You'd like to output a PDF file from the drawings of all the components found in an assembly file (if those components have a drawing file created), and you like also create a PDF of the top level assembly drawing as well. All of these PDFs should be written out to a single folder. Can this be done?
Here's an ilogic rule to batch output PDF files for each component in an assembly. This rule assumes that the component drawings share the same name and location of the component.
For example: C:\Temp\widget-450.ipt has a drawing: C:\Temp\widget-450.idw
If the drawing file is not found, then it simply moves on and looks at the next component.
This rule may not work for everyone, but it should provide a starting point from which it can be modified as needed. If you work with *.dwg files rather than *.idw files you can search and replace this code for idw and replace with dwg.
Here is the code in a *.txt file that can be downloaded as well:
http://forums.autodesk.com/autodesk/attachments/autodesk/78/455124/2/Batch%20PDFs.txt
'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 PDF
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 PDF Drawings for all of the assembly components?" _
& vblf & "This could take a
while.", "iLogic
- Batch Output PDFs ",MessageBoxButtons.YesNo)
If RUsure = vbNo Then
Return
Else
End If
'- - - - - - - - - - - - -PDF
setup - - - - - - - - - - - -
oPath = ThisDoc.Path
PDFAddIn = ThisApplication.ApplicationAddIns.ItemById("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}")
oContext = ThisApplication.TransientObjects.CreateTranslationContext
oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
oOptions = ThisApplication.TransientObjects.CreateNameValueMap
oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
If PDFAddIn.HasSaveCopyAsOptions(oDataMedium, oContext, oOptions) Then
'oOptions.Value("All_Color_AS_Black")
= 0
oOptions.Value("Remove_Line_Weights") = 1
oOptions.Value("Vector_Resolution") = 400
oOptions.Value("Sheet_Range") = Inventor.PrintRangeEnum.kPrintAllSheets
'oOptions.Value("Custom_Begin_Sheet")
= 2
'oOptions.Value("Custom_End_Sheet")
= 4
End If
'get PDF target folder path
oFolder = oPath & "\" & oAsmName & " PDF Files"
'Check for the PDF folder and
create it if it does not exist
If Not System.IO.Directory.Exists(oFolder) Then
System.IO.Directory.CreateDirectory(oFolder)
End If
'- - - - - - - - - - - - -
'- - - - - - - - - - - -
-Component Drawings - - - - - - - - - - - -
'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 PDF exists and is open or
read only, resume next
'Set the PDF
target file name
oDataMedium.FileName = oFolder & "\" & oFileName & "pdf"
'Write out the PDF
Call PDFAddIn.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
'- - - - - - - - - - - - -
'- - - - - - - - - - - - -Top
Level Drawing - - - - - - - - - - - -
oAsmDrawing = ThisDoc.ChangeExtension(".idw")
oAsmDrawingDoc = ThisApplication.Documents.Open(oAsmDrawing, True)
oAsmDrawingName = Left(oAsmDrawingDoc.DisplayName, Len(oAsmDrawingDoc.DisplayName) -3)
'write out the PDF for the Top
Level Assembly Drawing file
On error Resume Next ' if PDF exists and is open or
read only, resume next
'Set the PDF target file name
oDataMedium.FileName = oFolder & "\" & oAsmDrawingName & "pdf"
'Write out the PDF
Call PDFAddIn.SaveCopyAs(oAsmDrawingDoc, oContext, oOptions, oDataMedium)
'Close the top level drawing
oAsmDrawingDoc.Close
'- - - - - - - - - - - - -
MessageBox.Show("New Files Created in:
" & vblf & oFolder, "iLogic")
'open the folder where the new
ffiles are saved
Shell("explorer.exe " & oFolder,vbNormalFocus)
