Autodesk Inventor

[#1]

Hi All

I am after a rule to change the unit type of all .ipts from cm to mm.

This has to go down to all levels in hierarchy  but only change .ipt files

any code would be appreciated

 Dave

[#2]

Hi dclunie,

I think this will work for you (if you modify it a bit):

'get input from user
oUnit = InputRadioBox("Select a units of measure type", "Metric", "Imperial", False, "ilogic")

If oUnit = True then 
'set to millimeter
oUOM_1 = UnitsTypeEnum.kMillimeterLengthUnits 
'set to kilogram
oUOM_2 = UnitsTypeEnum.kKilogramMassUnits
Else 
'set to inch
oUOM_1 = UnitsTypeEnum.kInchLengthUnits 
'set to pounds mass
oUOM_2 = UnitsTypeEnum.kLbMassMassUnits 		
End if

'Define the open document
Dim openDoc As Document
openDoc = ThisDoc.Document

'Look at all of the files referenced in the open document
Dim docFile As Document 
For Each docFile In openDoc.AllReferencedDocuments	
	'look at only part files
	 If docFile.DocumentType = kPartDocumentObject Then	
	'format  file name		
	Dim FNamePos As Long
	FNamePos = InStrRev(docFile.FullFileName, "\", -1)		         
	Dim docFName As String	
	docFName = Right(docFile.FullFileName, Len(docFile.FullFileName) - FNamePos)       
	'set length units 
	docFile.unitsofmeasure.LengthUnits = oUOM_1 
	'set mass units 
	docFile.unitsofmeasure.MassUnits = oUOM_2 
	'rebuild to update the display
	docFile.Rebuild
	End If
Next	
iLogicVb.UpdateWhenDone = True

This is a variation of this rule:

http://inventortrenches.blogspot.com/2012/05/ilogic-rule-to-change-units-of-measure.html

 I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[#3 · Accepted solution]

Here's a version specifically, directed toward changing from mm to cm:

'get input from user
oUnit = InputRadioBox("Select a units of measure type", "millimeter", "centimeter", True, "ilogic")

If oUnit = True then 
'set to millimeter
oUOM_1 = UnitsTypeEnum.kMillimeterLengthUnits 
Else 
'set to centimeter
oUOM_1 = UnitsTypeEnum.kCentimeterLengthUnits 
	
End if

'Define the open document
Dim openDoc As Document
openDoc = ThisDoc.Document

'Look at all of the files referenced in the open document
Dim docFile As Document 
For Each docFile In openDoc.AllReferencedDocuments	
	'look at only part files
	 If docFile.DocumentType = kPartDocumentObject Then	
	'format  file name		
	Dim FNamePos As Long
	FNamePos = InStrRev(docFile.FullFileName, "\", -1)		         
	Dim docFName As String	
	docFName = Right(docFile.FullFileName, Len(docFile.FullFileName) - FNamePos)       
	'set length units 
	docFile.unitsofmeasure.LengthUnits = oUOM_1 
	'rebuild to update the display
	docFile.Rebuild
	End If
Next	
iLogicVb.UpdateWhenDone = True

 I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

[#4]

Curtis,

Since the OP didn't say thank you I will. This just saved one of my staff a tonne of time. Thank you very much!

Cheers

Scott.