Scan assembly and all sub-assemblies to export flat patterns
You could try something like this. The dxf file gets saved in the same directory as the part.
Public Sub main()
Dim doc As AssemblyDocument = ThisDoc.Document
For Each refDoc As Document In doc.AllReferencedDocuments
If (refDoc.DocumentType <> DocumentTypeEnum.kPartDocumentObject) Then Continue For
If (refDoc.SubType <> "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}") Then Continue For
Dim sheetMetalDoc = ThisApplication.Documents.Open(refDoc.FullFileName)
Dim fileName = CreateFileName(sheetMetalDoc)
Export(sheetMetalDoc, fileName)
Next
doc.Activate()
End Sub
Function CreateFileName(doc As PartDocument) As String
Dim dirName As String = IO.Path.GetDirectoryName(doc.FullFileName)
Dim fileNameWithoutExtension As String = IO.Path.GetFileNameWithoutExtension(doc.FullFileName)
Return String.Format("{0}\{1}.dxf", dirName, fileNameWithoutExtension)
End Function
Function Export(doc As PartDocument, newFileName As String)
Dim oCompDef As SheetMetalComponentDefinition = doc.ComponentDefinition
If oCompDef.HasFlatPattern = False Then
oCompDef.Unfold()
Else
oCompDef.FlatPattern.Edit()
End If
' more options can be found here:
' https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-54B44291-4E1D-4CDB-80CB-FBB38D0239C2
Dim sOut As String = "FLAT PATTERN DXF?AcadVersion=2000& "
sOut = sOut + "&BendUpLayerColor=255;0;0"
sOut = sOut + "&BendDownLayerColor=0;255;0"
sOut = sOut + "&InvisibleLayers=IV_TANGENT"
oCompDef.DataIO.WriteDataToFile(sOut, newFileName)
oCompDef.FlatPattern.ExitEdit()
End Function
Jelte de Jong
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If that document is being referenced by the assembly, it will not actually close anyways. If opened 'visibly', then closing it will just make it not visible anymore, but it will still remain open until the assembly that is referencing it is closed. You usually do not need to open each referenced document, because they are already open in the background. The exception is when all components referencing certain model documents have been suppressed. In that case, the document they reference can get 'unloaded' from session memory, for performance reasons. If you opened a document that is not being referenced by the assembly, then closing it would actually close it.
Wesley Crihfield
(Not an Autodesk Employee)
If you wanted to keep the Open() method in there, then you could just include the optional second input, which specifies whether to open it visibly or not visibly, and specify False, so they do not open visibly, then you would not have to close any document tabs. But as mentioned before, opening them is usually not needed. Each Document object has a ReadOnly Boolean property named Open, which will return True if it is already open, and False if the document has only been 'initialized' (not fully open yet, but will open if anything is done to it). The very definition of a Document tells us that it represents an 'in-memory' Inventor document. You can also check if a Document has been modified since it was last saved by checking its Document.Dirty property value. If True, then it has been modified since it was last saved, and you may want to update/save that document before exporting, depending on your needs.
And if you decide to include Revision Number into the exported file name, you should create a variable to hold the Revision Number value first, then set its value from the iProperty, then check the value of that variable, before trying to include it in the file name. If it has no value (empty String), then do not include it in the file name. Same goes for Part Number and other iProperty values.
Wesley Crihfield
(Not an Autodesk Employee)
Using the example code that @JelteDeJong provided above, I would create a 'shared' variable (declared between custom methods) just for the DXF's folder. Then set its value within the Sub Main area, while we have a direct reference to the main assembly. Then add the "\DXF's\" portion to the assembly's path, then make sure that directory exists. Then down within the CreateFileName Function, just use that variable when specifying the new full file name of the DXF file. Below is a modified version of that earlier code, with these changes.
Public Sub Main()
Dim doc As AssemblyDocument = ThisDoc.Document
sAsmDXFFolder = System.IO.Path.GetDirectoryName(doc.FullFileName)
sAsmDXFFolder = sAsmDXFFolder & "\DXF's"
If System.IO.Directory.Exists(sAsmDXFFolder) = False Then
System.IO.Directory.CreateDirectory(sAsmDXFFolder)
End If
For Each refDoc As Document In doc.AllReferencedDocuments
If (refDoc.DocumentType <> DocumentTypeEnum.kPartDocumentObject) Then Continue For
If (refDoc.SubType <> "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}") Then Continue For
Dim fileName = CreateFileName(refDoc)
Export(refDoc, fileName)
Next
doc.Activate()
End Sub
Dim sAsmDXFFolder As String
Function CreateFileName(doc As PartDocument) As String
Dim fileNameWithoutExtension As String = IO.Path.GetFileNameWithoutExtension(doc.FullFileName)
Return String.Format("{0}\{1}.dxf", sAsmDXFFolder, fileNameWithoutExtension)
End Function
Function Export(doc As PartDocument, newFileName As String)
Dim oCompDef As SheetMetalComponentDefinition = doc.ComponentDefinition
If oCompDef.HasFlatPattern = False Then
oCompDef.Unfold()
Else
oCompDef.FlatPattern.Edit()
End If
' more options can be found here:
' https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-54B44291-4E1D-4CDB-80CB-FBB38D0239C2
Dim sOut As String = "FLAT PATTERN DXF?AcadVersion=2000& "
sOut = sOut + "&BendUpLayerColor=255;0;0"
sOut = sOut + "&BendDownLayerColor=0;255;0"
sOut = sOut + "&InvisibleLayers=IV_TANGENT"
oCompDef.DataIO.WriteDataToFile(sOut, newFileName)
oCompDef.FlatPattern.ExitEdit()
End Function
Wesley Crihfield
(Not an Autodesk Employee)
Interesting....All was ok yesterday, but I went to run this today after closing down and restarting today, and now I get the following message. Only thing I did differently was installed Nesting 2024 to play around with it.
Hi @blandb. I am not 100% sure what caused that error, but what comes to mind is that the main assembly is the 'active' document, but then you are 'activating' the 'flat pattern edit mode' of one of the parts within the assembly, without first entering into 'component edit mode' for the component, and maybe that is where the problem originates from. In my opinion, you do not even need to enter into the 'edit mode' of the flat pattern. As long as the flat pattern exists, or it can be created using the 'unfold' method, then all you need to do is use the FlatPattern.DataIO instead of the SheetMetalComponentDefinition.DataIO object, without being in edit mode. That edit mode is just for user interactions.
Edit: Possibly, when you were opening them visibly, it was not a problem, but now that you are leaving them not visible, it does not like you trying to activate the edit mode on the flat pattern in a referenced part. Just my thoughts/suspicions.
Wesley Crihfield
(Not an Autodesk Employee)
