Save ALL associated files to DXF
Mike,
When I run the macro like I posted above, the macro runs... but I looked at the generated file using a text editor and it is creating dWf files rather than dXf files.
When I run the macro with the change like you recommend, I get this error "The parameter is incorrect".
Kirk
Accepted solution
Hi karthur1,
I'm short on time so did not test very much, but I think this will work for you. See the attached *.txt file if this code gives you Copy-Paste errors from this forum.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
'define the active document as an assembly file
Dim oAsmDoc As AssemblyDocument
oAsmDoc = ThisApplication.ActiveDocument
oAsmName = Left(oAsmDoc.DisplayName, Len(oAsmDoc.DisplayName) -4)
'check that the active document is an assembly file
If ThisApplication.ActiveDocument.DocumentType <> kAssemblyDocumentObject Then
MessageBox.Show("Please run this rule from the assembly file.", "iLogic")
Exit Sub
End If
'get user input
RUsure = MessageBox.Show ( _
"This will create a DXF file for all of the asembly components that have drawings files." _
& vbLf & "This rule expects that the drawing file shares the same name and location as the component." _
& vbLf & " " _
& vbLf & "Are you sure you want to create DXF Drawings for all of the assembly components?" _
& vbLf & "This could take a while.", "iLogic - Batch Output DXFs ",MessageBoxButtons.YesNo)
If RUsure = vbNo Then
Return
Else
End If
oPath = ThisDoc.Path
'get DXF target folder path
oFolder = oPath & "\" & oAsmName & " DXF Files"
'Check for the DXF folder and create it if it does not exist
If Not System.IO.Directory.Exists(oFolder) Then
System.IO.Directory.CreateDirectory(oFolder)
End If
'[ DXF setup
' Get the DXF translator Add-In.
Dim DXFAddIn As TranslatorAddIn
DXFAddIn = ThisApplication.ApplicationAddIns.ItemById("{C24E3AC4-122E-11D5-8E91-0010B541CD80}")
'Set a reference to the active document (the document to be published).
Dim oDocument As Document
oDocument = ThisApplication.ActiveEditDocument
Dim oContext As TranslationContext
oContext = ThisApplication.TransientObjects.CreateTranslationContext
oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
' Create a NameValueMap object
Dim oOptions As NameValueMap
oOptions = ThisApplication.TransientObjects.CreateNameValueMap
' Create a DataMedium object
Dim oDataMedium As DataMedium
oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
' Check whether the translator has 'SaveCopyAs' options
If DXFAddIn.HasSaveCopyAsOptions(oDocument, oContext, oOptions) Then
Dim strIniFile As String
strIniFile = "C:\temp\dxfout.ini"
' Create the name-value that specifies the ini file to use.
oOptions.Value("Export_Acad_IniFile") = strIniFile
End If
'] end of DXF setup
'[ ComponentDrawings
'look at the files referenced by the assembly
Dim oRefDocs As DocumentsEnumerator
oRefDocs = oAsmDoc.AllReferencedDocuments
Dim oRefDoc As Document
'work the the drawing files for the referenced models
'this expects that the model has a drawing of the same path and name
For Each oRefDoc In oRefDocs
idwPathName = Left(oRefDoc.FullDocumentName, Len(oRefDoc.FullDocumentName) - 3) & "idw"
'check to see that the model has a drawing of the same path and name
If(System.IO.File.Exists(idwPathName)) Then
Dim oDrawDoc As DrawingDocument
oDrawDoc = ThisApplication.Documents.Open(idwPathName, True)
oFileName = Left(oRefDoc.DisplayName, Len(oRefDoc.DisplayName) -3)
On Error Resume Next ' if DXF exists and is open or read only, resume next
'Set the DXF target file name
oDataMedium.FileName = oFolder & "\" & oFileName & "DXF"
'Write out the DXF
'Set the destination file name
oDataMedium.FileName = oFolder & "\" & oFileName & "dxf"
'Publish document.
Call DXFAddIn.SaveCopyAs(oDrawDoc, oContext, oOptions, oDataMedium)
'close the file
oDrawDoc.Close
Else
'If the model has no drawing of the same path and name - do nothing
End If
Next
'] End of ComponentDrawings
'[ Top Level Drawing
oAsmDrawing = ThisDoc.ChangeExtension(".idw")
oAsmDrawingDoc = ThisApplication.Documents.Open(oAsmDrawing, True)
oAsmDrawingName = Left(oAsmDrawingDoc.DisplayName, Len(oAsmDrawingDoc.DisplayName) -3)
'write out the DXF for the Top Level Assembly Drawing file
On Error Resume Next ' if DXF exists and is open or read only, resume next
'Set the DXF target file name
oDataMedium.FileName = oFolder & "\" & oAsmDrawingName & "dxf"
'Write out the DXF
Call DXFAddIn.SaveCopyAs(oAsmDrawingDoc, oContext, oOptions, oDataMedium)
'Close the top level drawing
oAsmDrawingDoc.Close
'] Top Level Drawing
MessageBox.Show("New Files Created in: " & vbLf & oFolder, "iLogic")
'open the folder where the new ffiles are saved
Shell("explorer.exe " & oFolder,vbNormalFocus)
Hi Curtis, thanks for your ruler but I would like to add the external line. I think so is the sheet scale-layout configuration before printing.
