G10 G90 L10 Improper G Code - 16i Robodrill Fanuc


Results 1 to 9 of 9

Thread: G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

  1. #1
    Registered
    Join Date
    May 2018
    Location
    United States
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

    Does someone know why I can use G10 with L2 but not L10?For example:I am able to useG10 L2 P1 X2.0;but when I useG10 G90 L10 P1 R4.0 (it says improper G Code) - This command has been used just fine on the other Robodrill 16i. Do I have to anable L10 somewhere in parameter?Thanks

    Similar Threads:


  2. #2
    Gold Member
    Join Date
    Feb 2006
    Location
    india
    Posts
    1742
    Downloads
    0
    Uploads
    0

    Default Re: G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

    I use G90 G10 instead of G10 G90.
    Not sure if this will make any difference, but you may try.



  3. #3
    Registered
    Join Date
    May 2018
    Location
    United States
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

    Quote Originally Posted by sinha_nsit View Post
    I use G90 G10 instead of G10 G90.
    Not sure if this will make any difference, but you may try.
    Tried. It does not work. Thank you.



  4. #4
    Registered
    Join Date
    Apr 2011
    Location
    USA
    Posts
    426
    Downloads
    0
    Uploads
    0

    Default Re: G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

    (1) For tool compensation memory A
    G10 L11 P_R_;
    where P_: Offset No.
    R_: Tool compensation amount
    (2) For tool compensation memory B
    Setting/changing the geometric compensation amount
    G10 L10 P_R_;
    Setting/changing the wear compensation amount
    G10 L11 P_R_;
    (3) For tool compensation memory C
    Setting/changing the geometric compensation amount for H code
    G10 L10 P_R_;
    Setting/changing the geometric compensation amount for D code
    G10 L12 P_R_;
    Setting/changing the wear compensation amount for H code
    G10 L11 P_R_;
    Setting/changing the wear compensation amount for D code
    G10 L13 P_R_;



  5. #5
    Gold Member
    Join Date
    Feb 2006
    Location
    india
    Posts
    1742
    Downloads
    0
    Uploads
    0

    Default Re: G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

    Try 5001#0 (TLC) = 1



  6. #6
    Registered
    Join Date
    May 2018
    Location
    United States
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

    Quote Originally Posted by sinha_nsit View Post
    Try 5001#0 (TLC) = 1
    It still does not work with the L10. I was able to use G10 G90 Px Rx.x but not with L10.

    Last edited by tecoknn; 05-16-2018 at 08:28 AM.


  7. #7
    Gold Member
    Join Date
    Feb 2006
    Location
    india
    Posts
    1742
    Downloads
    0
    Uploads
    0

    Default Re: G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

    The book says that no L-word is needed on a lathe. Mills do need this.

    If the problem still persists, use system variables instead.
    In fact, if the machine is macro enabled, use of G10 may be avoided.



  8. #8
    Registered
    Join Date
    May 2018
    Location
    United States
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

    I am able to use:
    G10 L1
    G10 L2..
    ..
    G10 L11

    Same control 16i-MB same model alpha-T21iDL with macro enable on a diff Fanuc Robodrill Milling machine, I am able to use G10 L10.



  9. #9
    Registered
    Join Date
    May 2018
    Location
    United States
    Posts
    8
    Downloads
    0
    Uploads
    0

    Default Re: G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

    Problem solved. Thank you for all the help guys. Basically, you just need to switch to a separate height and diameter (radius) offset screen (some call Offset Memory Type C?) and it will enable L10 to use with G10. Can't say much because it is one of 9900 paid option parameters from Fanuc (I believe).



Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

G10 G90 L10 Improper G Code - 16i Robodrill Fanuc

G10 G90 L10 Improper G Code - 16i Robodrill Fanuc