Results 1 to 12 of 12

Thread: G10 to select coordinate system

  1. #1
    Registered jorgehrr's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    203
    Downloads
    0
    Uploads
    0

    G10 to select coordinate system

    All my fixture offsets are full (G54, G55.....)

    I know I can use G10 to input new offsets, my question is at the end of the program.... are the original numbers going to go back and what is the M/G code that does it.

    I just want to make sure if the original fixture offsets will remain after I use G10.

    Thank you in advance

    George


  2. #2
    Registered hoidahl's Avatar
    Join Date
    Sep 2007
    Location
    usa
    Posts
    34
    Downloads
    0
    Uploads
    0

    example

    Yes the offsets should remain. Here is an example of what we use.

    G10L20P1X-9.9149Y-11.8528Z-22.419
    G10L20P2X-1.9459Y-11.8528Z-29.771
    G10L20P3X-17.8819Y-11.8528Z-29.771
    G0G17G40G80
    T5
    M6
    T6
    G54.1P1
    G0G90X0.Y1.375S1579M3
    G43Z1.H5M8
    G81G98X0.Y1.375Z-.1565R.1F9.47
    Y-1.375
    G0G80Z1.
    G91G28Z0.
    G54.1P2
    G90G0X.75Y0.
    G43Z1.H5
    G81G98X.75Y0.Z-.0985R.1F9.47
    G0G80Z1.
    G91G28Z0.
    G54.1P3
    G90G0X-.75Y0.
    G43Z1.H5
    G81G98X-.75Y0.Z-.0985R.1F9.47
    G0G80Z12.
    M9
    G91G30X0Y0Z0M67
    M1


  3. #3
    Registered jorgehrr's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    203
    Downloads
    0
    Uploads
    0
    Ohhh.

    Do you see anything wrong with mine????

    O6001
    G80 G40
    T01M06 (1/2 Drill)
    G0 G90 G10 L2 P1 X-22.3837 Y-12.2827 Z-11.0387 M3 T2
    G43 H01 Z0.1 M08
    G54 P1 X1.0 Y1.0
    G81 R0.1 Z-0.3 F5.0
    G0 G80 Z1.0 M9
    G91 G28 Z0 M19
    M30

    Thank you in advance

    George


  4. #4
    Registered hoidahl's Avatar
    Join Date
    Sep 2007
    Location
    usa
    Posts
    34
    Downloads
    0
    Uploads
    0
    We just put the g10 lines at the beginning of the program so they can be located easily. Looks like it should work. Does it?


  • #5
    Registered
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    11,960
    Downloads
    0
    Uploads
    0
    Quote Originally Posted by jorgehrr View Post
    All my fixture offsets are full (G54, G55.....)

    I know I can use G10 to input new offsets, my question is at the end of the program.... are the original numbers going to go back and what is the M/G code that does it.

    I just want to make sure if the original fixture offsets will remain after I use G10.

    Thank you in advance

    George
    The G10 line will permanently change the offset values. The only way to get your original ones back is to have another G10 line that re-enters the original values.

    Based on the little bit you have written I think you should do some reading about G52.

    G52 gives you an offset shift and it does not change the G54, etc offset values. You can use many different G52 commands in a single program; in effect with G52 you have an unlimited number of offsets possible.

    Depending on your machine the G52 values may be zeroed by M30 or RESET but you can always zero them by using G52 X0. Y0. Z0.
    An open mind is a virtue...so long as all the common sense has not leaked out.


  • #6
    Registered hoidahl's Avatar
    Join Date
    Sep 2007
    Location
    usa
    Posts
    34
    Downloads
    0
    Uploads
    0
    g54 isn't changed doing it this way its put into a p1(101)p2(102) etc. offset and g54 remains the same.


  • #7
    Registered jorgehrr's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    203
    Downloads
    0
    Uploads
    0
    Well.......

    It changed mine. I was convince numbers will remain the same after the M99 code but Geof. is correct, the change stays.

    In my machine I can not use G54.1 P? (machine alarms out)
    It has to be only G54 P?

    May be that is the reason.

    Thank you guys. I'll find the way to get them back.

    Cheers

    George


  • #8
    Registered
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    11,960
    Downloads
    0
    Uploads
    0
    Quote Originally Posted by jorgehrr View Post
    ....

    Thank you guys. I'll find the way to get them back.

    Cheers

    George
    Like I said above...read up on G52, it will do what you want.
    An open mind is a virtue...so long as all the common sense has not leaked out.


  • #9
    Registered
    Join Date
    Dec 2006
    Location
    USA
    Posts
    24
    Downloads
    0
    Uploads
    0
    "my machine I can not use G54.1 P? (machine alarms out).."

    You do not have the Extended offset option so the G54.1 P? will generate an alarm, there is a cost if you need that many offsets.

    G54 G55, G56, etc. is standard on the controls, and it gives you six offests to play with. The extended offset option gives you those 6 plus 48 additional.


  • #10
    Registered
    Join Date
    Jul 2007
    Location
    usa
    Posts
    16
    Downloads
    0
    Uploads
    0
    G52 or G92 works good.


  • #11
    Registered
    Join Date
    Nov 2008
    Location
    USA
    Posts
    11
    Downloads
    0
    Uploads
    0
    Our machines run several different programs and we change the work offset many, many times within a given program. I guess my question would be: Why not use the G10 as much as needed. With good programing discipline you can change as much as need to accomplish the programming needs.


  • #12
    Registered
    Join Date
    Dec 2006
    Location
    USA
    Posts
    24
    Downloads
    0
    Uploads
    0
    These were production machines and machine operators did not adjust the offsets. That was process engineer function. We used a single G54 offset register but transfered in the offsets for specific table positions from the extended offset table. The B<value> selected the offsets to use automatically. Basically think of a dynamic offset that follows the table, but on a control that did not have the option. So we created a sub program that accomplished the task automatically.


  • Similar Threads

    1. G68 Coordinate Rotation System
      By ebigfoot2 in forum Fanuc
      Replies: 2
      Last Post: 08-13-2007, 08:33 AM
    2. coordinate system
      By kiethnt in forum G-Code Programing
      Replies: 6
      Last Post: 04-26-2007, 08:46 AM
    3. Coordinate system problems
      By R.thayer in forum LinuxCNC (formerly EMC2)
      Replies: 0
      Last Post: 11-19-2006, 03:36 PM
    4. coverting from Right-hand to left-hand coordinate system
      By eltonr in forum General CAM Discussion
      Replies: 6
      Last Post: 10-14-2004, 09:40 PM
    5. User coordinate system?
      By HuFlungDung in forum OneCNC
      Replies: 5
      Last Post: 04-18-2003, 10:26 PM

    Posting Permissions


     


    About CNCzone.com

      We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

    Follow us on

    Facebook Dribbble RSS Feed


    Search Engine Friendly URLs by vBSEO ©2011, Crawlability, Inc.