Hi @mikejones. I am not sure about the true scope of your task, or how you need to specify which view to process, so I wasn't sure how deep you wanted this to go. For instance, do you only want the rule to process the view if it directly references an assembly? Do you only want the part numbers of 'top level' assembly components in that assembly, or do you want it to go down into sub levels, and sub sub levels, etc? Do you only want one part number listed for each 'unique' component (even if multiple components reference same model file), or one for every component, even if there are 10 components referencing the same model file? Below is an example that lets you 'Pick' a view, then just processes the top level components that are not suppressed.
Sub Main
Dim oView As DrawingView = PickDrawingView
Dim oModel As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oPNList As New List(Of String)
If oModel.DocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then Exit Sub
Dim oAModel As AssemblyDocument = oModel
Dim oOccs As ComponentOccurrences = oAModel.ComponentDefinition.Occurrences
If oOccs.Count = 0 Then Exit Sub 'no components to process
For Each oOcc As ComponentOccurrence In oOccs
If oOcc.Suppressed Then Continue For
Dim oPN As String = iProperties.Value(oOcc.Name, "Project", "Part Number")
oPNList.Add(oPN)
Next
oMyPN = InputListBox("", oPNList, "", "Part Numbers")
End Sub
Function PickDrawingView(Optional oPrompt As String = vbNullString) As DrawingView
If oPrompt = "" Then oPrompt = "Select a Drawing View."
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, oPrompt)
If IsNothing(oObj) OrElse (TypeOf oObj Is DrawingView = False) Then Return Nothing
Dim oView As DrawingView = oObj
Return oView
End FunctionIf this solved your problem, or answered your question, please click ACCEPT SOLUTION .
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Wesley Crihfield
(Not an Autodesk Employee)
OK. I have modified the code to iterate through the assembly document's 'AllReferencedDocuments', which reaches every level of the assembly. It is still possible though, that this does not include some documents, if every component, in every level that references that document has been suppressed. I am using an iLogic shortcut within the loop that was only made available in the 2021 product year, so if you are using an earlier version, we may have to change that to using API route, to get the iProperty value. Just let me know. I am just using an InputListBox to show you the resulting list of part numbers, but you can modify to do whatever you need with that list.
Sub Main
Dim oView As DrawingView = PickDrawingView
Dim oModel As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oPNList As New List(Of String)
If oModel.DocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then Exit Sub
Dim oAModel As AssemblyDocument = oModel
Dim oRefDocs As DocumentsEnumerator = oAModel.AllReferencedDocuments
If oRefDocs.Count = 0 Then Exit Sub
For Each oRefDoc As Document In oRefDocs
Dim SOP = StandardObjectFactory.Create(oRefDoc) 'Inventor 2021 or later only
Dim oPN As String = SOP.iProperties.Value("Project", "Part Number")
oPNList.Add(oPN)
Next 'oRefDoc
oMyPN = InputListBox("", oPNList, "", "Part Numbers")
End Sub
Function PickDrawingView(Optional oPrompt As String = vbNullString) As DrawingView
If oPrompt = "" Then oPrompt = "Select a Drawing View."
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, oPrompt)
If IsNothing(oObj) OrElse (TypeOf oObj Is DrawingView = False) Then Return Nothing
Dim oView As DrawingView = oObj
Return oView
End Function
Wesley Crihfield
(Not an Autodesk Employee)
OK. Here you go. I think this should do the trick.
Sub Main
Dim oView As DrawingView = PickDrawingView
Dim oModel As Document = oView.ReferencedDocumentDescriptor.ReferencedDocument
Dim oPNList As New List(Of String)
If oModel.DocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then Exit Sub
Dim oAModel As AssemblyDocument = oModel
Dim oRefDocs As DocumentsEnumerator = oAModel.AllReferencedDocuments
If oRefDocs.Count = 0 Then Exit Sub
For Each oRefDoc As Document In oRefDocs
Dim oBOMSt As BOMStructureEnum = oRefDoc.ComponentDefinition.BOMStructure
If oBOMSt = BOMStructureEnum.kReferenceBOMStructure Or _
oBOMSt = BOMStructureEnum.kPhantomBOMStructure Then
Continue For 'skip to next oRefDoc in loop, if any
End If
Dim SOP = StandardObjectFactory.Create(oRefDoc) 'Inventor 2021 or later only
Dim oPN As String = SOP.iProperties.Value("Project", "Part Number")
oPNList.Add(oPN)
Next 'oRefDoc
oMyPN = InputListBox("", oPNList, "", "Part Numbers")
End Sub
Function PickDrawingView(Optional oPrompt As String = vbNullString) As DrawingView
If oPrompt = "" Then oPrompt = "Select a Drawing View."
oObj = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kDrawingViewFilter, oPrompt)
If IsNothing(oObj) OrElse (TypeOf oObj Is DrawingView = False) Then Return Nothing
Dim oView As DrawingView = oObj
Return oView
End Function
Wesley Crihfield
(Not an Autodesk Employee)
Hi @mikejones. I'm still using 2022.3.2, so I wouldn't be able to open your files, but using Parts only BOMView certainly sounds doable. To you want to keep the 'Pick View' functionality, or would you prefer to just have it work with the first view on the active sheet of the drawing? And is the 'InputListBox' thing working OK for you, or would you prefer to have the bulk of the code set-up as a separate Function which will return the List(Of String) object, since this is just part of a larger automation project?
Wesley Crihfield
(Not an Autodesk Employee)
To avoid the weldment BOMStructure issue, we could just try doing the iteration of the assembly components directly, instead of using the Parts Only BOMView, and instead of using the AllReferendedDocuments routes. It's slightly less efficient, but certainly doable that way, I would just have to incorporate an extra List type variable for keeping track of component referenced documents that I've already processed, so I don't process the same ones multiple times. I have done that before several times in other solutions, so its not too bit a deal. I might also have to incorporate a separate recursive Sub routine, for digging down through all the levels, but I've done that before many times too, so no big deal there either. Getting the first base view on the active sheet shouldn't be a problem either. I would just have to start the code a bit more traditionally. No promises on timing, because I've got a few things going on at the same time, but I'll see what I can do.
Wesley Crihfield
(Not an Autodesk Employee)
Hi @mikejones. I've got something for you to try out. It may look a bit intimidating, but I think it might work for you. I only put a few comments in there, because its already a fairly lengthy code, but if you need to ask about anything, please do. I'm not 100% sure if the Document object filter will work as planned now that ModelStates have complicated those references, but if not, we can try something else, like maybe FullFileName or FullDocumentName or something else unique about each one. Let me know how this works out for you.
Class ThisRule
Dim oDocs As List(Of Document) 'shared with all routines
Dim oPNList As List(Of String) 'shared with all routines
Sub Main
If ThisDoc.Document.DocumentType <> DocumentTypeEnum.kDrawingDocumentObject Then
MsgBox("A Drawing document must be active for this code to work. Exiting.", vbCritical, "")
Exit Sub
End If
Dim oDDoc As DrawingDocument = ThisDoc.Document
Dim oViews As DrawingViews = oDDoc.ActiveSheet.DrawingViews
If oViews.Count = 0 Then Exit Sub 'may want a feedback message or Log entry here.
Dim oBV As DrawingView
For Each oView As DrawingView In oViews
If oView.ViewType = DrawingViewTypeEnum.kStandardDrawingViewType Then
oBV = oView : Exit For
End If
Next 'oView
If IsNothing(oBV) Then Exit Sub 'may want a feedback message or Log entry here.
Dim oADoc As AssemblyDocument = oBV.ReferencedDocumentDescriptor.ReferencedDocument
Dim oOccs As ComponentOccurrences = oADoc.ComponentDefinition.Occurrences
oDocs = New List(Of Document) 'to initiate it
oPNList = New List(Of String) 'to initiate it
RecursivelyProcessComponents(oOccs)
oMyPN = InputListBox("", oPNList, "", "Part Numbers")
End Sub
Sub RecursivelyProcessComponents(oComps As ComponentOccurrences)
If IsNothing(oComps) OrElse oComps.Count = 0 Then Exit Sub
For Each oComp As ComponentOccurrence In oComps
Dim ProcessFurther As Boolean = ProcessComponent(oComp) 'run our other routine
If ProcessFurther = False Then Exit Sub
If oComp.SubOccurrences.Count > 0 Then
RecursivelyProcessComponents(oComp.SubOccurrences)
End If
Next
End Sub
Function ProcessComponent(oComp As ComponentOccurrence) As Boolean
If IsNothing(oComp) OrElse oComp.Suppressed Then Return False
'filter by BOMStructure values
'Note: BOMStructure of component can be different than its referenced document
If oComp.BOMStructure <> BOMStructureEnum.kNormalBOMStructure And _
oComp.BOMStructure <> BOMStructureEnum.kInseparableBOMStructure Then
Return False
End If
If oComp.DefinitionDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
If oComp.Definition.BOMStructure = BOMStructureEnum.kReferenceBOMStructure Then Return False
ElseIf oComp.DefinitionDocumentType = DocumentTypeEnum.kPartDocumentObject Then
If oComp.Definition.BOMStructure <> BOMStructureEnum.kNormalBOMStructure Then Return False
End If
Dim oDoc As Document = oComp.Definition.Document
If oDocs.Contains(oDoc) Then Return False 'do not process the same document again
Dim SOP = StandardObjectFactory.Create(oDoc) 'Inventor 2021 or later only
Dim oPN As String = SOP.iProperties.Value("Project", "Part Number")
oPNList.Add(oPN)
oDocs.Add(oDoc)
Return True 'return True, so it will process any sub occurrances of this component
End Function
End Class
Wesley Crihfield
(Not an Autodesk Employee)
Good morning @mikejones. I see my mistake. I should have used the 'oView' variable in that line, instead of the 'oBV' variable. The loop definition line is using the oView variable, so it will always have a value, while the oBV variable will not have a value until after that line, if the oView passes the test. So that line should have been:
If oView.ViewType = DrawingViewTypeEnum.kStandardDrawingViewType ThenI will fix that line in my code, so others can copy/paste it without the error being in there.
Wesley Crihfield
(Not an Autodesk Employee)
