What's new
What's new

Fanuc OT stopped counting with count code.

  • Thread starter Guest
  • Start date
  • Replies 19
  • Views 3,769
G

Guest

Guest
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:
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?
 
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.
 
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.
 
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
 
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.
 
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.
 
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:
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.
 
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.
 
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......
 
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.
 
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 :crazy:
 

Attachments

  • 20200804_184404.jpg
    20200804_184404.jpg
    100.2 KB · Views: 438
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.
 
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
 
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.
 
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.
 
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:








 
Back
Top