4 Replies Latest reply on Sep 1, 2010 7:49 AM by patrick.cashman

    Expedition OUTPUT Files- Script


      Does anyone have a script or could they make one for me that runs all the output files for instance.


      Silkscreen Generator


      IPC356 netlist


      Drill files

      PDF Drawings


      I would like to do this in one script!


      Can anyone help me?




      Erik P. Wainwright

      Sr. PCB Designer

      Viasat Inc.

      6122 El Camino Real

      Carlsbad, CA. 92008


        • 1. Re: Expedition OUTPUT Files- Script

          Hello Erik-san,


          Do you want the sample script which uses the Automatio Pro?




          • 2. Re: Expedition OUTPUT Files- Script

            PDF Files? You mean Assembly Drawings?

            • 3. Re: Expedition OUTPUT Files- Script

              Hello Erik,


              there be should some in Kendalls Auto Active Toolkit at https://sourceforge.net/projects/uwtoolbox/


              Also see section Pro Engines in his thread http://communities.mentor.com/thread/3490




              • 4. Re: Expedition OUTPUT Files- Script



                What you are asking is not a trivial task.  It is also not a 'one size fits all' kind of thing.  There are several reasons for this:


                • There is usually a company naming convention for output files that needs to be included in this kind of script.
                • Some remove unused pads, some don't.  This is part of Gerber Setup.  Lots of other company specific rules about Gerber Setup.
                • There are often user layers that are included in Gerber output.  How to know which ones?
                • Not all companies include the same output files in what they create/store/send to vendors.
                • The way the files get collected and stored in the database file structure is probably unique.
                • And so on . . .


                Having said that, I can assure you that it is possible to do all the things you asked, and meet all the company specific requirements for what to output, how to name the files, and where to put them.  A lot of it is done by writing out the Gerber/Drill setup files in the Config directory, then executing the output commands programmatically.  In a lot of cases it's only a question of executing the command via a script.  Getting the syntax right for creating those config files is a bit tricky.  From there, it is a lot of File I/O operations to create directories, copy/move files, rename them etc.


                The Gui.ProcessCommand function is very useful.  It is what you use to execute commands via scripts.  Here is an example that writes out Gerber data: (VB6)


                Private Sub write_gerber()

                    Dim gui As gui
                    Dim dlg As Dialog
                    Dim btn As button
                    Set gui = app.gui
                    gui.SuppressTrivialDialogs = True
                    If gui.ProcessCommand("Output->Gerber", True) Then
                        Set dlg = gui.FindDialog("Gerber Output")
                        If dlg.IsValid() Then
                            Set btn = dlg.FindButton("Process Checked Output Files")
                            If btn.IsValid Then
                                Call btn.Click
                                'MsgBox ("Found Process Checked Output Files button")
                                MsgBox ("The Process Checked Output Files button was not found.")
                            End If           
                            Set btn = dlg.FindButton("Close")
                            Call btn.Click
                            MsgBox ("The Gerber Output Dialog box was not found.")
                        End If
                        MsgBox ("The Output Gerber Command was not found. Try restarting the Application.")
                    End If
                    MsgBox ("Gerber Data is in the /Output/Gerber directory.")

                End Sub


                I hope this gets you going on the right path.