Thank you and others for your starting code. Here's an ilogic macro for copying the part and drawing together. Basically does the same thing as a copy design in Vault.
Change log:
1. Doesn't replace it in the assembly anymore.
2. Extension will be dropped if user puts in the extension as part of its name.
3. Workaround implemented to correctly show the initial folder
4. Commented out touching the vault addin. Undesirable behaviour for my application.
5. Close out background openings of files.
6. Changed filetype to idw instead of dwg for my purposes.
7. Commented out some iproperty stuff I didn't want for what I need.
'Adapted from darrell.wcd at https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/copy-model-and-drawing/td-p/11505007
Sub main
' Dim oVault As ApplicationAddIn
' For Each oVault In ThisApplication.ApplicationAddIns
' If oVault.DisplayName = "Inventor Vault" Then Exit For
' Next
' If oVault IsNot Nothing Then oVault.Deactivate
'SilentOperation = True
''' Set drawing extension
Dim DWGType As String = ".idw"
Dim BoxNote As String = "Drawing Automation"
Dim filex As String 'file extension
opendoc = ThisDoc.PathAndFileName()
''' Initial file dialogue box declarations
oDoc = ThisDoc.Document
filePath = ThisDoc.Path
'MessageBox.Show(filePath)
''' check file type and set dialog filter
If oDoc.DocumentType = kPartDocumentObject Then
'oFileDlg.Filter = "Autodesk Inventor Part Files (*.ipt)|*.ipt"
filex = ".ipt"
Else If oDoc.DocumentType = kAssemblyDocumentObject Then
'oFileDlg.Filter = "Autodesk Inventor Assembly Files (*.iam)|*.iam"
filex = ".iam"
Else If oDoc.DocumentType = kDrawingDocumentObject Then
'oFileDlg.Filter = "Autodesk Inventor Drawing Files (*.idw)|*.idw"
filex = ".idw"
End If
'doc = ThisApplication.Documents.Open(opendoc & filex,True)
''' Get current filename
CurrentFilename = ThisDoc.PathAndFileName(False)
oPart = ThisDoc.PathAndFileName(False)
''' Check that the drawing for this assembly can be found
If Not System.IO.File.Exists(CurrentFilename & DWGType) Then
MessageBox.Show("Unable to locate the drawing file below for this part:" & vbLf & vbLf & _
CurrentFilename & DWGType & vbLf & vbLf & _
"Please make sure it's in the same folder as this part, has the same name, and has the file extension. '"& DWGType & "'", BoxNote)
Return
End If
'define the active document
oDoc = ThisDoc.Document
''' create a file dialog box
Dim oFileDlg As Inventor.FileDialog = Nothing
InventorVb.Application.CreateFileDialog(oFileDlg)
oFileDlg.InitialDirectory = ThisDoc.Path() ' Bug since Sept 2021 causes this line to be ignored at the .ShowAs() line
'Work Around for ShowSave() bug. Thank you ThaleFUWKH (https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/file-dialog-initial-directory-stuck-on-workspace/m-p/6883307#M70261)
Dim iFileName As String = ThisDoc.Path() + "\" + ThisDoc.FileName(False)
'set the file name string to use in the input box
oFileDlg.FileName = iFileName 'iProperties.Value("Project", "Part Number")
'work with an error created by the user backing out of the save
oFileDlg.CancelError = True
Logger.Debug("oFileDlg.FileName " & oFileDlg.FileName)
On Error GoTo 1: 'Error catch for if user cancels out
'specify the file dialog as a save dialog (rather than a open dialog)
oFileDlg.ShowSave()
'On Error GoTo 1:'Resume Next
''' catch an empty string in the input
If Err.Number <> 0 Then
Logger.Debug("Error at file dialogue box")
MessageBox.Show("No File Saved.", "iLogic: Dialog Canceled")
ElseIf oFileDlg.FileName <> "" Then
MyFile = oFileDlg.FileName
Logger.Debug("No Error for file save dialogue")
''' Get new filename (without extension)
NewFileName = MyFile'filePath &"\"& FileName
NewFileName = System.IO.Path.ChangeExtension(NewFileName, Nothing)
'If Str.Contains(MyFile, ".ipt") Or Str.Contains(MyFile, ".iam") Or Str.Contains(MyFile, ".idw") Or Str.Contains(MyFile, ".dwg") Then
'MyFile = Right(MyFile, (Len(MyFile) -4))
'End If
Logger.Debug("NewFileName/MyFile: " + MyFile + filex)
''' Perform Save As Of Assembly/Part
ThisDoc.Document.SaveAs(NewFileName & filex, True)
Logger.Debug("New file save successful")
''' Update model iProperties
iNewFileName = ThisDoc.FileName(False)
oDoc.PropertySets("Design Tracking Properties").Item("Part Number").Value = iNewFileName
Logger.Debug("File save attempted")
''' Open the current drawing (in same folder location)
Dim oDrawingDoc As DrawingDocument = ThisApplication.Documents.Open(CurrentFilename & DWGType,False)
oDrawingDoc.SaveAs(NewFileName & DWGType, True)
oDrawingDoc.Close
oDrawingDoc = ThisApplication.Documents.Open(NewFileName & DWGType,False)
Logger.Debug("File save successful :" & NewFileName & DWGType)
''' Replace reference to assembly model
Dim oFD As FileDescriptor
oFD = oDrawingDoc.ReferencedFileDescriptors(1).DocumentDescriptor.ReferencedFileDescriptor
oFD.ReplaceReference(NewFileName & filex)
oDrawingDoc.Update()
'oDrawingDoc.Activate()
' Perform 'Save As' on the drawing
Dim newdwgname As String = NewFileName & DWGType
Logger.Debug("newdwgname :" + newdwgname)
oDrawingDoc.Save()
' ThisApplication.Documents.Open(oDWGPath, True)
oDrawingDoc.Close
Logger.Debug("Replaced model reference")
Call Prop
End If
1:
'ThisDoc.Document.Activate
'Call Prop
'SilentOperation = False
'oVault.Activate
Logger.Debug("completed")
End Sub
Public Sub Prop
oDoc = ThisApplication.ActiveDocument
iProperties.Value("Summary", "Author") = ThisApplication.GeneralOptions.UserName
iProperties.Value("Project", "Designer") = ThisApplication.GeneralOptions.UserName
'iProperties.Value("Project", "Stock Number") = "=<Part Number>"
iProperties.Value("Project", "Creation Date" ) = Now
InventorVb.DocumentUpdate()
' Save the document and its dependents.
oDoc.Save2(True)
oDoc.Save2(True)
End Sub
