Print ALL drawings related to an Assembly?

[Anonymous]

Is there a way (either thru Inventor or Vault) of print ALL idw (drawings) files related to an iam (assembly)?

Inventor (and Vault) are capable of creating and managing a BOM of the iam files and would think that it would be reltivly easy to query this bom and "find" all the associated idw files and batch print them. Possibly with the option to select the "levels" to dril down to (All, Top Level, Sub Assemblies within the iam, etc, etc)

Can anyone please help with this as I often have to print a "drawing package" for a complete build and doing this manually is very time consuming.

Thanking you in advance.

[ASI_Aaron]

Is the PDF Creator listed as a printer?  There should be options under the Printer Preferences to turn off Prompt for Filename.  You can then Apply that to the printer and when you create through the Task Scheduler, it shouldn't ask.

I'm only assuming here.  I use Adobe PDF to print and it has this option...

[Thomas.Kneidl]

Hi everybody,

thank you for your responses. I figured out that for my situation the be best way is to use Vault-->'Pack and Go' with attached files. By using 'Pack and Go' i can assure that i get the latest drawing version of every part. For PDF-creating i use the Autodesk Scheduling tool and set up a print job to PDF-Creator with 'Autosave' enabled.

So i am able to get about 200 drawings in pdf in like 15 minutes with just a few clicks.

[cameron]

Resurrecting old thread -

Trying out Porter, does nearly what we need, is there a solution that does the same but without an inventor install?

[ic198]

I tried to run this code as an External iLogic Rule and got most of the way through fixing the errors before I realised my mistake. Here is the (fixed) code if anyone would rather have it as an iLogic rule. I have also added the option to print more than one copy at a time.

Sub Main()

    Dim oAsmDoc As AssemblyDocument
    oAsmDoc = ThisApplication.ActiveDocument
    If ThisApplication.ActiveDocument.DocumentType <> kAssemblyDocumentObject Then
        MsgBox("This is NOT an assembly document!", vbExclamation)
        Exit Sub
    End If

	MsgBox("Any .idw files directly referencing " & oAsmDoc.FullFileName & " will not be printed. Print them manually", vbExclamation, "Assembly idw warning")
	MsgBox("Only idw files that exist on the local drive will be printed. Ensure all .idw files have been downloaded from Vault", vbExclamation, "Vault warning")

	Dim numCopies As Integer
	numCopies = InputBox("How many copies of each .idw?", "Copies", 1)

    Dim oPrintMgr As PrintManager
    oPrintMgr = ThisApplication.ActiveDocument.PrintManager
    If MsgBox("Using printer " & oPrintMgr.Printer & ", printing "& numCopies &" copy/s, A4 paper, landscape, B&W. Do you want to continue?", vbYesNo + vbQuestion, "Print Setup Summary") = vbNo Then
        Exit Sub
    End If

    Dim oDrgPrintMgr As DrawingPrintManager

    dirPath = Left(oAsmDoc.FullFileName, Len(oAsmDoc.FullFileName) - Len(oAsmDoc.DisplayName))

    Dim oRefDocs As DocumentsEnumerator
    oRefDocs = oAsmDoc.AllReferencedDocuments
    Dim oRefDoc As Document
    numFiles = 0

    For Each oRefDoc In oRefDocs
        idwPathName = Left(oRefDoc.FullDocumentName, Len(oRefDoc.FullDocumentName) -3) & "idw"
		Dim fileExists As Boolean
		If Dir(idwPathName) <> "" Then fileExists = True Else fileExists = False
        If fileExists Then
            numFiles = numFiles + 1
            Dim oDrawDoc As DrawingDocument
            oDrawDoc = ThisApplication.Documents.Open(idwPathName, True)
            oDrawDoc.Activate
            oDrawDoc = ThisApplication.ActiveDocument
            oDrgPrintMgr = oDrawDoc.PrintManager

            oDrgPrintMgr.AllColorsAsBlack = True
            oDrgPrintMgr.ScaleMode = kPrintBestFitScale
            oPrintMgr = ThisApplication.ActiveDocument.PrintManager

            ' Printer setup, default printer
            oPrintMgr.ColorMode = kPrintDefaultColorMode ' Set to default
	    oPrintMgr.PrintRange = kPrintAllSheets 'Prints all sheets in the idw
            oPrintMgr.NumberOfCopies = numCopies
            oPrintMgr.Orientation = kLandscapeOrientation ' Set to print using landscape orientation.
            oPrintMgr.PaperSize = kPaperSizeA4 'Set the paper size.
            oPrintMgr.SubmitPrint ' Submit the print.
            oDrawDoc.Close (True)
        End If
    Next
    MsgBox(numFiles & " idw files have been sent to the printer.",,"Print Summary")

End Sub 

[dg2405 · Accepted solution]

Here is some code which uses Vault to get all assembly-related drawings and print them. Some lines of the code are specific to our company and are not necessary:

AddReference "Autodesk.Connectivity.WebServices.dll"
Imports ACW = Autodesk.Connectivity.WebServices
AddReference "Autodesk.DataManagement.Client.Framework.Vault.dll"
AddReference "Autodesk.DataManagement.Client.Framework.dll"
Imports VDF = Autodesk.DataManagement.Client.Framework
AddReference "Connectivity.Application.VaultBase.dll"
Imports VB = Connectivity.Application.VaultBase
Public Class ThisRule

Dim idwcounter As Integer = 0

Sub Main()

Dim oApp As Inventor.Application = ThisApplication
Dim oAsmDoc As AssemblyDocument = ThisDoc.Document
Dim asmfullfilename As String = oAsmDoc.FullFileName
Dim asmfilename As String = RToBackSlash(oAsmDoc.FullFileName)

'Vault-Addin deaktivieren
Dim vaultAddin As ApplicationAddIn = oApp.ApplicationAddIns.ItemById("{48B682BC-42E6-4953-84C5-3D253B52E77B}")
Dim dsAddin As ApplicationAddIn = oApp.ApplicationAddIns.ItemById("{3AD251E3-02DD-4B8C-8882-86C97C80E00C}")
'iLogic Auto-Regeln deaktivieren
Try 'Wenn Datei nicht gefunden wird kommt sonst Fehler
	Rename("C:\Vault-Workspace\Preferences\ilogic Regeln\RulesOnEvents.xml", "C:\Vault-Workspace\Preferences\ilogic Regeln\RulesOnEvents_NotActive.xml")
Catch
End Try
vaultAddin.Deactivate()
dsAddin.Deactivate()

'Baugruppe schließen
oAsmDoc.Close(True)

'Alle Zeichnungen aus dem Vault abrufen
'Auf Vault-Connection zugreifen und ggf. rausgehen
Dim mVltCon As VDF.Vault.Currency.Connections.Connection = VB.ConnectionManager.Instance.Connection
If mVltCon Is Nothing Then Exit Sub
'Auf ACW-PropertyDefininition Status zugreifen
Dim filePropDefs As ACW.PropDef() = mVltCon.WebServiceManager.PropertyService.GetPropertyDefinitionsByEntityClassId("FILE")
Dim ACWNamePropDef As ACW.PropDef
For Each def As ACW.PropDef In filePropDefs
    If def.DispName = "Name" Then
        ACWNamePropDef = def
		Exit For
    End If
Next def  
'Suchoptionen festlegen
Dim namesucheoptionen As New ACW.SrchCond() With { _
	.PropDefId = ACWNamePropDef.Id, _
	.PropTyp = ACW.PropertySearchType.SingleProperty, _
	.SrchOper = 3, _
	.SrchRule = ACW.SearchRuleType.Must, _
	.SrchTxt = asmfilename _
}
Dim bookmark As String = String.Empty
Dim status As ACW.SrchStatus = Nothing
Dim results As ACW.File() = mVltCon.WebServiceManager.DocumentService.FindFilesBySearchConditions(New ACW.SrchCond() {namesucheoptionen}, Nothing, Nothing, False, True, bookmark, status)
Dim oFileIteration As VDF.Vault.Currency.Entities.FileIteration = New VDF.Vault.Currency.Entities.FileIteration(mVltCon, results(0))
Dim settings As New VDF.Vault.Settings.AcquireFilesSettings(mVltCon)
settings.OptionsRelationshipGathering.FileRelationshipSettings.IncludeChildren = True
settings.OptionsRelationshipGathering.FileRelationshipSettings.RecurseChildren = True
settings.OptionsRelationshipGathering.FileRelationshipSettings.IncludeRelatedDocumentation = True
settings.OptionsRelationshipGathering.FileRelationshipSettings.VersionGatheringOption = VDF.Vault.Currency.VersionGatheringOption.Latest
settings.AddFileToAcquire(oFileIteration, VDF.Vault.Settings.AcquireFilesSettings.AcquisitionOption.Download)
Dim aquiresults As VDF.Vault.Results.AcquireFilesResults = mVltCon.FileManager.AcquireFiles(settings)

'AsmDoc wieder öffnen
oAsmDoc = oApp.Documents.Open(asmfullfilename,False)

'Alle heruntergeladenen idw's in Liste
Dim idwList As New ArrayList
For Each aquiresult As VDF.Vault.Results.FileAcquisitionResult In aquiresults.FileResults
	Dim aquiresultpath As String = aquiresult.LocalPath.FullPath
	If UCase(aquiresultpath).Contains(".IDW") Then
		If Right(UCase(LWoPoint(aquiresultpath)), 2) = "-Z" _
		Or IsNumeric(Right(LWoPoint(aquiresultpath), 2)) = True Then
			idwList.Add(aquiresultpath)
		End If
	End If
Next

'Vars definieren von BOM
Dim oBOM As BOM = oAsmDoc.ComponentDefinition.BOM
Dim oBOMView As BOMView = oBOM.BOMViews("Nur Bauteile")
If oBOMView.BOMRows.Count = 0 Then Exit Sub
Dim oDrwDoc As DrawingDocument
'Zusammenbauzeichnung drucken
For Each idw As String In idwList
	If idw.Contains(RPointToBackSlash(oAsmDoc.FullFileName)) Then
		idwcounter = idwcounter + 1
		oDrwDoc = oApp.Documents.Open(idw, True)
		Print(oDrwDoc, True)
		oDrwDoc.Close(True)
	End If
Next
'Alle Zeichnungen der Einzelteile drucken
GoThruEachBom(oBOMView, idwList)

'AutoRegeln wieder aktivieren
Rename("C:\Vault-Workspace\Preferences\ilogic Regeln\RulesOnEvents_NotActive.xml", "C:\Vault-Workspace\Preferences\ilogic Regeln\RulesOnEvents.xml")

'AsmDoc schließen
oAsmDoc.Close(True)

MessageBox.Show("Es wurden " & idwcounter & " Zeichnungen gedruckt." & vbCrLf & "Wenn Inventor anschließend wieder normal genutzt werden soll, bitte den Inventor schließen und erneut öffnen. Anschließend sind das Vauld- u. DS-Addin wieder geladen.", "Title")

End Sub

Function RToBackSlash(ByVal strText As String) As String
    RToBackSlash = Right(strText, Len(strText) - InStrRev(strText, "\"))
End Function

Function RPointToBackSlash(ByVal strText As String) As String
    strText = Left(strText, InStrRev(strText, ".") - 1)
    RPointToBackSlash = Right(strText, Len(strText) - InStrRev(strText, "\"))
End Function

Function LWoPoint(ByVal strText As String) As String
    LWoPoint = Left(strText, InStrRev(strText, ".")-1)
End Function

Function GoThruEachBom(oBomView As BOMView, idwList As ArrayList)
For Each oBomRow As BOMRow In oBomView.BOMRows
	Dim oRowDoc As Document = oBomRow.ComponentDefinitions(1).Document
	Dim filename As String = RPointToBackSlash(oRowDoc.FullFileName)
	For Each idw As String In idwList
		If idw.Contains(filename) Then
			idwcounter = idwcounter + 1
			Dim oDrwDoc As DrawingDocument = ThisApplication.Documents.Open(idw, True)
			Dim bezeichnung As String = UCase(oDrwDoc.PropertySets("Design Tracking Properties")("Description").Value)
			If bezeichnung.Contains("TISCHPLATTE") _
			Or bezeichnung.Contains("GRUNDKÖRPER") _
			Or bezeichnung.Contains("DICHTPLATTE") _
			Or bezeichnung.Contains("GESTELL") _
			Or bezeichnung.Contains("GRUNDPLATTE") Then
				System.Threading.Thread.CurrentThread.Sleep(500)
				Print(oDrwDoc, True)
			Else
				System.Threading.Thread.CurrentThread.Sleep(500)
				Print(oDrwDoc, False)
			End If
			oDrwDoc.Close(True)
		End If
	Next
	If TypeOf oRowDoc Is AssemblyDocument Then
		If oBomRow.ComponentDefinitions(1).BOMStructure = BOMStructureEnum.kPurchasedBOMStructure Then
			GoThruEachBom(oRowDoc.ComponentDefinitions(1).BOM.BOMViews("Nur Bauteile"), idwList)
		End If
	End If
Next
End Function

Function Print(oDrwDoc As DrawingDocument, printAsA2 As Boolean)
Dim oApp As Inventor.Application = ThisApplication
oDrwDoc.MakeAllViewsPrecise
oApp.CommandManager.ControlDefinitions.Item("DrawingUpdateAllSheetsCmd").Execute2(True)
Dim oDrwPrintMgr As DrawingPrintManager = oDrwDoc.PrintManager
oDrwPrintMgr.ColorMode = PrintColorModeEnum.kPrintColorPalette
oDrwPrintMgr.PrintRange = PrintRangeEnum.kPrintAllSheets
Dim oSheetSize As DrawingSheetSizeEnum = oDrwDoc.Sheets(1).Size
If oSheetSize = DrawingSheetSizeEnum.kA4DrawingSheetSize Then
	oDrwPrintMgr.ScaleMode = PrintScaleModeEnum.kPrintFullScale
	oDrwPrintMgr.Orientation = PrintOrientationEnum.kPortraitOrientation
	oDrwPrintMgr.Printer = "\\KMSSRV10\Kopierer_Konstruktion _A4_Farbe"
	oDrwPrintMgr.PaperSize = PaperSizeEnum.kPaperSizeA4
End If
If oSheetSize = DrawingSheetSizeEnum.kA3DrawingSheetSize Then
	oDrwPrintMgr.ScaleMode = PrintScaleModeEnum.kPrintBestFitScale
	oDrwPrintMgr.Orientation = PrintOrientationEnum.kLandscapeOrientation
	oDrwPrintMgr.Printer = "\\KMSSRV10\Kopierer_Konstruktion _A4_Farbe"
	oDrwPrintMgr.PaperSize = PaperSizeEnum.kPaperSizeA4
End If
If oSheetSize = DrawingSheetSizeEnum.kA2DrawingSheetSize Then
	oDrwPrintMgr.ScaleMode = PrintScaleModeEnum.kPrintBestFitScale
	oDrwPrintMgr.Orientation = PrintOrientationEnum.kLandscapeOrientation
	oDrwPrintMgr.Printer = "\\KMSSRV10\Kopierer_Konstruktion _A3_Farbe"
	oDrwPrintMgr.PaperSize = PaperSizeEnum.kPaperSizeA3
End If
If oSheetSize = DrawingSheetSizeEnum.kA1DrawingSheetSize Then
	oDrwPrintMgr.ScaleMode = PrintScaleModeEnum.kPrintBestFitScale
	oDrwPrintMgr.Orientation = PrintOrientationEnum.kLandscapeOrientation
	oDrwPrintMgr.Printer = "\\KMSSRV10\Kopierer_Konstruktion _A3_Farbe"
	oDrwPrintMgr.PaperSize = PaperSizeEnum.kPaperSizeA3
End If
If oSheetSize = DrawingSheetSizeEnum.kA0DrawingSheetSize Then
	oDrwPrintMgr.ScaleMode = PrintScaleModeEnum.kPrintBestFitScale
	oDrwPrintMgr.Orientation = PrintOrientationEnum.kLandscapeOrientation
	oDrwPrintMgr.Printer = "\\KMSSRV10\Kopierer_Konstruktion _A3_Farbe"
	oDrwPrintMgr.PaperSize = PaperSizeEnum.kPaperSizeA3
End If
If (oSheetSize = DrawingSheetSizeEnum.kA1DrawingSheetSize _
	 Or oSheetSize = DrawingSheetSizeEnum.kA0DrawingSheetSize) _
	 And printAsA2 = True Then
	oDrwPrintMgr.ScaleMode = PrintScaleModeEnum.kPrintBestFitScale
	oDrwPrintMgr.Orientation = PrintOrientationEnum.kLandscapeOrientation
	oDrwPrintMgr.Printer = "\\KMSSRV10\HP DesignJet T1530 HPGL2 A2"
	'oDrwPrintMgr.PaperSize = PaperSizeEnum.kPaperSizeA2 'Führt zu Error, warum? Geht auch ohne...
End If

'Logger.Info("Zeichnungsgröße: " & oSheetSize.ToString & "|Druckgröße: " & oDrwPrintMgr.PaperSize.ToString & oDrwPrintMgr.Printer, "dsds")

oDrwPrintMgr.SubmitPrint
End Function

End Class

[matthew.zelei-good]

Hi! I tried to use this code for myself to print all drawings for a file but got an error:
"Error in rule: Print All Drawings, in document: Q13605 06 00 Release.iam

Unspecified error (Exception from HRESULT: 0x80004005 (E_FAIL))"

In the 'More Info' tab:

"System.Runtime.InteropServices.COMException (0x80004005): Unspecified error (Exception from HRESULT: 0x80004005 (E_FAIL))
at System.RuntimeType.ForwardCallToInvokeMember(String memberName, BindingFlags flags, Object target, Int32[] aWrapperTypes, MessageData& msgData)
at Inventor.ApplicationAddIns.get_ItemById(String ClientId)
at ThisRule.Main()
at Autodesk.iLogic.Exec.AppDomExec.ExecRuleInAssembly(Assembly assem)
at iLogic.RuleEvalContainer.ExecRuleEval(String execRule)"

Do you have any idea what is the cause of the error? I'm literally starting out with iLogic, and I'm getting bogged down with doing my normal work and trying to interrogate the code and find the issue!

Why does it disable the vault add in? Does it need to know the location of the specific printer it will be printed on, i.e. I can't run the code and then choose which printer to run on? All of our drawings are .dwg rather than .idw, I've replaced all in the code, but still getting the same error.

TIA!!!

[johnsonshiue]

Hi! Do you have Vault running? Also, the folder paths and file names may need to be changed.

Many thanks!

[dg2405]

I think he's stopping at deactivating the addins vault and datastandard. If you don't have datastandard remove the line. You can also completly run the code without deaktivating the addins. It's only for supreesing the update messages while open the drawings if they're not up to date.

[dg2405]

Also you don't need this code, it's for deactivating auto iLogic rules.

Try 'Wenn Datei nicht gefunden wird kommt sonst Fehler
	Rename("C:\Vault-Workspace\Preferences\ilogic Regeln\RulesOnEvents.xml", "C:\Vault-Workspace\Preferences\ilogic Regeln\RulesOnEvents_NotActive.xml")
Catch
End Try

:

[matthew.zelei-good]

This is fantastic, a great help to going to Vault and selecting drawings individually and printing! Is there a way to give the option to be able to choose A4 or A3 in a pop up?

Thanks,

MG