Fanuc OT stopped counting with count code.
Close
Login to Your Account
Likes Likes:  0
Results 1 to 20 of 20
  1. #1
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,509
    Post Thanks / Like
    Likes (Given)
    1040
    Likes (Received)
    4236

    Default Fanuc OT stopped counting with count code.

    Here is a stumper, the lathe counts when using M2(end of program, reset) when doing single cycle parts. It will no longer count when putting M99(end of sub program)at the bottom preceded by M12 (end of cycle, count). The latter is what is done if you want to run continuously out of bar stock. The same program I ran over and over for years all of a sudden stopped counting like all of a sudden M12 isn't recognized. During the period it stopped working no parameters or settings were altered or any components replaced.
    Last edited by Dualkit; 08-01-2020 at 02:54 PM.

  2. #2
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    3,779
    Post Thanks / Like
    Likes (Given)
    824
    Likes (Received)
    2609

    Default

    Quote Originally Posted by Dualkit View Post
    Here is a stumper, the lathe counts when using M2(end of program, reset) when doing single cycle parts. It will no longer count when putting M99(end of sub program)at the bottom preceded by M12 (end of cycle, count). The latter is what is done if you want to run continuously out of bar stock. The same program I ran over and over for years all of a sudden stopped counting like all of a sudden M12 isn't recognized. During the period it stopped working no parameters or settings were altered or any components replaced.
    Have you looked at parameter 6710 to see if 12 is still registered?

    What about if you MDI an M12. Does that increment the counter?

  3. #3
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,509
    Post Thanks / Like
    Likes (Given)
    1040
    Likes (Received)
    4236

    Default

    Quote Originally Posted by jancollc View Post
    Have you looked at parameter 6710 to see if 12 is still registered?

    What about if you MDI an M12. Does that increment the counter?
    I will check that out later tonight, the job is almost done. With my low budget homemade puller, no way I can let it run out of stock without me there. Been using the stop watch on my phone to make sure I am there in time. I have every manual for the machine except the diagnostic one.

  4. #4
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,509
    Post Thanks / Like
    Likes (Given)
    1040
    Likes (Received)
    4236

    Default

    It takes M12 on mdi, but that does not alter the count. The machine does not show a parameter 6710, in fact it has parameters 0-999 and some in the 8000's and that is it. It is only 2 axis, single 12 station turret and no power tools, simple as it gets. It seems to have very limited options, few canned cycles, and not many options on the soft keys either. It doesn't even have a soft key for number search on parameters.

  5. #5
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    3,779
    Post Thanks / Like
    Likes (Given)
    824
    Likes (Received)
    2609

    Default

    Yeah, I have Oi's. Didn't mean to send you on a wild goose chase.

    I found this old post from vancbiker.

    Fanuc OT Parts counter and bar pulling

    Check parameter 219.

  6. #6
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,509
    Post Thanks / Like
    Likes (Given)
    1040
    Likes (Received)
    4236

    Default

    Quote Originally Posted by jancollc View Post
    Yeah, I have Oi's. Didn't mean to send you on a wild goose chase.

    I found this old post from vancbiker.

    Fanuc OT Parts counter and bar pulling

    Check parameter 219.
    Thanks, I will try the stuff in the other thread tomorrow. Wasn't much of a wild goose chase, only took a couple minutes. I think my OT is revision C and it is almost 30 years old.

  7. #7
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    1,003
    Post Thanks / Like
    Likes (Given)
    90
    Likes (Received)
    366

    Default

    Quote Originally Posted by Dualkit View Post
    Here is a stumper, the lathe counts when using M2(end of program, reset) when doing single cycle parts. It will no longer count when putting M99(end of sub program)at the bottom preceded by M12 (end of cycle, count). The latter is what is done if you want to run continuously out of bar stock. The same program I ran over and over for years all of a sudden stopped counting like all of a sudden M12 isn't recognized. During the period it stopped working no parameters or settings were altered or any components replaced.
    On my miyano with ot early one think its a "A" I have to use M25 before the m30/m99 or m02

  8. #8
    Join Date
    Feb 2014
    Location
    FL
    Posts
    3,490
    Post Thanks / Like
    Likes (Given)
    11866
    Likes (Received)
    4016

    Default

    Doesn't fix your problem, but a quick fix would be to use a #5XX variable as a counter, until you can get your issue sorted. Just make sure to reset it every time you change a bar.

  9. #9
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,509
    Post Thanks / Like
    Likes (Given)
    1040
    Likes (Received)
    4236

    Default

    Quote Originally Posted by Delw View Post
    On my miyano with ot early one think its a "A" I have to use M25 before the m30/m99 or m02
    M25 on my machine is for a door switch option, that I do not have. I think M25 on your machine is like M12 on mine. It just strangely stop working out of the blue. Mine will count on M2 and M30 on MDI or running continuous from the program, but they cause the program to rewind and stop. M99 is the only code that will rewind and repeat, but it doesn't trigger the count. I suppose when I am bored I will flip through the parameter manual and see if a parameter controls what codes count. I have had parameters erase themselves before that happened after a long distance move, the only time I ever encountered that in all the CNC machines I have owned or worked on.

  10. #10
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,509
    Post Thanks / Like
    Likes (Given)
    1040
    Likes (Received)
    4236

    Default

    Quote Originally Posted by TeachMePlease View Post
    Doesn't fix your problem, but a quick fix would be to use a #5XX variable as a counter, until you can get your issue sorted. Just make sure to reset it every time you change a bar.
    Interesting, I only use #5XX variables for tool widths, part lengths, tool nose radii and the assorted calculations. Care to show an example of how to use as a counter? That is if it isn't a lot of trouble. I am sure I could find it in an operators manual somewhere. Do note this machine is a Fanuc OT revision C that was born almost 30 years ago. I is kind of a strange machine, you can use a lot of programing characters that aren't on the keypad or soft keys. Editing sometimes can be a PITA.
    Last edited by Dualkit; 08-04-2020 at 02:11 PM.

  11. #11
    Join Date
    Feb 2014
    Location
    FL
    Posts
    3,490
    Post Thanks / Like
    Likes (Given)
    11866
    Likes (Received)
    4016

    Default

    Quote Originally Posted by Dualkit View Post
    Interesting, I only use #5XX variables for tool widths, part lengths, tool nose radii and the assorted calculations. Care to show an example of how to use as a counter? That is if it isn't a lot of trouble. I am sure I could find it in an operators manual somewhere. Do note this machine is a Fanuc OT revision C that was born almost 30 years ago. I is kind of a strange machine, you can use a lot of programing characters that aren't on the keypad or soft keys. Editing sometimes can me a PITA.
    At the beginning of your code:

    IF[#501 GT 110]GOTO1

    Then put an N1 at the end of your program (after M2), followed by M0.


    Then before your M2, put #501 = #501+1. This will increment #501 by 1 every time you hit the end of the program.


    Now if #501 is greater than 110pcs (obviously make this whatever your desired part count is), the program will skip to the M0 and stop the machine.

  12. #12
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    1,003
    Post Thanks / Like
    Likes (Given)
    90
    Likes (Received)
    366

    Default

    Quote Originally Posted by Dualkit View Post
    M25 on my machine is for a door switch option, that I do not have. I think M25 on your machine is like M12 on mine. It just strangely stop working out of the blue. Mine will count on M2 and M30 on MDI or running continuous from the program, but they cause the program to rewind and stop. M99 is the only code that will rewind and repeat, but it doesn't trigger the count. I suppose when I am bored I will flip through the parameter manual and see if a parameter controls what codes count. I have had parameters erase themselves before that happened after a long distance move, the only time I ever encountered that in all the CNC machines I have owned or worked on.
    I figured the m25 was different was more on the Before end of program codes is were I have to put it. for some reason I thoguth you said you put it after the m99 m02 m30 code.
    do you only have a count readout in the screen, or does your machine also have a clicker counter on the side? my Miyano will quit counting in the screen one of the clicker counter on the side is full.
    I have the manuals with prms on the early controls but again its for the miyano(should be the same prm# just different m codes)



    My citizen with a fanuc t10 control quite counting after I lost prms. I uploaded all the rpms and even verified with citizen about it still nothing.
    we use the counter for the same thing so not to run out of bar and scrap tools.

  13. #13
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,733
    Post Thanks / Like
    Likes (Given)
    743
    Likes (Received)
    1081

    Default

    I'll second the 501 counter. It's bulletproof, tried, true, and tested. I have it embedded in my post for mill and lathe to keep the production workers honest. I found the off shift people were running M99 with loop counts to trick the parts count so they would get production bonuses. I like the way TeachMePlease uses the GOTO statement. Im sure I can find some uses for that......

  14. #14
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    984
    Post Thanks / Like
    Likes (Given)
    344
    Likes (Received)
    467

    Default

    Quote Originally Posted by Dualkit View Post
    It takes M12 on mdi, but that does not alter the count. The machine does not show a parameter 6710, in fact it has parameters 0-999 and some in the 8000's and that is it. It is only 2 axis, single 12 station turret and no power tools, simple as it gets. It seems to have very limited options, few canned cycles, and not many options on the soft keys either. It doesn't even have a soft key for number search on parameters.
    I have a machine with an OT C also and there is a way to search parameters without a soft key, I forget what it is since it's been a while since I've been in there playing around.

  15. #15
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    984
    Post Thanks / Like
    Likes (Given)
    344
    Likes (Received)
    467

    Default

    Press the LQP key, then the parameter number, then INPUT and that should take you directly there.

    Also on my machine Diagnostic 401 bit 7 1 enables work counter 0 disables. I don't know enough about them to know if that is dependent on the ladder and machine specific or common to all OT Cs

    And yes before anyone says anything I do have a OM membrane on an OT
    Attached Thumbnails Attached Thumbnails 20200804_184404.jpg  

  16. #16
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,509
    Post Thanks / Like
    Likes (Given)
    1040
    Likes (Received)
    4236

    Default

    Quote Originally Posted by TeachMePlease View Post
    At the beginning of your code:

    IF[#501 GT 110]GOTO1

    Then put an N1 at the end of your program (after M2), followed by M0.


    Then before your M2, put #501 = #501+1. This will increment #501 by 1 every time you hit the end of the program.


    Now if #501 is greater than 110pcs (obviously make this whatever your desired part count is), the program will skip to the M0 and stop the machine.
    Thanks! I will probably give that a try later on today or tomorrow, got another puller job to set up.

  17. #17
    Join Date
    Feb 2014
    Location
    FL
    Posts
    3,490
    Post Thanks / Like
    Likes (Given)
    11866
    Likes (Received)
    4016

    Default

    Quote Originally Posted by Dualkit View Post
    Thanks! I will probably give that a try later on today or tomorrow, got another puller job to set up.
    Just because I re-read my post and it may not have been the clearest, here's what I mean

    BEGIN PROGRAM
    IF [#501 GT 110] GOTO 1
    ENTIRE PROGRAM
    GUTS GO HERE
    #501 = #501+1
    M2

    N1
    M0

  18. #18
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,509
    Post Thanks / Like
    Likes (Given)
    1040
    Likes (Received)
    4236

    Default

    Quote Originally Posted by TeachMePlease View Post
    At the beginning of your code:

    IF[#501 GT 110]GOTO1

    Then put an N1 at the end of your program (after M2), followed by M0.


    Then before your M2, put #501 = #501+1. This will increment #501 by 1 every time you hit the end of the program.


    Now if #501 is greater than 110pcs (obviously make this whatever your desired part count is), the program will skip to the M0 and stop the machine.
    It won't work, it is either in the controller or the DNC software I use to send and receive, I just tried it. Everything goes in except when it hits N1, (I even tried N2) it thinks it has seen another start of a program and puts it under the next available program number. So I end up with two separate programs in the machine, the second one only two lines. The same thing happens if you make a mistake hand coding and type the letter O in a location call out instead of a zero. I honestly haven't used a N for a line number in a machine since I ran machines that did not have a CRT and just a 6 or so digit display. You know back in the day when you were just a twinkle in your parent's eye. I will dig in to the DNC software settings and see what is in there as I run the machine with a watchful eye. At least this part is only 3/8" long with 1:30 cycle time. Thanks again for the suggestion.

  19. #19
    Join Date
    Feb 2014
    Location
    FL
    Posts
    3,490
    Post Thanks / Like
    Likes (Given)
    11866
    Likes (Received)
    4016

    Default

    Quote Originally Posted by Dualkit View Post
    It won't work, it is either in the controller or the DNC software I use to send and receive, I just tried it. Everything goes in except when it hits N1, (I even tried N2) it thinks it has seen another start of a program and puts it under the next available program number. So I end up with two separate programs in the machine, the second one only two lines. The same thing happens if you make a mistake hand coding and type the letter O in a location call out instead of a zero. I honestly haven't used a N for a line number in a machine since I ran machines that did not have a CRT and just a 6 or so digit display. You know back in the day when you were just a twinkle in your parent's eye. I will dig in to the DNC software settings and see what is in there as I run the machine with a watchful eye. At least this part is only 3/8" long with 1:30 cycle time. Thanks again for the suggestion.
    Hmmm.......


    Less elegant, but it works:


    BEGIN PROGRAM
    #502=100.0
    IF[#501 GT 110]
    #502=0.0

    FIRST MOVE
    G1 G98 X2.0 F#502

    PROGRAM GUTS
    M2

    That way, your initial feedrate will always be whatever you program, until #501 is greater than 110pcs, and then machine will just stop at the first move.

    Granted, it's not elegant, but it's a quick and dirty fix.

  20. #20
    Join Date
    Apr 2005
    Location
    Beaverdam, Virginia
    Posts
    8,509
    Post Thanks / Like
    Likes (Given)
    1040
    Likes (Received)
    4236

    Default

    Quote Originally Posted by TeachMePlease View Post
    Hmmm.......


    Less elegant, but it works:


    BEGIN PROGRAM
    #502=100.0
    IF[#501 GT 110]
    #502=0.0

    FIRST MOVE
    G1 G98 X2.0 F#502

    PROGRAM GUTS
    M2

    That way, your initial feedrate will always be whatever you program, until #501 is greater than 110pcs, and then machine will just stop at the first move.

    Granted, it's not elegant, but it's a quick and dirty fix.
    M2 won't work, I have to use M99, M2 gets a program to rewind, but it stops and won't repeat. M99 will rewind & repeat. Will try again tomorrow, using M99 in place of M2.
    Last edited by Dualkit; 08-06-2020 at 05:13 AM.


Tags for this Thread

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
  •