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I'm writing a macro in Microsoft Visual Basic for Applications for Autodesk Inventor Professional 2019. The intention for the macro is to automatically generate in-process inspection documents to accompany manufacturing process prints to the machine shop floor.
Is there a way to get the values and tolerances associated with a given ChamferNote? I believe that this question has been answered in the negative in this forum for versions of the software prior to 2010, with references to future improvements. I'm not seeing any more recent discussion of the issue. I'm not finding an answer to this question in the Inventor API Reference Manual.
Andrew
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Try below VBA code to determine values and tolerances of chamfer notes. Usually, tolerances will return in integer values which can mapped to respective LinearPrecisionEnum using below Inventor 2019 help documentation link.
http://help.autodesk.com/view/INVNTOR/2019/ENU/?guid=GUID-FBD80F0D-AF01-47AA-BC61-8DB782ACAE0D
Sub Main()
Dim oDoc As DrawingDocument
Set oDoc = ThisApplication.ActiveDocument
Dim oSheet As Sheet
Set oSheet = oDoc.ActiveSheet
Dim oChamferNote As ChamferNote
Set oChamferNote = oSheet.DrawingNotes.ChamferNotes.Item(1)
Debug.Print oChamferNote.Text
Dim oStyle As DimensionStyle
Set oStyle = oChamferNote.DimensionStyle
Dim oLinear As LinearPrecisionEnum
oLinear = oStyle.LinearPrecision
Debug.Print "Linear precision : " & oLinear
Dim oAngular As LinearPrecisionEnum
oAngular = oStyle.AngularPrecision
Debug.Print "Angular precision : " & oAngular
End Sub
Thanks and regards,
CHANDRA SHEKAR G
Developer Advocate
Autodesk Developer Network

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Thanks for the response. It appears that this provides the precision level of the default dimension.
I'm hoping to get the linear and angular tolerance ranges when the default dimensions are not used.
Andrew
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Custom tolerances of chamfer note are available through FormattedChamferNote API as XML tags as shown below.
<Distance1 Precision='3' AlternatePrecision='0' UpperTolerance='0.000000' LowerTolerance='0.000000' ToleranceType='kSymmetricTolerance' TolerancePrecision='2' ToleranceAlternatePrecision='2'></Distance1> X <Angle Precision='2' UpperTolerance='0.000000' LowerTolerance='0.000000' ToleranceType='kSymmetricTolerance' TolerancePrecision='2'></Angle> Chamfer
VBA code:
Sub Main()
Dim oDoc As DrawingDocument
Set oDoc = ThisApplication.ActiveDocument
Dim oSheet As Sheet
Set oSheet = oDoc.ActiveSheet
Dim oChamferNote As ChamferNote
Set oChamferNote = oSheet.DrawingNotes.ChamferNotes.Item(1)
Debug.Print oChamferNote.FormattedChamferNote
End Sub
Thanks and regards,
CHANDRA SHEKAR G
Developer Advocate
Autodesk Developer Network
