1) Then
'no sketch found
Return
End If

Dim extrudeBuilder1 As NXOpen.Features.ExtrudeBuilder
extrudeBuilder1 = workPart.Features.CreateExtrudeBuilder(nullNXOpen_Features_Feature)

Dim section1 As NXOpen.Section
section1 = workPart.Sections.CreateSection(0.00038, 0.0004, 0.5)

extrudeBuilder1.Section = section1

extrudeBuilder1.AllowSelfIntersectingSection(True)

extrudeBuilder1.DistanceTolerance = 0.0004

extrudeBuilder1.BooleanOperation.Type = NXOpen.GeometricUtilities.BooleanOperation.BooleanType.Create

Dim nullNXOpen_Body As NXOpen.Body = Nothing

extrudeBuilder1.BooleanOperation.SetTargetBodies({nullNXOpen_Body})

extrudeBuilder1.Limits.StartExtend.Value.RightHandSide = "0"

extrudeBuilder1.Limits.EndExtend.Value.RightHandSide = "10"

theSession.SetUndoMarkName(markId1, "Extrude Dialog")

section1.DistanceTolerance = 0.0004

section1.ChainingTolerance = 0.00038

section1.SetAllowedEntityTypes(NXOpen.Section.AllowTypes.OnlyCurves)

Dim markId2 As NXOpen.Session.UndoMarkId
markId2 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Invisible, "section mark")

Dim markId3 As NXOpen.Session.UndoMarkId
markId3 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Invisible, Nothing)

Dim curveFeatureRule1 As NXOpen.CurveFeatureRule
curveFeatureRule1 = workPart.ScRuleFactory.CreateRuleCurveFeature({sketchFeature1})

section1.AllowSelfIntersection(True)

Dim rules1(0) As NXOpen.SelectionIntentRule
rules1(0) = curveFeatureRule1

Dim nullNXOpen_NXObject As NXOpen.NXObject = Nothing

Dim helpPoint1 As NXOpen.Point3d = New NXOpen.Point3d(0.0, 0.0, 0.0)
section1.AddToSection(rules1, nullNXOpen_NXObject, nullNXOpen_NXObject, nullNXOpen_NXObject, helpPoint1, NXOpen.Section.Mode.Create, False)

theSession.DeleteUndoMark(markId3, Nothing)

Dim direction1 As NXOpen.Direction
direction1 = workPart.Directions.CreateDirection(sketch1, NXOpen.Sense.Forward, NXOpen.SmartObject.UpdateOption.WithinModeling)

extrudeBuilder1.Direction = direction1

theSession.DeleteUndoMark(markId2, Nothing)

Dim markId4 As NXOpen.Session.UndoMarkId
markId4 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Invisible, "Extrude")

theSession.DeleteUndoMark(markId4, Nothing)

Dim markId5 As NXOpen.Session.UndoMarkId
markId5 = theSession.SetUndoMark(NXOpen.Session.MarkVisibility.Invisible, "Extrude")

extrudeBuilder1.ParentFeatureInternal = False

Dim feature1 As NXOpen.Features.Feature
feature1 = extrudeBuilder1.CommitFeature()

theSession.DeleteUndoMark(markId5, Nothing)

theSession.SetUndoMarkName(markId1, "Extrude")

extrudeBuilder1.Destroy()

End Sub
End Module