Inspection dimensions - not what I am looking for....

[Anonymous]

Hi all

when QC asks for a markup drawing (dimensions are marked with a number or letter) to be used as references on the measuring reports I struggle to find a good solution.

1) I can make a dimension to an "Inspection dimension" - and add a number/letter. However, I cannot do this with a "Feature" - e.g. run-out. Also I cannot supress the inspection dimension (I do not want this to be part of the drawing that we send to subsuppliers). So this does not really full fill me needs.

2) I can make a "skecth symbol" (I choose a circle with a number inside) and place the sketch symbol net to all the dimensions and features that needs to be checked by QC. The problem is that I cannot "hide" or "suppress" my sketch symbol. So to do this I need to make a seperate IDW with the markup. And then if I update my drawing with a new dimension or a dimension changes I need to make another new draiwng and add the "sketch symbols".

It there an easier way to do this. What I would have liked was that I could have a "stamp" (e.g. a circle with a number inside) with a counter build-in. So every time I use the stamp the number increases by 1. This stamp I could then use on the drawing, print the drawing with the markups, "hide"/"Suppress" the "stamp" and then save the drawing as the one my supplier receives. Then If I need to make a drawing changes I just open the drawing, make the change, "unhide" the stamps (e.g. add a new stamp if a new dimension has been added), print for QC, "hide" the stamp and save the drawing again.

Ideally the stamps where connected to the dimensions and features and through this you could create a spreasheet of dimensions to be checked with tolerances and everything.

Bo

[Xun.Zhang]

Hi Bo,

How about leverage layer visibility with Text stamp? Put all related Inspection dimensions tags into this layer and you can turn on/off the visibility to switch. Example was listed below.

[kelly.young]

Hello @Anonymous there was a very similar post a while back that should help you out.

numerate my dimension

Please select the Accept as Solution button if a post solves your issue or answers your question.

[mcgyvr]

@Anonymous

Bo..

Try this ilogic rule..

Select Yes to add numbering to dimensions (and turn them into Inspection dimension boxes)  and to add a numerical note to feature control frames

Select No to remove that all..

Dim oDrawingDoc As DrawingDocument
    If ThisApplication.activeDocument.DocumentType <> kDrawingDocumentObject Then
        Return
        Else
        oDrawingDoc = ThisApplication.activeDocument
    End If

Dim oSheet As Sheet
oSheet = oDrawingDoc.ActiveSheet
Dim oDims As DrawingDimensions
oDims = oSheet.DrawingDimensions
Dim oDim As DrawingDimension
Dim i As Long
Dim oThreadNotes As HoleThreadNotes
oThreadNotes = oSheet.DrawingNotes.HoleThreadNotes
Dim oThreadNote As HoleThreadNote
Dim oFeatContFrames As FeatureControlFrames
oFeatContFrames = oSHeet.FeatureControlFrames
Dim oFreatContFram As FeatureControlFrame

'ask question if we want to turn on inspection dimension numbering/style. No will remove them..
question = MessageBox.Show("Do you want to show inspection dimension numbering?", "iLogic Question",MessageBoxButtons.YesNo,MessageBoxIcon.Question)
'[if yes then 
If question = vbYes Then
	'start numbering at 1
	i = 1
	'loop through each dimension and set it to an inspection dimension and add the numbers
	For Each oDim In oDims
		oDim.IsInspectionDimension = True
		oDim.SetInspectionDimensionData _
		(InspectionDimensionShapeEnum.kRoundedEndsInspectionBorder, i)
		i = i + 1
	Next
	'loop through each thread note and set it to an inspection dimension and add the numbers
	For Each oThreadNote In oThreadNotes
		oThreadNote.IsInspectionDimension = True
		oThreadNote.SetInspectionDimensionData _
		(InspectionDimensionShapeEnum.kRoundedEndsInspectionBorder, i)
		i = i + 1
	Next
	'loop through each feature control frame and set its note to the inspection number
	For Each oFeatContFrame In oFeatContFrames
		'adds a note to the control frame
		oFeatContFrame.notes = i	
		i = i + 1
	Next
'remove all inspection numbering/formatting
Else

	For Each oDim In oDims
		oDim.IsInspectionDimension = False
	Next

	For Each oThreadNote In oThreadNotes
		oThreadNote.IsInspectionDimension = False
	Next
	
	For Each oFeatContFrame In oFeatContFrames
		oFeatContFrame.notes = ""	
	Next

End If

If no you get this..

If yes you get this..

[mcgyvr · Accepted solution]

Or I like this better..

It just uses the feature control frame data identifier for the number spot instead of the notes

Dim oDrawingDoc As DrawingDocument
    If ThisApplication.activeDocument.DocumentType <> kDrawingDocumentObject Then
        Return
        Else
        oDrawingDoc = ThisApplication.activeDocument
    End If

Dim oSheet As Sheet
oSheet = oDrawingDoc.ActiveSheet
Dim oDims As DrawingDimensions
oDims = oSheet.DrawingDimensions
Dim oDim As DrawingDimension
Dim i As Long
Dim oThreadNotes As HoleThreadNotes
oThreadNotes = oSheet.DrawingNotes.HoleThreadNotes
Dim oThreadNote As HoleThreadNote
Dim oFeatContFrames As FeatureControlFrames
oFeatContFrames = oSHeet.FeatureControlFrames
Dim oFreatContFram As FeatureControlFrame

'ask question if we want to turn on inspection dimension numbering/style. No will remove them..
question = MessageBox.Show("Do you want to show inspection dimension numbering?", "iLogic Question",MessageBoxButtons.YesNo,MessageBoxIcon.Question)
'[if yes then 
If question = vbYes Then
	'start numbering at 1
	i = 1
	'loop through each dimension and set it to an inspection dimension and add the numbers
	For Each oDim In oDims
		oDim.IsInspectionDimension = True
		oDim.SetInspectionDimensionData _
		(InspectionDimensionShapeEnum.kRoundedEndsInspectionBorder, i)
		i = i + 1
	Next
	'loop through each thread note and set it to an inspection dimension and add the numbers
	For Each oThreadNote In oThreadNotes
		oThreadNote.IsInspectionDimension = True
		oThreadNote.SetInspectionDimensionData _
		(InspectionDimensionShapeEnum.kRoundedEndsInspectionBorder, i)
		i = i + 1
	Next
	'loop through each feature control frame and set its note to the inspection number
	For Each oFeatContFrame In oFeatContFrames
		'adds a note to the control frame
		oFeatContFrame.DatumIdentifier = i	
		i = i + 1
	Next
'remove all inspection numbering/formatting
Else

	For Each oDim In oDims
		oDim.IsInspectionDimension = False
	Next

	For Each oThreadNote In oThreadNotes
		oThreadNote.IsInspectionDimension = False
	Next
	
	For Each oFeatContFrame In oFeatContFrames
		oFeatContFrame.DatumIdentifier = ""	
	Next

End If

[johndtomlinson]

Thanks for that it works great! Cool time-saver!

Not to be greedy, but is there a way to export this so QC can have get an inspection report spreadsheet?

Ideally it would have:

Bubble number/Dimension with Tolerance/Zone.

Would save a even more work!

[johndtomlinson]

My CE says the zone export is not needed. But..

Just found a problem. All "basic" dimensions are converted to "inspection" dimensions which changes the intent of the annotation. They could be filtered out I suppose, but still need to be "bubbled" somehow.

I'm thinking of adding or appending a line of text of {xx} in the text box. Might need another solution for FCF's and surface finishes.

Also would want to be able to add or delete dimensions to a drawing then run it again without changing the existing "bubble" numbers.

??

[Anonymous]

A particular measurement should be investigated on each part that is created. This "100% assessment" could be signified by utilizing "100%" within a hover by the measurement with a drawing note expressing "100% investigation required." 2. For a particular measurement a Control Plan or extraordinary Inspection Procedure is required.

[baran.blaser]

Hi this code works for me and helped me out a lot! Is there any way to get it to put numbered bubbles around notes as well? Maybe if there is a way to get a note to be a dimension somehow. I'm just not sure how to do it. I'm talking about like thread notes, knurling notes, stuff like that, with a leader attached to it pointing to the position. If you know of anything, let me know! Thanks!