584,866 active members*
5,090 visitors online*
Register for free
Login
Results 1 to 6 of 6
  1. #1
    Join Date
    Sep 2008
    Posts
    1

    c axis feed rate on a turn /mill machine

    Have an OM-LTD turn mill machine and can not get the feed rate for the C axis mill mode to work. I have anFANUC 18i-T controld. Any one been through this before??

    N366( TOOL #03 OFFSET #03)
    N368( 1.00 END MILL )
    N370( MILL THE O.D. )
    N372( OP# 12 )
    N374G97S19100M3
    N376G0X38.8876Z3.C.007M8
    N378G12.1
    N380X38.8876C0Z3.
    N382Z-.25
    N384G42G1C.3F11.46 Feed here at full c axis rate
    N386G3X38.6876C.3R.5
    N388G2X38.6876C-.0025R19.3438
    N390X-38.6876C.0025R19.3438
    N392X38.6876C-.0025R19.3438
    N394X38.6876C-.005R19.3438
    N396G3X38.8874C-.305R.5
    N398G1G40X38.8876C-.005
    N400C-.005Z3.
    N402G13.1
    N404G18
    N406M9
    N408G28U.0W.0 M05
    N410T0300
    N412M0


    thanks Bike

  2. #2
    Join Date
    Feb 2006
    Posts
    992
    check to see if you still have G94(feed per rev) or G95 feed(feed per min).... G95 is what you want.

    Other thing, I don't see and code switch to milling mode.
    The best way to learn is trial error.

  3. #3
    Join Date
    May 2007
    Posts
    1003
    Not familiar with your control. How is M3 starting the live tooling instead of the main spindle? Or does the main spindle use a different M-code?

  4. #4
    Join Date
    Jul 2003
    Posts
    263
    Quote Originally Posted by newtexas2006 View Post
    check to see if you still have G94(feed per rev) or G95 feed(feed per min).... G95 is what you want.

    Other thing, I don't see and code switch to milling mode.
    G94 & G95 are for the mills

    the lathe uses

    G98 Feed per Minute
    G99 Feed per Rev

    and he needs to active his mill mode
    the live tool uses a different M code than the main spindle
    If you can ENVISION it I can make it

  5. #5
    Join Date
    May 2006
    Posts
    99
    I have a Deawoo Puma with Fanuc 18 . I always use M33 G97 S... to start the " mill " Do you call it "live tooling" in the US? Always wonderd what "live tooling" meant.
    Then G98 G00 X.. Z.. C.. M08.
    When done with the milling call G99 or you'll get a "NO FEEDRATE" alarm when you go back to turning.
    As for G12.1, I use G112 or I get "inproper G-code alarm". Same for G13.1 ( G113 ).

  6. #6
    Join Date
    May 2007
    Posts
    1003
    Quote Originally Posted by Stebedeff View Post
    I have a Deawoo Puma with Fanuc 18 . I always use M33 G97 S... to start the " mill " Do you call it "live tooling" in the US? Always wonderd what "live tooling" meant.
    Then G98 G00 X.. Z.. C.. M08.
    When done with the milling call G99 or you'll get a "NO FEEDRATE" alarm when you go back to turning.
    As for G12.1, I use G112 or I get "inproper G-code alarm". Same for G13.1 ( G113 ).
    Pretty much how we do it. Guess it got called "live tooling" because the tools move whereas standard tools are "dead". Hope one doesn't say "Hi" to me one day. LOL.

Similar Threads

  1. Replies: 0
    Last Post: 04-22-2008, 07:20 PM
  2. Feed rate Ovverride also Increases rapid rate.
    By Korellibopper in forum Machines running Mach Software
    Replies: 1
    Last Post: 01-31-2008, 12:37 AM
  3. Feed Rate and Spindle Rate for this cut?
    By DroopyPawn in forum MetalWork Discussion
    Replies: 20
    Last Post: 11-22-2007, 06:12 AM
  4. Mill Drill Real World CNC Feed Rate
    By wmgeorge in forum Benchtop Machines
    Replies: 1
    Last Post: 09-28-2005, 08:39 PM
  5. Advice needed for Mill Feed Rate
    By raytor in forum Benchtop Machines
    Replies: 4
    Last Post: 03-25-2005, 08:11 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
  •