512,240 active members
4,536 visitors online
Register for free
Results 1 to 7 of 7
  1. #1
    Join Date
    May 2003

    Question How to mirror GCode file?

    Hi all,

    Well I have managed to find and run the script to go from a Eagle board file to Gcode. Now the only problem I have is how do I mirror the GCode? The program works fine for the top copper but I need to mirror the bottom to have the traces in the correct orientation.

    Thanks for your help!


  2. #2
    Join Date
    May 2003
    Assuming you disnt generate the code from a CAM system (in which case mirroring in the CAM system and reposting would be easiest), and assuming your control wont do it... Use an editor such as cimco, editcnc (you can search for free downloads or 30 day trial versions of these editors) they have a function that does this automaticaly.

    If you are simply miroring about the X axis, all non-zero X values and I values get the sign changed from positive to negative or vice versa. The editors I mentioned also have a backplot feature that will display graphicaly the edited toolpath.

    Try this link


    CAM teh "left ... left ... left . right . left"
    Wee aim to please ... You aim to ... PLEASE.

  3. #3
    Join Date
    Apr 2003
    In Eagle CAM, set the mirror option ON when doing the bottom side. This will automatically mirror your trace.

    Another way is to reverse the direction setting in your CNC software; that how I do it if I can do it at source application.
    Stupid questions make me smarter...
    See how smart I've become at www.9w2bsr.com ;-P

  4. #4
    Join Date
    Jun 2003
    I agree with CAMmando. Just follow his link and the rest should be history.
    no problem!

  5. #5
    Join Date
    Jun 2003


    Try G51 X0 Y0 I-1000 J-1000

    This will scale around point X0 Y0, with a scale factor of 100% (full size) and the - (minus sign) means it will mirror it in this plane.

    So to mirror in X but not in Y use I-1000 J1000. Or just leave the J out. G51 X0 I-1000

    Use G50 to cancel G51.


  6. #6
    Join Date
    Apr 2003
    There is also a very basic way that I have done and tested before in word pad.

    Select Search and Replace from the menu.

    Check match whole word.

    Find X-

    Replace with V$

    Then find X

    Replace with X-

    Then find V$

    And replace with X

    Do this also with your I values in arcs

    FYI this is a great way to change the axis integers if you are wishing to convert a Z plane program to an X or a Y plane program on a universal milling machine.
    "A Helicopter Hovers Above The Ground, Kind Of Like A Brick Doesn't"
    Greetings From Down Under
    Dave Drain
    Akela Australia Pty. Ltd.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)

  7. #7
    Gold Member
    Join Date
    Mar 2003
    Mighty interesting! Haven't thought doing things this way. Normally i do mirroring, rotation etc on the machine....that's the nice thing of wire eroders, but if the machine can't do it, well.....

    *** KloX ***
    I'm lazy, I'm only "sparking" when the EDM is running....

Similar Threads

  1. How do i get my autocad file onto mastercam?
    By EdE in forum Uncategorised CAM Discussion
    Replies: 3
    Last Post: 02-23-2011, 06:54 AM
  2. Emco Compact 5 PC...have ????
    By Double G in forum Mini Lathe
    Replies: 42
    Last Post: 08-23-2010, 12:26 AM
  3. Boot disk for EZ-Track DX, batch file?
    By mmm2003 in forum Bridgeport / Hardinge Mills
    Replies: 8
    Last Post: 01-31-2007, 06:47 PM
  4. File Extensions in PFE
    By E-Stop in forum Mastercam
    Replies: 0
    Last Post: 06-25-2004, 12:53 PM
  5. AutoCad 2000 Missing .dll file
    By E-Stop in forum Autodesk
    Replies: 12
    Last Post: 05-30-2003, 05:43 PM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts