Insert a note for a threaded hole in a drawing in Inventor using C# / VBA

[vincenzobYFDD6]

Good morning, is there a way to insert a thread note in Inventor via API? See image.sd

[NachoShaw]

Yes its possible.

this code assumes you have the note selected

    Dim oDoc As DrawingDocument = ThisApplication.ActiveDocument

    If oDoc.SelectSet.Count <> 1 Then
        MsgBox ("A thread note must be selected.")
        Exit Sub
    End If

    If Not TypeOf oDoc.SelectSet(1) Is HoleThreadNote Then
        MsgBox ("A thread note must be selected.")
        Exit Sub
    End If

	Dim oThreadNote As HoleThreadNote = CType(oDoc.SelectSet(1), HoleThreadNote)
	oThreadNote.FormattedHoleThreadNote = "Thread Note Value Changed"

[NachoShaw]

and this one creates a thread note. Again, it assumes the thread is selected.

	Dim oApp As Inventor.Application = ThisApplication
    Dim oDoc As DrawingDocument = oApp.ActiveDocument

    If oDoc.SelectSet.Count <> 1 Then
        MsgBox ("A single thread edge must be selected.")
        Exit Sub
    End If

    If Not TypeOf oDoc.SelectSet(1) Is DrawingCurveSegment Then
        MsgBox ("A thread edge must be selected.")
        Exit Sub
    End If

    Dim oThreadEdge As DrawingCurve = oDoc.SelectSet(1).Parent

    If Not (oThreadEdge.EdgeType = kThreadEdge) Then
        MsgBox ("A thread edge must be selected.")
        Exit Sub
    End If

    Dim oPosition As Point2d = oApp.TransientGeometry.CreatePoint2d(22, 21)
    Dim oThreadNote As HoleThreadNote = oDoc.ActiveSheet.DrawingNotes.HoleThreadNotes.Add(oPosition, oThreadEdge)

[JelteDeJong]

Something you might want to have a look at. In the blog post "Automatically generate hole position dimensions" I show how you can add notes to all your holes, automatically to your drawing

[vincenzobYFDD6]

Sure, JelteDeJong, I had already found your solution. Very, very valid and helpful.