502,912 active members
7,186 visitors online
Register for free
Login
IndustryArena Forum > Machine Controllers Software and Solutions > Fanuc > Troubleshooting MO3/M04 operation
Results 1 to 7 of 7
  1. #1
    Junior Member
    Join Date
    Oct 2018
    Posts
    11

    Troubleshooting MO3/M04 operation

    I have a 1983 Kitamura mycenter 3 with Fanuc 6m controller. I can issue a spindle speed and m03 or m04 command in MDI and machine responds. RPM gage reads whatever S**** I entered. However when I right a test code with a few moves etc it comes to the S500 M03 line, spindle turns on and program stops like it's not receiving speed obtained signal. I can hit reset, spindle stops and rest of program continues on thru. Anyone have ideas on fixing this...or even a parameter to change to eliminate the speed verify?

  2. #2
    Flies Fast
    Join Date
    Dec 2008
    Posts
    2790

    Re: Troubleshooting MO3/M04 operation

    put up you bit of test code that is not working
    .... it may not be that line that is at fault

  3. #3
    Registered
    Join Date
    Jun 2003
    Posts
    194

    Re: Troubleshooting MO3/M04 operation

    Superman's suggestion is a good one. In full auto the control reads in several lines ... so the issues may well be further down the code.
    Another suggestion ... did you try single block instead of full auto? ... does it go any further in single block?

    Hope this helps ...
    Check out our Real World Machine Shop Software at Kipware® Software - Real World Machine Shop and CNC Software

  4. #4
    Junior Member
    Join Date
    Oct 2018
    Posts
    11
    Good morning gentlemen and thanks for the response. I'm sure you'll get a chuckle out of my feeble attemp at g-code programming but here is what I did

    G90 G17 G28 X0 Y0 Z0
    G54
    G01 X2.00 Y2.00 Z-1.00 F50.00
    G01 X4.00 Y2.00 F50.00
    G02 X6.00 Y6.00 F50.00
    G01 Z-2.500 F40.00
    M8
    S500 M03
    G01 Z-2.625 F20.00
    G02 X2.00 Y3.00 F50.00
    G02 X2.00 Y2.00 F50.00
    M9
    G01 Z.00 F60.00
    M30
    %

    I tried different spindle speeds as well as M04 instead of M03 Always same results. Machine moves to Z-2.500, spindle turns on and program stops and machine stops. I can press reset, spindle turns off. Press cycle start and program and machine continues to end of cycle

  5. #5
    Junior Member
    Join Date
    Oct 2018
    Posts
    11
    single block still will not continue past Mo3 unless I press reset first.

  6. #6
    Registered
    Join Date
    Dec 2012
    Posts
    315

    Re: Troubleshooting MO3/M04 operation

    Hi,

    Remove the G02 in all the lines or add a R-value ( I / J) in these G02 lines.
    Is there no alarm ?

    Regards,
    Heavy_Metal.

  7. #7
    Junior Member
    Join Date
    Oct 2018
    Posts
    11
    Heavy Metal thank you so much. That simple to you correction fixed it right up Program cycles all the way to end. Now all I should have left is troubleshooting the tool changer carousel and I should have chips flying

  8. #8
    Registered
    Join Date
    Feb 2006
    Posts
    1765

    Re: Troubleshooting MO3/M04 operation

    Another suggestion:
    G28 X0 Y0 Z0 must be commanded in G91 mode. Change to G90 thereafter.
    For safety reasons, it is better to home Z first, followed by XY home::
    G91 G28 Z0;
    G28 X0 Y0;;
    G90;

  9. #9
    Flies Fast
    Join Date
    Dec 2008
    Posts
    2790
    Quote Originally Posted by Hopcycle1 View Post
    ... I'm sure you'll get a chuckle out of my feeble attemp at g-code programming but here is what I did

    G90 G17 G28 X0 Y0 Z0
    G54
    G01 X2.00 Y2.00 Z-1.00 F50.00
    G01 X4.00 Y2.00 F50.00
    G02 X6.00 Y6.00 F50.00
    G01 Z-2.500 F40.00
    M8
    S500 M03
    G01 Z-2.625 F20.00
    G02 X2.00 Y3.00 F50.00
    G02 X2.00 Y2.00 F50.00
    M9
    G01 Z.00 F60.00
    M30
    %
    a little chuckle....????????
    you 1st need to form some sort of programming structure...
    everyone had to have a start sometime...
    ie.
    top of prog...
    O1234 (job info)
    (header info... setup etc)
    G0 G17 G40 G80 G99 (safety codes)
    M5 M9
    G91 G28 Z0 (Z home)
    G90
    M1 ( optional stop)
    ()
    (toolchange)
    Ttt M6 ( tool info)
    ()
    (set tool data)
    G90 G54 ( set co-ord system.... you could use more in one program)
    G0 Xx Yy
    Ssss M3
    G43 Htt Zz ( add toollenght to spindle while moving to z)
    .... your prog
    ( retract procedure )
    M5 M9
    G91 G28 Z0.
    G90
    M1
    ()
    ...repeat for next tool from (toolchange) for each tool
    ...
    (final retract)
    G91 G28 Y0. (move table to front for part unloading)
    M30
    %

    This is only a guide... but a point to remember....
    if you turn a code ON..... turn it OFF ..... & build a good set of safety codes that restate the machine's startup condition.
    ... I've seen drilling done at near rapid rate because feed per rev. was not corrected after a tapping cycle....

  10. #10
    Junior Member
    Join Date
    Oct 2018
    Posts
    11
    Thank you Superman! I'm going to use your example to help me troubleshoot the ATC. At least I'll know it's not another one of my program failures

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
  •