Get iProperties of Component Occurrences

[Kyle.Arnold]

Hi Folks.

I'm working on a program to get into the iProperties of each Component within an Assembly.

The attached code can run through each occurrence in an assembly and return the "Name" displayed in the browser window, printed out as a list in the Immediate window of the VBA Editor.

I would like to return the value of the "Category" iProperty of each occurrence.  I would assume that I need to access the part associated with each occurrence in order to get to the iProperties of that part. 

After fighting it most of the day yesterday, I'm fed up and need some help.

How do I access the iProperties of an OCCURRENCE? I can get the iProperties from a PART, ASSEMBLY, or DRAWING easily, but OCCURRENCES are killing me... Should be a cakewalk for some of you more experienced people.

The attached code was inspired by/imitates/borrowed from a Brian Ekins post on Mod the Machine. 

Sub Test()

' Get the active assembly.
Dim oAsmDoc As AssemblyDocument
Set oAsmDoc = ThisApplication.ActiveDocument

' Get the definition of the assembly.
Dim oAsmCompDef As AssemblyComponentDefinition
Set oAsmCompDef = oAsmDoc.ComponentDefinition

' Get the occurrences that represent this document.
Dim oOccs As ComponentOccurrencesEnumerator
Set oOccs = oAsmCompDef.Occurrences.AllLeafOccurrences

' Iterate through the Occurrences
Dim oOcc As ComponentOccurrence
For Each oOcc In oOccs

    Debug.Print oOcc.Name
    
Next

End Sub

[MechMachineMan]

You jsut need to access the Component Definition of the Occurrence, and from there you can access the Document from where you grab the iProperties.

iProps are not stored on occurrences, but only within the part, so pulling an iProp from an occurrence doesn't make sense; instead you need to pull it from the document the occurrence references.

Also, depending on what you are trying to accomplish, it may just be easier to iterate through all of the referenced documents for the active file, rather than going through occurrences. You still will end up accessing the same files in the end, so the only real benefit to going through occurrences is for order/suppression.

See resource below for API regarding component definition.

"C:\Program Files\Autodesk\Inventor 2016\Local Help\admapi_20_0.chm"

See below for "proper" calls to properties:

http://modthemachine.typepad.com/my_weblog/2010/02/accessing-iproperties.html

ie; 

'in vb.net, not vba, so use as a rule/external rule vs as a macro

Sub Main()

Dim oDoc as Document

For Each oDoc in ThisApplication.ActiveDocument.AllReferencedDocuments

      oStr = oDoc.PropertySets.Item("Design Tracking Properties").Item("Part Number").Value & " <<<<<< " & oStr

Next

MsgBox(oStr)

End Sub

[Kyle.Arnold]

AllReferencedDocuments won't work for me in the way you show above, becuase I need a list of the Category iProperty of each Occurrence or Leaf.  I need the list to tell me what each leaf's Category is regardless of how many time that particular refereced part shows up in an assembly. For example:

Assembly A's browser tree looks like this-

Part 1:1

Part 1:2

Part 1:3

Part 2:1

Part 3:1

Part 1:4

I need the program to return:

Category X

Category X

Category X

Category Y

Category Z

Category X

Do you know if there is a way to get this using AllLeafOccurrences or something similar?

[Kyle.Arnold]

Sub Main()

Dim oDoc As Document

For Each oDoc In ThisApplication.ActiveDocument.AllReferencedDocuments

      oStr = oDoc.PropertySets.Item("Inventor Document Summary Information").Item("Category").Value & vbNewLine & oStr
Next

Debug.Print oStr

End Sub

A slight modification of your proposed code gives me what I'm looking for EXCEPT it's giving me the category of the referenced documents only. On an assembly with 9 parts (4 unique) it only returns the category of each unique part, so 4 lines returned rather than the desired 9.  

I don't know how to adapt it to give me the category of every occurrence in the assembly.

[MechMachineMan]

http://modthemachine.typepad.com/my_weblog/2009/03/accessing-assembly-components.html

[Kyle.Arnold]

Yep, that's the page I got the idea and the first draft of code from. In the last paragraph of the "Assembly Structure" section, the author is talking about replacing the "Debug.Print" line and says:

"This line is executed for every occurrence in the assembly.  You can replace this with code that performs whatever functionality you need to accomplish.  For example, if you need to create a custom BOM your code might access the document that’s referenced by this occurrence and extract some iProperty values and then print this out as part of a structured BOM." 

The underlined section is what I can't figure out.  How do I extract iProperties of the Parts referenced by the Occurrences?

All should have to do is replace the "Debug.Print" line of that code with the code neccessary to extract the iProperties.  I don't know enough about VBA and using the Inventor API to figure out the answer on my own.

There is definitely something that I'm missing.

[MechMachineMan]

This is close, but still not quite what you need.

Why exactly do you need each browser node to be printed/accessed though? They change quite often so it seems to be a weird thing to track.

SyntaxEditor Code Snippet

Class PVars
    Dim oPStr As String

Sub Main()
    Dim PVar As New PVars
    Dim oAsmDoc As AssemblyDocument 
    oAsmDoc = ThisApplication.ActiveDocument 

    TraverseAssembly(oAsmDoc.ComponentDefinition.Occurrences, 1)
    MsgBox(PVar.oPStr)
End Sub 

Sub TraverseAssembly(Occurrences As ComponentOccurrences, Level As Integer) 
       Dim PVar As New PVars
    Dim oOcc As ComponentOccurrence 
    For Each oOcc In Occurrences
        PVar.oPStr = PVar.oPStr & " - " & oOcc.Definition.Document.PropertySets.Item("Inventor Document Summary Information").Item("Category").Value
        MsgBox(PVar.oPStr)
        If oOcc.DefinitionDocumentType = kAssemblyDocumentObject Then 
            Call TraverseAssembly(oOcc.SubOccurrences, Level + 1) 
        End If 
    Next
End Sub

End Class

[MechMachineMan]

Here are 2 working methods you could possibly adapt:

Note: Both are written as external rules, rather than macros.

Outputs to msgbox:

Sub Main()
    Dim oStr As String
    Dim oAsmDoc As AssemblyDocument 
    oAsmDoc = ThisApplication.ActiveDocument 

    oStr = TraverseAssembly(oAsmDoc.ComponentDefinition.Occurrences, 1, oStr)
    MsgBox(oStr)
End Sub 

Function TraverseAssembly(Occurrences As ComponentOccurrences, Level As Integer, oStr As String) 

   	Dim oOcc As ComponentOccurrence 
   	For Each oOcc In Occurrences
        oStr = oStr & " - " & oOcc.Definition.Document.PropertySets.Item("Inventor Document Summary Information").Item("Category").Value
		'oStr = oStr & " - " & oOcc.Definition.Document.PropertySets.Item("Design Tracking Properties").Item("Stock Number").Value
        If oOcc.DefinitionDocumentType = kAssemblyDocumentObject Then 
            oStr = TraverseAssembly(oOcc.SubOccurrences, Level + 1, oStr) 
        End If
    Next
	Return oStr
End Function

Outputs to text file:

SyntaxEditor Code Snippet

Public Class PVars
    Shared oTextSave As String = "C:\Windows\Temp\iLogicBuffer.txt"

Sub Main()
    Dim PVar As New PVars
    oWrite = System.IO.File.CreateText(PVar.oTextSave)
    oWrite.WriteLine("CATEGORY")
    oWrite.Close()
    
    Dim oStr As String
    Dim oAsmDoc As AssemblyDocument 
    oAsmDoc = ThisApplication.ActiveDocument 

    TraverseAssembly(oAsmDoc.ComponentDefinition.Occurrences, 1)
    
    Process.Start ("Notepad.exe",PVar.oTextSave)
End Sub 

Sub TraverseAssembly(Occurrences As ComponentOccurrences, Level As Integer) 
    Dim PVar As New PVars
       Dim oOcc As ComponentOccurrence 
       For Each oOcc In Occurrences
        oWrite = System.IO.File.AppendText(PVar.oTextSave)
        'oWrite.WriteLine(oOcc.Definition.Document.PropertySets.Item("Design Tracking Properties").Item("Stock Number").Value)
        oWrite.WriteLine(oOcc.Definition.Document.PropertySets.Item("Inventor Document Summary Information").Item("Category").Value)
        oWrite.Flush()
        oWrite.Close()

        If oOcc.DefinitionDocumentType = kAssemblyDocumentObject Then 
            TraverseAssembly(oOcc.SubOccurrences, Level + 1) 
        End If
    Next
End Sub

End Class

[Kyle.Arnold]

Ok, I'm back after a month-long hiatus...

So, trying those two options, I can get it to work exactly how I want except that it works in an assembly file. Which, judging by the first few lines of code, this program was intended to do.

However, I'm trying to do exactly what the first of the two above programs does, except I want to do it from a drawing file.

Assuming that I'm only worried about doing this for drawings of assembly files, how do I "step into" the Assembly files represented in each view?

[MechMachineMan]

If you want it only for the active sheet when the rule is ran, you need to access the drawing view's referenced document.

ie;

ThisApplication.ActiveDocument.ActiveSheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocument

[MechMachineMan · Accepted solution]

So full code to check one sheet with an assembly on it in the active document would be:

Sub Main()
    Dim oStr As String

    Dim oDrawingDoc As DrawingDocument 
    Try
        oDwgDoc = ThisApplication.ActiveDocument 
    Catch
        MsgBox("For use in drawing documents only!")
        Exit Sub
    End Try

    Dim oAsmDoc As AssemblyDocument 
    Try
        oAsmDoc = oDwgDoc.ActiveSheet.DrawingViews.Item(1).ReferencedDocumentDescriptor.ReferencedDocument
    Catch
        MsgBox("This rule only works on drawing sheets with an assembly as the first view!")
        Exit Sub
    End Try

    oStr = TraverseAssembly(oAsmDoc.ComponentDefinition.Occurrences, 1, oStr)
    MsgBox(oStr)
End Sub 

Function TraverseAssembly(Occurrences As ComponentOccurrences, Level As Integer, oStr As String) 

   	Dim oOcc As ComponentOccurrence 
   	For Each oOcc In Occurrences
        oStr = oStr & vblf & oOcc.Definition.Document.DisplayName & " - " & oOcc.Definition.Document.PropertySets.Item("Inventor Document Summary Information").Item("Category").Value
		'oStr = oStr & " - " & oOcc.Definition.Document.PropertySets.Item("Design Tracking Properties").Item("Stock Number").Value
        If oOcc.DefinitionDocumentType = kAssemblyDocumentObject Then 
            oStr = TraverseAssembly(oOcc.SubOccurrences, Level + 1, oStr) 
        End If
    Next
	Return oStr
End Function

[Kyle.Arnold]

Fantastic! This is exactly what I was trying to accomplish!!!  Made my day!

[Anonymous]

Hi, can you please explain where exactly do I have to get in and type the definition code please?

Thanks,

Gabriel

[dschulteHR4D5]

Hello, i am using a modified version of this code, to display the materials i have set in an assembly, basically a quick reference, i use material library to automate drawings.. So this is the code i am using, which works perfectly, but a couple questions...

Sub main
'Make sure ASM document is active'
If ThisDoc.Document.DocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then
MsgBox("An Assembly Document must be active for this rule to work. Exiting.", vbCritical, "")
Exit Sub
End If

Dim oADoc As AssemblyDocument = ThisDoc.Document


oStr = TraverseAssembly(oADoc.ComponentDefinition.Occurrences, 1, oStr)
MsgBox(oStr)
End Sub

Function TraverseAssembly(Occurrences As ComponentOccurrences, Level As Integer, oStr As String)

Dim oOcc As ComponentOccurrence
For Each oOcc In Occurrences
oStr = oStr & vbCrLf & oOcc.Definition.Document.DisplayName & " = " & oOcc.Definition.Document.PropertySets.Item("Design Tracking Properties").Item("Material").Value
'oStr = oStr & " - " & oOcc.Definition.Document.PropertySets.Item("Design Tracking Properties").Item("Part Number").Value
If oOcc.DefinitionDocumentType = kAssemblyDocumentObject Then
oStr = TraverseAssembly(oOcc.SubOccurrences, Level + 1, oStr)
End If
Next
Return oStr
End Function



1) when running this rule, the MsgBox title comes up as random characters and letters, is there any way to change this to say something like, IPT Material List?

2) The List shows the file extension, like
Part1.ipt =
Part2.ipt =
Is there a different command to pull the displayname without the .ipt?

thanks for any help!!

[dudde.giridhar]

Hello,

In this reply,

you have given the method to get the properties from referenced document but not from the occurrence.

There might be new cutouts made in assembly level, so both are not same,

Please let us know if there is any chance to get the updated iproperties from component occurrence of assembly doc.

Thanks in advance

[nmunro]

If you are on Inventor 2022 or later, instance properties enable you to assign unique property values to each assembly component occurrence. Search for Print instance properties  in the API help to find an example VBA macro that should get you started.

[scott_ainsworth]

I'm working in Inventor 2024 and need to do something similar.  My attempts to access property sets via: 

oCustomProps = oOccurrence.Definition.Document.PropertySets.Item("Custom Properties")

 results in an error message: 

"Error on line 32 in rule: AW Next Assy and Qty, in document: 40066295-A01.iam

Class not registered"

When I am typing this into the ilogic editor, I never get a pick for anything other than ToString after "Document."  It seems like something is amiss.  

Any help would be welcome.

[MechMachineMan]

Have you actually declared and assigned 'oOccurrence' anywhere in your
document?

Have you declared the 'oCustomProp' as well?