topic Re: iLogic to Batch Export PDF and DXF in Inventor Programming Forum

iLogic to Batch Export PDF and DXF

esaldana — Fri, 04 Jun 2021 13:03:37 GMT

Good morning everyone,

I found this great code (shown below) at: AutoDesk Inventor - Batch Exporting PDFs & DXFs with iLogic - Thingimajigs,

Is really good, and saving me a lot of time when exporting,

the question I have is if there is a way to export only the profile of my parts when exporting to DXF's and not the whole title block and dimensions? any suggestions are welcome.

Thanks you,

code:

Sub Main()
  Dim myDate As String = Now().ToString("yyyy-MM-dd HHmmss")
  myDate = myDate.Replace(":","")  ' & " - " & TypeString
 userChoice = InputRadioBox("Defined the scope", "This Document", "All Open Documents", True, Title := "Defined the scope")
 UserSelectedActionList = New String(){"DXF & PDF", "PDF Only", "DXF Only"}
  UserSelectedAction = InputListBox("What action must be performed with selected views?", _
          UserSelectedActionList, UserSelectedActionList(0), Title := "Action to Perform", ListName := "Options")
      Select UserSelectedAction
   Case "DXF & PDF": UserSelectedAction = 3
   Case "PDF Only": UserSelectedAction = 1
   Case "DXF Only":    UserSelectedAction = 2
   End Select
 If userChoice Then
   Call MakePDFFromDoc(ThisApplication.ActiveDocument, myDate, UserSelectedAction)
  Else
   For Each oDoc In ThisApplication.Documents
    If oDoc.DocumentType = kDrawingDocumentObject
     Try
      If Len(oDoc.File.FullFileName)>0 Then
       Call MakePDFFromDoc(oDoc, myDate, UserSelectedAction)
      End If
     Catch
     End Try
    End If
   Next
  End If
 End Sub
 Sub MakePDFFromDoc(ByRef oDocument As Document, DateString As String, UserSelectedAction As Integer)
 ' oPath = oDocument.Path
 ' oFileName = oDocument.FileName(False) 'without extension
  'oDocument = ThisApplication.ActiveDocument
  oPDFAddIn = ThisApplication.ApplicationAddIns.ItemById _
  ("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}")
  oContext = ThisApplication.TransientObjects.CreateTranslationContext
  oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism
  oOptions = ThisApplication.TransientObjects.CreateNameValueMap
  oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
 oFullFileName = oDocument.File.FullFileName
  oPath = Left(oFullFileName, InStrRev(oFullFileName, "\")-1)
  oFileName = Right(oFullFileName, Len(oFullFileName)-InStrRev(oFullFileName, "\"))
  oFilePart = Left(oFileName, InStrRev(oFileName, ".")-1)
 'oRevNum = oDocument.iProperties.Value("Project", "Revision Number")
  'oDocument = ThisApplication.ActiveDocument
 ' If oPDFAddIn.HasSaveCopyAsOptions(oDataMedium, oContext, oOptions) Then
  oOptions.Value("All_Color_AS_Black") = 0
  oOptions.Value("Remove_Line_Weights") = 0
  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 = Left(oPath, InStrRev(oPath, "\")) & "PDF"
  oFolder = oPath & "\iLogic PDF's (" & DateString & ")"
 '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
 'Set the PDF target file name
  oDataMedium.FileName = oFolder & "\" & oFilePart & ".pdf"
 'Publish document
  If (UserSelectedAction = 1) Or (UserSelectedAction = 3) Then
   oPDFAddIn.SaveCopyAs(oDocument, oContext, oOptions, oDataMedium)'For PDF's
  End If
  If (UserSelectedAction = 2) Or (UserSelectedAction = 3) Then
   oDocument.SaveAs(oFolder & "\" & oFilePart & ".dxf", True) 'For DXF's
  End If
  'oDocument.SaveAs(oFolder & "\" & ThisDoc.ChangeExtension(".dxf"), True) 'For DXF's
  '------end of iLogic-------
 End Sub

Re: iLogic to Batch Export PDF and DXF

Curtis_Waguespack — Fri, 04 Jun 2021 14:15:51 GMT

Hi @esaldana

You can turn off the layers of the objects you don't want to include and then do the export, then turn the layers back on.

Here is a PDF export example that demonstrates this.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

oPath = ThisDoc.Path oFileName = ThisDoc.FileName(False) 'without extension oPDFAddIn = ThisApplication.ApplicationAddIns.ItemById _ ("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}") oContext = ThisApplication.TransientObjects.CreateTranslationContext oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism oOptions = ThisApplication.TransientObjects.CreateNameValueMap oDataMedium = ThisApplication.TransientObjects.CreateDataMedium oOptions.Value("All_Color_AS_Black") = 0 oOptions.Value("Remove_Line_Weights") = 0 oOptions.Value("Vector_Resolution") = 400 oOptions.Value("Sheet_Range") = Inventor.PrintRangeEnum.kPrintAllSheets 'get PDF target folder path oFolder = Left(oPath, InStrRev(oPath, "\")) & "PDF" 'add layers to collection Dim oCollection As ObjectCollection oCollection = ThisApplication.TransientObjects.CreateObjectCollection oLayers = ThisApplication.ActiveDocument.StylesManager.Layers oCollection.Add(oLayers(("Title (ANSI)"))) oCollection.Add(oLayers(("Border (ANSI)"))) oCollection.Add(oLayers(("Dimension (ANSI)"))) 'turn layers off For Each oLayer In oCollection oLayer.visible = False Next ThisApplication.ActiveView.Update() '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 'Set the PDF target file name oDataMedium.FileName = oFolder & "\" & oFileName & ".pdf" oPDFAddIn.SaveCopyAs(ThisApplication.ActiveDocument, oContext, oOptions, oDataMedium)'For PDF's MessageBox.Show("PDF saved to: " & oFolder, "iLogic") Process.Start(oFolder) 'turn layers back on For Each oLayer In oCollection oLayer.visible = True Next

Re: iLogic to Batch Export PDF and DXF

esaldana — Fri, 04 Jun 2021 14:57:43 GMT

Thank you Curtis,

I applied the section of the layers on/off to the existing code and it works really well,

Not to be too demanding this morning, but is there any way to instead of cancelling the layers that I don't want, just export to dxf the flatten portion , I'm using exclusively sheet metal and all that I always need is the flat pattern to be either lasered or punched. Usually I used the export from the actual sheet metal part but that way I have to go one by one, while this code is batching from the drawings which is nice.

thanks for you help,

Eric

Re: iLogic to Batch Export PDF and DXF

Curtis_Waguespack — Fri, 04 Jun 2021 15:08:41 GMT

Hi @esaldana ,

So you want to run the rule from the assembly file and export DXFs for all sheet metal part flat patterns?

Or you want to run the rule from a drawing file of the assembly and export DXFs for all sheet metal part flat patterns?

Or you want to run the rule from drawing file that contains views of multiple flat patterns and export DXFs for all sheet metal part flat patterns?

Re: iLogic to Batch Export PDF and DXF

esaldana — Fri, 04 Jun 2021 15:26:11 GMT

Hi @Curtis_Waguespack ,

really appreciate your attention to this message,

Wherever is the easiest, I will always have a single file (DWG) with several sheets (assembly drawing firs, then the sub-assemblies and finally all the parts) and need to create a single PDF with all those sheets included, finally I need to create DXFs' for all the parts having a flat pattern on them.

What do you suggest me? It could be from either the top assembly or top drawing.

Honestly what I liked it from that original code was being able to select from either export only PDF or DXF or both and also the creation of folder with time stamp, so I could know my latest output.

But it can be different as soon it accomplish the tasks.

Thank you,

Eric

Re: iLogic to Batch Export PDF and DXF

Curtis_Waguespack — Fri, 04 Jun 2021 17:47:34 GMT

Hi @esaldana

I would run this from the top level drawing, but you can run it from the top level assembly...

if you run it from the assembly, you get a PDF of the assembly, which I'm not sure sure is useful...

This runs through all the referenced files and DXFs out the sheet metal flat patterns... if there is no flat pattern it will create it, so you might see the model open and close in that case.

I just set it to output to a temp folder, but you can set the folder as needed... there are a few examples commented out for this also.

Post back if it's not exactly what you're after, it can likely be tweaked to be what you're after.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Sub Main() Dim myDate As String = Now().ToString("yyyy-MM-dd HH:mm:ss") myDate = myDate.Replace(":", ".") 'change this as needed oRoot = "C:\Temp\" ' oRoot = ThisDoc.Path 'use the document's containing folder path 'change this as needed oSuffix = "Outputs" 'oSuffix = iProperties.Value("Project", "Project") 'use the document's Project# 'oSuffix = iProperties.Value("Project", "Part Number") 'use the document's Part# 'get target folder path oFolder = oRoot & "\" & oSuffix & " (" & myDate & ")" '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 'open the folder Process.Start(oFolder) Dim oDoc As Document oDoc = ThisApplication.ActiveDocument 'PDF of the file you're running it this from Call PDF_Out(oDoc, oFolder) 'Loop through all referenced documents j= 1 For Each oDoc In ThisApplication.ActiveDocument.AllReferencedDocuments oName = oDoc.DisplayName ck = j Mod 2 If ck = 0 Then oFlicker = ".......... " Else oFlicker = ".... " End If ThisApplication.StatusBarText = "Processing DXF" & oFlicker & oName j = j + 1 'created DXF's of sheetmetal parts Call DXF_Out(oDoc, oFolder) Next ThisApplication.StatusBarText = "Done!!!!!" End Sub Sub DXF_Out(ByRef oDoc As Document, oFolder As String) oFullFileName = oDoc.FullFileName oFileName = Right(oFullFileName, Len(oFullFileName) - InStrRev(oFullFileName, "\")) oName = Left(oFileName, InStrRev(oFileName, ".") - 1) 'name without extension 'look at only Sheet metal parts If oDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then Dim oCompDef As SheetMetalComponentDefinition oCompDef = oDoc.ComponentDefinition i = 0 For Each oBody In oCompDef.SurfaceBodies If oBody.IsSolid = True Then i = i +1 End If Next If i > 1 Then Exit Sub End If 'check for flat pattern If oCompDef.HasFlatPattern = False Then oCompDef.Unfold oCreated_Flat = True Else 'if flat pattern exists oCompDef.FlatPattern.Edit End If sOut = "FLAT PATTERN DXF?AcadVersion=2000&OuterProfileLayer=IV_INTERIOR_PROFILES" sFullDXFname = oFolder & "\" & oName & ".dxf" 'Output the DXF oCompDef.DataIO.WriteDataToFile(sOut, sFullDXFname) oCompDef.FlatPattern.ExitEdit Try If oCreated_Flat = True Then oDoc.Save Catch End Try oDoc.Close End If End Sub Sub PDF_Out(ByRef oDocument As Document, oFolder As String) ThisApplication.StatusBarText = "Processing PDF.........." & oDocument.displayname oFullFileName = oDocument.FullFilename oFileName = Right(oFullFileName, Len(oFullFileName) - InStrRev(oFullFileName, "\")) oName = Left(oFileName, InStrRev(oFileName, ".") -1) 'name without extension sFullPDFname = oFolder & "\" & oName & ".pdf" oPDFAddIn = ThisApplication.ApplicationAddIns.ItemById _ ("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}") oContext = ThisApplication.TransientObjects.CreateTranslationContext oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism oOptions = ThisApplication.TransientObjects.CreateNameValueMap oDataMedium = ThisApplication.TransientObjects.CreateDataMedium oOptions.Value("All_Color_AS_Black") = 0 oOptions.Value("Remove_Line_Weights") = 0 oOptions.Value("Vector_Resolution") = 400 oOptions.Value("Sheet_Range") = Inventor.PrintRangeEnum.kPrintAllSheets 'Set the PDF target file name oDataMedium.FileName = sFullPDFname 'output the PDF oPDFAddIn.SaveCopyAs(oDocument, oContext, oOptions, oDataMedium) End Sub

Re: iLogic to Batch Export PDF and DXF

esaldana — Fri, 04 Jun 2021 17:57:49 GMT

Hi @Curtis_Waguespack ,

The PDF goes really well and fast,

but is the only file in that temp folder,

I have the following error message:

I have absolutely no idea of the error meaning,

Do you see something there?

Thank you Curtis,

Re: iLogic to Batch Export PDF and DXF

Curtis_Waguespack — Fri, 04 Jun 2021 18:43:43 GMT

Hi @esaldana

I just ran this on one of Autodesk's sample assemblies and the DXF part hit an error with that assembly in trying to access the sheet metal part files... so I added a missing line to open the files... it was probably accessing files in Inventor's memory when I ran this earlier.... so the error didn't happen...

Give this a try and see if that resolved it.

If not, What version of Inventor are you using?.... and can you provide a simple file set that demonstrates the problem, to test?

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Sub Main() Dim myDate As String = Now().ToString("yyyy-MM-dd HH:mm:ss") myDate = myDate.Replace(":", ".") 'change this as needed oRoot = "C:\Temp" 'oRoot = ThisDoc.Path 'use the document's containing folder path 'change this as needed oSuffix = "Outputs" 'oSuffix = iProperties.Value("Project", "Project") 'use the document's Project# 'oSuffix = iProperties.Value("Project", "Part Number") 'use the document's Part# 'get target folder path oFolder = oRoot & "\" & oSuffix & " (" & myDate & ")" '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 'open the folder Process.Start(oFolder) Dim oDoc As Document oDoc = ThisApplication.ActiveDocument 'PDF of the file you're running it this from Call PDF_Out(oDoc, oFolder) 'Loop through all referenced documents j= 1 For Each oDoc In ThisApplication.ActiveDocument.AllReferencedDocuments oName = oDoc.DisplayName ck = j Mod 2 If ck = 0 Then oFlicker = ".......... " Else oFlicker = ".... " End If ThisApplication.StatusBarText = "Processing DXF" & oFlicker & oName j = j + 1 'created DXF's of sheetmetal parts Call DXF_Out(oDoc, oFolder) Next ThisApplication.StatusBarText = "Done!!!!!" End Sub Sub DXF_Out(ByRef oDoc As Document, oFolder As String) oCreated_Flat = False oFullFileName = oDoc.FullFileName oFileName = Right(oFullFileName, Len(oFullFileName) - InStrRev(oFullFileName, "\")) oName = Left(oFileName, InStrRev(oFileName, ".") - 1) 'name without extension Logger.Info("oName: " & oName) 'look at only Sheet metal parts If oDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then Logger.Info("Is Sheetmetal") Dim oCompDef As SheetMetalComponentDefinition oCompDef = oDoc.ComponentDefinition i = 0 For Each oBody In oCompDef.SurfaceBodies If oBody.IsSolid = True Then i = i +1 End If Next If i > 1 Then Exit Sub End If 'check for flat pattern If oCompDef.HasFlatPattern = False Then Logger.Info("HasFlatPattern: " & HasFlatPattern) oCompDef.Unfold oCreated_Flat = True Else 'if flat pattern exists Logger.Info("Trying to get flatpattern...") ThisApplication.Documents.Open(oFullFileName, True) oCompDef.FlatPattern.Edit End If sOut = "FLAT PATTERN DXF?AcadVersion=2000&OuterProfileLayer=IV_INTERIOR_PROFILES" sFullDXFname = oFolder & "\" & oName & ".dxf" Logger.Info("sFullDXFname: " & sFullDXFname) 'Output the DXF oCompDef.DataIO.WriteDataToFile(sOut, sFullDXFname) oCompDef.FlatPattern.ExitEdit Try If oCreated_Flat = True Then oDoc.Save Catch End Try oDoc.Close End If End Sub Sub PDF_Out(ByRef oDocument As Document, oFolder As String) ThisApplication.StatusBarText = "Processing PDF.........." & oDocument.displayname oFullFileName = oDocument.FullFilename oFileName = Right(oFullFileName, Len(oFullFileName) - InStrRev(oFullFileName, "\")) oName = Left(oFileName, InStrRev(oFileName, ".") -1) 'name without extension sFullPDFname = oFolder & "\" & oName & ".pdf" oPDFAddIn = ThisApplication.ApplicationAddIns.ItemById _ ("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}") oContext = ThisApplication.TransientObjects.CreateTranslationContext oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism oOptions = ThisApplication.TransientObjects.CreateNameValueMap oDataMedium = ThisApplication.TransientObjects.CreateDataMedium oOptions.Value("All_Color_AS_Black") = 0 oOptions.Value("Remove_Line_Weights") = 0 oOptions.Value("Vector_Resolution") = 400 oOptions.Value("Sheet_Range") = Inventor.PrintRangeEnum.kPrintAllSheets 'Set the PDF target file name oDataMedium.FileName = sFullPDFname 'output the PDF oPDFAddIn.SaveCopyAs(oDocument, oContext, oOptions, oDataMedium) End Sub

Re: iLogic to Batch Export PDF and DXF

esaldana — Fri, 04 Jun 2021 18:55:54 GMT

Hi @Curtis_Waguespack ,

so close.

This time one of the DXF's was created (the 3rd one in the drawing, see attached PDF), but not the others, got an error message after creating the first DXF.

I'm using Inventor 2020

Thank you Curtis,

Re: iLogic to Batch Export PDF and DXF

Curtis_Waguespack — Fri, 04 Jun 2021 19:14:55 GMT

Hi @esaldana

Note sure what the issue is, but I added some debugging and error catching to this version, so maybe you can figure out what it's tripping on...

Go to the View tab , User Interface button/pulldown, and check the iLogic Log option, they you can watch the log and see if you can tell what the issue is with the part file.

If not, I'd need to have the files to test, if you can share them, you can zip them and attach them here.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Sub Main() Dim myDate As String = Now().ToString("yyyy-MM-dd HH:mm:ss") myDate = myDate.Replace(":", ".") 'change this as needed oRoot = "C:\Temp" 'oRoot = ThisDoc.Path 'use the document's containing folder path 'change this as needed oSuffix = "Outputs" 'oSuffix = iProperties.Value("Project", "Project") 'use the document's Project# 'oSuffix = iProperties.Value("Project", "Part Number") 'use the document's Part# 'get target folder path oFolder = oRoot & "\" & oSuffix & " (" & myDate & ")" '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 'open the folder Process.Start(oFolder) Dim oDoc As Document oDoc = ThisApplication.ActiveDocument 'PDF of the file you're running it this from Call PDF_Out(oDoc, oFolder) 'Loop through all referenced documents j= 1 For Each oDoc In ThisApplication.ActiveDocument.AllReferencedDocuments oName = oDoc.DisplayName ck = j Mod 2 If ck = 0 Then oFlicker = ".......... " Else oFlicker = ".... " End If ThisApplication.StatusBarText = "Processing DXF" & oFlicker & oName j = j + 1 'created DXF's of sheetmetal parts Call DXF_Out(oDoc, oFolder) Next ThisApplication.StatusBarText = "Done!!!!!" End Sub Sub DXF_Out(ByRef oDoc As Document, oFolder As String) oCreated_Flat = False oFullFileName = oDoc.FullFileName oFileName = Right(oFullFileName, Len(oFullFileName) - InStrRev(oFullFileName, "\")) oName = Left(oFileName, InStrRev(oFileName, ".") - 1) 'name without extension 'look at only Sheet metal parts If oDoc.SubType = "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then Logger.Info("File Name: " & oFileName) Logger.Info("Is Sheetmetal") Dim oCompDef As SheetMetalComponentDefinition oCompDef = oDoc.ComponentDefinition i = 0 Logger.Info("Looking at solid bodies....") For Each oBody In oCompDef.SurfaceBodies If oBody.IsSolid = True Then i = i +1 End If Next If i > 1 Then Exit Sub End If Logger.Info(".....solid bodies ok") 'check for flat pattern If oCompDef.HasFlatPattern = False Then Logger.Info("HasFlatPattern: " & oCompDef.HasFlatPattern) Logger.Info("/////////////\\\\\\\\\\\\ Trying to create flatpattern...") Try oCompDef.Unfold oCreated_Flat = True Catch ex As Exception oCreated_Flat = False Logger.Info("Problem creating flat!!!!") Logger.Info(ex.Message) End Try Else 'if flat pattern exists Logger.Info("HasFlatPattern: " & oCompDef.HasFlatPattern) Logger.Info("Trying to get flatpattern...") ThisApplication.Documents.Open(oFullFileName, True) Try oCompDef.FlatPattern.Edit Catch ex As Exception Logger.Info("Problem editing flat!!!!") Logger.Info(ex.Message) End Try End If sOut = "FLAT PATTERN DXF?AcadVersion=2000&OuterProfileLayer=IV_INTERIOR_PROFILES" sFullDXFname = oFolder & "\" & oName & ".dxf" 'Output the DXF oCompDef.DataIO.WriteDataToFile(sOut, sFullDXFname) Try Logger.Info("DXF created!!!: " & sFullDXFname) Catch ex As Exception Logger.Info("Problem creating DXF!!!!") Logger.Info(ex.Message) End Try oCompDef.FlatPattern.ExitEdit Try If oCreated_Flat = True Then oDoc.Save Catch ex As Exception Logger.Info("Saving the file.") Logger.Info(ex.Message) End Try oDoc.Close Logger.Info("*******************") End If End Sub Sub PDF_Out(ByRef oDocument As Document, oFolder As String) ThisApplication.StatusBarText = "Processing PDF.........." & oDocument.displayname oFullFileName = oDocument.FullFilename oFileName = Right(oFullFileName, Len(oFullFileName) - InStrRev(oFullFileName, "\")) oName = Left(oFileName, InStrRev(oFileName, ".") -1) 'name without extension sFullPDFname = oFolder & "\" & oName & ".pdf" oPDFAddIn = ThisApplication.ApplicationAddIns.ItemById _ ("{0AC6FD96-2F4D-42CE-8BE0-8AEA580399E4}") oContext = ThisApplication.TransientObjects.CreateTranslationContext oContext.Type = IOMechanismEnum.kFileBrowseIOMechanism oOptions = ThisApplication.TransientObjects.CreateNameValueMap oDataMedium = ThisApplication.TransientObjects.CreateDataMedium oOptions.Value("All_Color_AS_Black") = 0 oOptions.Value("Remove_Line_Weights") = 0 oOptions.Value("Vector_Resolution") = 400 oOptions.Value("Sheet_Range") = Inventor.PrintRangeEnum.kPrintAllSheets 'Set the PDF target file name oDataMedium.FileName = sFullPDFname 'output the PDF oPDFAddIn.SaveCopyAs(oDocument, oContext, oOptions, oDataMedium) End Sub

Re: iLogic to Batch Export PDF and DXF

ErnestoGL — Sun, 16 Oct 2022 07:02:23 GMT

Thank you for this rule, it´s really amazing. I´ve been trying to modify the rule in order to get the "Title" ipropertie from the part file as a PDF file name and adding the revision number at the end but I´ve not get it. Im realatively new in iLogic and programming, doy you have any ideas guys?

Re: iLogic to Batch Export PDF and DXF

ryan_holtonVREQV — Thu, 06 Jul 2023 11:04:36 GMT

Hi,

Would you be able to alter this code so that I can pick the save destination / file path each time rather than it automatically saving to a specified location.

Thanks

Re: iLogic to Batch Export PDF and DXF

ALadZ339U — Thu, 29 Aug 2024 12:12:26 GMT

can i pleaswe get the code to save the pdf and dxf file in same folder where the original drawing file is ?