"Hole and Thread" dimensions as "Inspection Dimension". How do you do it?

[design]

Hello,

I'm adding in inspection dimensions for a PPAP submission drawing and have found that I cannot set hole and thread dimensions as inspection dimensions. I'm quite surprised to find that this option isn't available. Is it there, just hidden, or is it really not available to me?

To the top right of this picture is the inspection dimension I want and to the left the thread dimension which I can't get into this format.

Any help much appreciated.

Bob.

[Daniela_Koloszko]

This is a current limitation of inspection dimensions. Inspection dimension option is supported on regular dimensions only, no notes.

[design]

Thank you Daniella,

Do you know if this is going to be added in future releases? I'm getting increased requirements for inspection dimensions to be on drawings for automotive and military customers due to PPAP quality requirements. I'm sure I'm not alone in that!

Regards,

Bob.

[SBix26]

Put it on the Inventor IdeaStation forum, then come back here and link to it, to garner additional support.  Sounds like a very reasonable request.

Sam B
Inventor 2012 Certified Professional

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[Daniela_Koloszko]

Currently I am not aware of plans to support this feature for notes, however you can register an enhancement request on Inventor IdeaStation as suggested already. This site is monitored by our development team and your request will be taken into account. 

[tim.burnsRZN3A]

I was looking for a solution to the same issue.  Here is a little vba code that should do the trick:

Public Sub MakeInspection()
' Set HoleThreadNotes to Inspection
Dim oDoc As Document
Dim oHoleThreadNote As HoleThreadNote
Dim n As Integer
n = 1

' Set reference to active doc
Set oDoc = ThisApplication.ActiveDocument

' Set each Hole Note to be inspection
For Each oHoleThreadNote In oDoc.SelectSet
oHoleThreadNote.IsInspectionDimension = True
Call oHoleThreadNote.SetInspectionDimensionData(kRoundedEndsInspectionBorder, n, "5/BATCH")
n = n + 1
Next

End Sub

Select one or more hole notes, then run the macro.

[edwin.smith5K6MK]

Can this also be applied to Leader notes and Chamfer notes? 

e.g.

Public Sub MakeInspection()
' Set LeaderNotes to Inspection
Dim oDoc As Document
Dim oLeaderNote As LeaderNote
Dim n As Integer
n = 1

' Set reference to active doc
Set oDoc = ThisApplication.ActiveDocument

' Set each Leader Note to be inspection
For Each oLeaderNote In oDoc.SelectSet
oLeaderNote.IsInspectionDimension = True
Call oLeaderNote.SetInspectionDimensionData(kRoundedEndsInspectionBorder, n, "5/BATCH")
n = n + 1
Next

End Sub

I've got no coding knowledge so when I tried this it came up with a type mismatch error.

[tim.burnsRZN3A]

Unfortunately no it does not work with Leader notes or Chamfer notes.  We created a sketch symbol that we insert next to Leader notes, Chamfer notes, and Text notes to mark them as inspection.

[SER4]

Looks like someone forgot to link the Idea to vote for, so here it is:

https://forums.autodesk.com/t5/inventor-ideas/inspection-dimensions-option-for-hole-and-thread-annot...

[SER4]

@tim.burnsRZN3A this is pretty awesome and almost gets me there!

(BTW, we use the "Angular" inspection border, so the last Call line for me is:

Call oHoleThreadNote.SetInspectionDimensionData(kAngularEndsInspectionBorder, n)

 However, I have a pre-set tolerance on the hole diameter...why does it change the units of only the tolerance from inches to cm?

Before.

After.

*Ninja-edit: I think the solution was to change the STYLE of the dimension (after running macro), then change it back, and finally re-fix the precision & tolerances:

Annoying, but it works.

The next question is how to manually change the Inspection Numbers.