Show Imperial & Metric Frame Sizes on BoM

@ClintBrown3D Autodesk Inventor 54

I saw a thread on Reddit, where someone asked how to “show both Imperial and Metric steel sizes in a Parts List”

I initially replied with a single line of iLogic, but this got me thinking. I’ve written an iLogic utility that lets users specify an alternative value for each of the members in their Frame model . The code is set up for 5 frame members, but could easily be expanded to include more.

The code is looks at the “Stock Number” of the frame member (in iProperties) and then adds a custom iProperty for the alternative member size.

Sizes are set up in the table shown below o1 is the Stock number and oA is the Alternative size, likewise for o2 and oB etc.

'Alternate Member sizes
			o1 = "100x100x3" 	: oA = "ANSI 4 x 4 x 1/4"
			o2 = "50x50x2" 		: oB = "ANSI 2 x 2 x 1/8"
			o3 = "" 			: oC = ""
			o4 = "" 			: oD = ""
			o5 = "" 			: oE = ""


Inventor iproperties

Here is an animated GIF showing the code in action:

Alternate Frame sizes -748
Click me for higher resolution version


Below is the iLogic code

'iLogic code by Clint Brown @ClintBrown3D
'Code originally posted at
Sub Main()
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisApplication.ActiveDocument
Call Iterate(oAsmDoc.ComponentDefinition.Occurrences, 1)
End Sub

Private Sub Iterate(Occurrences As ComponentOccurrences, Level As Integer)
	'Iterate through Assembly

	Dim oOcc As ComponentOccurrence
	For Each oOcc In Occurrences

		'Find Parts in Assembly
		Dim ClintsPart As String
		ClintsPart = oOcc.Name
			'Alternate Member sizes
			o1 = "100x100x3" 	: oA = "ANSI 4 x 4 x 1/4"
			o2 = "50x50x2" 		: oB = "ANSI 2 x 2 x 1/8"
			o3 = "" 			: oC = ""
			o4 = "" 			: oD = ""
			o5 = "" 			: oE = ""

			'Write iProps to Parts
			If iProperties.Value(ClintsPart, "Project", "Stock Number") = o1 Then : iProperties.Expression(ClintsPart, "Custom", "Alternate Size") = oA : End If
			If iProperties.Value(ClintsPart, "Project", "Stock Number") = o2 Then : iProperties.Expression(ClintsPart, "Custom", "Alternate Size") = oB : End If
			If iProperties.Value(ClintsPart, "Project", "Stock Number") = o3 Then : iProperties.Expression(ClintsPart, "Custom", "Alternate Size") = oC : End If
			If iProperties.Value(ClintsPart, "Project", "Stock Number") = o4 Then : iProperties.Expression(ClintsPart, "Custom", "Alternate Size") = oD : End If
			If iProperties.Value(ClintsPart, "Project", "Stock Number") = o5 Then : iProperties.Expression(ClintsPart, "Custom", "Alternate Size") = oE : End If
		End Try

		'Cycle through the sub assemblies 
		If oOcc.DefinitionDocumentType = kAssemblyDocumentObject Then
			Call Iterate(oOcc.SubOccurrences, Level + 1)
		End If
End Sub

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