Results 1 to 8 of 8
  1. #1
    spock is offline Hot Rolled
    Join Date
    Dec 2006
    Location
    Central Ky
    Posts
    923

    Default Fanuc OT, feedrate missing, but its not!

    Well, after 20 years it looks like I need a lesson in Programming 101. Starting a program with a facing cut, IF it is the first time I push cycle start, it runs fine. After that, I am getting the "O11 P/S" alarm, indicating that there is no feedrate. Please, look at my program, and tell me what I am missing. Cause I see a feedrate, but the control is not for some reason. And, keep in mind, that the other 2 programs that I have run on this lathe are programmed the same and I had no trouble at all. So, I must be missing something.

    Here is my code:

    O3333
    N1 G50 S2500
    G00 T0101
    G40
    G96 S0500 M03
    X0.8 Z0.0 (machine positions here, then alarms)
    G01 X-.064 F0.006
    Z0.02
    G00 X.591
    etc......

  2. #2
    alphonso is online now Stainless
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    1,555

    Default

    I don't see anything to cause the error.

    Curious to why you have the G00 3 blocks from first move.

  3. #3
    spock is offline Hot Rolled
    Join Date
    Dec 2006
    Location
    Central Ky
    Posts
    923

    Default

    habit, always programmed that way.

    So, it just goes to show, you want to figure out something simple, post it here first! I am bar pulling at teh end, using G98, and on this control, unlike my 10T, I MUST put in a G99 to get it back into feed per revolution.

    Im ready for my dunce cap now.

  4. #4
    hdrider63's Avatar
    hdrider63 is offline Aluminum
    Join Date
    Oct 2007
    Location
    Watertown, SD
    Posts
    237

    Default

    Are you using a G98 further down in the program? It may be looking at IPM rather than IPR in which case your feedrate would be too slow for the control to handle. I would try this:
    G99G1XZF.006

    Good luck!

    I see you beat me to the punch!!
    Last edited by hdrider63; 09-01-2010 at 06:01 AM. Reason: Posted just after he figgered it out.

  5. #5
    Ox's Avatar
    Ox
    Ox is offline Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    17,559

    Default

    Quote Originally Posted by spock View Post
    habit, always programmed that way.

    So, it just goes to show, you want to figure out something simple, post it here first! I am bar pulling at teh end, using G98, and on this control, unlike my 10T, I MUST put in a G99 to get it back into feed per revolution.

    Im ready for my dunce cap now.


    I find that any time my machine doesn't like to "re-start" properly in AUTO cycle - it always comes back to how I left it at the end of the prog. Not how I started it.


    ------------------

    Think Snow Eh!
    Ox

  6. #6
    Philabuster's Avatar
    Philabuster is online now Titanium
    Join Date
    Jul 2006
    Location
    Tempe, AZ
    Posts
    2,628

    Default

    Quote Originally Posted by spock View Post
    Well, after 20 years it looks like I need a lesson in Programming 101. Starting a program with a facing cut, IF it is the first time I push cycle start, it runs fine. After that, I am getting the "O11 P/S" alarm, indicating that there is no feedrate. Please, look at my program, and tell me what I am missing. Cause I see a feedrate, but the control is not for some reason. And, keep in mind, that the other 2 programs that I have run on this lathe are programmed the same and I had no trouble at all. So, I must be missing something.

    Here is my code:

    O3333
    N1 G50 S2500
    G00 T0101
    G40
    G96 S0500 M03
    G00 X0.8 Z0.0 (machine positions here, then alarms)
    G01 X-.064 F0.006
    Z0.02
    G00 X.591
    etc......
    I would add the G00 command. It should be modal from the T0101 line but I do not see an X or Z move there so it may be the issue.

  7. #7
    gcodeguy is offline Cast Iron
    Join Date
    Jun 2007
    Location
    Easton, PA
    Posts
    482

    Default

    One way to avoid such problems is to have a subprogram containing default settings (or whatever else you like) called at the beginning of each operation similar to the Hardinge Safe Index programs.

    My first command (when not setting a workshift) is M91. This calls up program 9001 which has commands such as G0G40G99G97G80, etc.

    Not only saves typing in the main program, but eliminates senior moments.

  8. #8
    Gerrythewelshman is offline Cast Iron
    Join Date
    Oct 2006
    Location
    Ireland
    Posts
    392

    Default feed

    Hi,
    Just a thought . If the machine is reading G21 metric by 'mistake' it might not read 0.006mm (0.0002") and fault out.

Bookmarks

Posting Permissions

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