How to iterate and activate each row in an iAssembly or iPart without the Inventor UI.

[AlexFielder]

Hi all,

Apologies if I have overlooked an existing example but I am just about to head out for the day and wondered if I have missed or overlooked an example somewhere that shows how to iterate the table rows of an iAssembly (or iPart) without using the Inventor UI?

The working example I have that shows how to do so using the UI is as follows:

Sub Main()
CheckiTableForErrors()
End Sub
Sub CheckiTableForErrors()
    Dim oErrorManager As ErrorManager = ThisApplication.ErrorManager

    If TypeOf (ThisApplication.activedocument) Is partdocument Then
        Dim oDoc As PartDocument = ThisApplication.ActiveDocument
        Dim oiPart As iPartFactory = oDoc.ComponentDefinition.iPartFactory
        Dim oTop As BrowserNode = oDoc.BrowserPanes("Model").TopNode
        Dim bHasErrorOrWarning As Boolean
        Dim i As Integer
        InventorVb.DocumentUpdate()
        ThisApplication.SilentOperation = True
        For i = 1 To oiPart.TableRows.Count 'use first 10 rows only for debugging purposes!
            ' Highlight the 3rd iPart table row which has invalid data
            oTop.BrowserNodes("Table").BrowserNodes.Item(i).DoSelect

            ' Activate the iPart table row
            Dim oCommand As ControlDefinition = ThisApplication.CommandManager.ControlDefinitions("PartComputeiPartRowCtxCmd")
            oCommand.Execute

            ThisApplication.SilentOperation = False
            ThisApplication.CommandManager.ControlDefinitions.Item("AppZoomallCmd").Execute
            If oErrorManager.HasErrors Or oErrorManager.HasWarnings Then
                MessageBox.Show(oErrorManager.LastMessage, "Title")
            End If
        Next i
        MessageBox.Show("No errors shown = None found!", "Title")
    ElseIf TypeOf (ThisApplication.activedocument) Is assemblydocument Then
        Dim odoc As assemblydocument = ThisApplication.activedocument
        Dim iAssy As iAssemblyFactory = odoc.componentdefinition.iassemblyfactory
        Dim oTop As BrowserNode = odoc.BrowserPanes("Model").TopNode
        Dim bHasErrorOrWarning As Boolean
        Dim i As Integer
        InventorVb.DocumentUpdate()
        ThisApplication.SilentOperation = True
        For rowIndex = 1 To iAssy.tablerows.count
            oTop.BrowserNodes("Table").BrowserNodes.Item(i).DoSelect
            Dim oCommand As ControlDefinition = ThisApplication.CommandManager.ControlDefinitions("PartComputeiPartRowCtxCmd")
            oCommand.Execute
            ThisApplication.SilentOperation = False
            ThisApplication.CommandManager.ControlDefinitions.Item("AppZoomallCmd").Execute
            If oErrorManager.HasErrors Or oErrorManager.HasWarnings Then
                MessageBox.Show(oErrorManager.LastMessage, "Title")
            End If

        Next
    End If
End Sub

Which works fine if you wish to verify that each row is buildable as a user- but can I do the same without access to the Inventor UI? (for instance if the iAssembly/iPart is opened by coolOrange PowerJobs)

Thanks,

Alex.

[Frederick_Law]

VBA Macro to update and generate all iPart/iAssembly files:

Sub CreateAlliPart()
    On Error Resume Next
    
    ' Open the factory document
    Dim oFacDoc As PartDocument
    ' Set oFacDoc = oInventorApp.Documents.Open(sFacFullFileName)
    Set oFacDoc = ThisApplication.ActiveDocument

    Dim oCompDef As PartComponentDefinition
    Set oCompDef = oFacDoc.ComponentDefinition

    Dim iNumRows As Integer
    Dim oiPrtFac As iPartFactory
    Set oiPrtFac = oCompDef.iPartFactory

    iNumRows = oiPrtFac.TableRows.Count

    ' Create a member for each row and update the member to make sure that it is in-synch
    ' with the factory
    Dim iRow As Integer
    Dim oMem As iPartMember
    For iRow = 1 To iNumRows
        Set oMem = oiPrtFac.CreateMember(iRow)

        Dim oMemDoc As Document
        Set oMemDoc = oMem.Parent.Document

        ' Update the member
        oMemDoc.Update
        oMemDoc.Save
        oMemDoc.Close
    Next

    oFacDoc.Close

End Sub

Sub CreateAlliAssemblies()
    On Error Resume Next
    
    ' Open the factory document
    Dim oFacDoc As AssemblyDocument
    ' Set oFacDoc = oInventorApp.Documents.Open(sFacFullFileName)
    Set oFacDoc = ThisApplication.ActiveDocument

    Dim oCompDef As AssemblyComponentDefinition
    Set oCompDef = oFacDoc.ComponentDefinition

    Dim iNumRows As Integer
    Dim oiAsmFac As iAssemblyFactory
    Set oiAsmFac = oCompDef.iAssemblyFactory

    iNumRows = oiAsmFac.TableRows.Count

    ' Create a member for each row and update the member to make sure that it is in-synch
    ' with the factory
    Dim iRow As Long
    'Dim oiMem As iAssemblyMember
    'Set oiMem = oiAsmFac.
    For iRow = 1 To iNumRows
    
        'Set oiMem = oiAsmFac.CreateMember(iRow)

        Dim oMemDoc As Document
        Set oMemDoc = oiMem.Parent.Document

        ' Update the member
        oMemDoc.Update
        oMemDoc.Save
        oMemDoc.Close
    Next

    oFacDoc.Close

End Sub

[AlexFielder]

thanks @Frederick_Law that is really useful.

My next question (thinking out loud) is that I am exporting BOM data from Inventor Assemblies (iAssemblies in particular) and, because of the way iAssemblies function, exporting a BOM from an iAssembly always results in the same data within the exported data. 

I think I can workaround this (for the purposes of doing this from inside Vault) by wrapping a for loop of the manner you describe in your VBA sample, inside an Inventor transaction (in case something goes awry) and then, to create a new transaction inside of which I can delete the iAssembly table (thus converting the iAssembly into a regular assembly), then run the BOM export, before undoing the second transaction and continuing the loop again.

[Frederick_Law]

Haven't used iPart/iAssembly for a while.

Using ModelState but idea is similar.

Activate each iPart/iAssembly/ModelState and do what you need to do.

The "problem" with iPart/iAssembly is the member files are not created until it is used.

Hence the CreateMember.

https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-6A5B70B1-5AF3-4824-9060-857F22114B4F