(too old to reply)
Parts Counter Help
Stan-O
2005-04-14 00:54:28 UTC
People

Is there a way to trip the parts counter on a looped program? I know
that M30 trips the counter, but what if i'm using a bar puller with a
M99. With the M99, the parts counter doesn't trip. I thought about
macros, but the M30 still has to be in there at some point.

Any help would be greatly appreciated.

Thanks
-S
D Murphy
2005-04-14 01:46:05 UTC
Post by Stan-O
People
Is there a way to trip the parts counter on a looped program? I know
that M30 trips the counter, but what if i'm using a bar puller with a
M99. With the M99, the parts counter doesn't trip. I thought about
macros, but the M30 still has to be in there at some point.
Any help would be greatly appreciated.
Depending on which control you have and if you have custom macro
(parametric programming) you coul add 1 to the system variable for the
parts counter every cycle. On a Fanuc it's 3901. So put this in the
program:

#3901=[#3901+1]

You can set the number of parts required in 3902. What I don't know is if
the parts counter reaching the parts required will stop your machine. That
depends on how the builder wrote the ladder. On some machines that I've
worked on the M30 command is also used to trip the parts count alarm. If
the machine does not stop you can create your own alarm.

#3901=[#3901+1]
IF[#3901 GE #3902] GOTO 9000
M99;
N9000
#3901=0
#3000=1(PARTS COUNTER COUNT UP)
--
Dan
Greg
2005-04-14 01:53:31 UTC
OTOH, M81 ?
Greg.
Post by Stan-O
People
Is there a way to trip the parts counter on a looped program? I know
that M30 trips the counter, but what if i'm using a bar puller with a
M99. With the M99, the parts counter doesn't trip. I thought about
macros, but the M30 still has to be in there at some point.
Any help would be greatly appreciated.
Thanks
-S
MachineTools
2005-04-14 01:55:01 UTC
Post by Stan-O
People
Is there a way to trip the parts counter on a looped program? I know
that M30 trips the counter, but what if i'm using a bar puller with a
M99. With the M99, the parts counter doesn't trip. I thought about
macros, but the M30 still has to be in there at some point.
Any help would be greatly appreciated.
Thanks
-S
what is your CNC ?
if you have a fanuc cnc, you can use other M-code to count, Read parameter
manaul.
6700 bit0 Set 1 .... use customer's M code , Not M30/02
6710 M code what you want
6711 Start No. for counting
6712 Total part No.
6713 part No. to cutting
good luck!
Matt Stawicki
2005-04-14 04:26:56 UTC
Post by Stan-O
People
Is there a way to trip the parts counter on a looped program? I know
that M30 trips the counter, but what if i'm using a bar puller with a
M99. With the M99, the parts counter doesn't trip. I thought about
macros, but the M30 still has to be in there at some point.
Any help would be greatly appreciated.
Thanks
-S
What control?

Have you tried M20?
That's a "one cycle stop" code that usually does not trip the counter,
but then M99 should and it doesn't. Never know, it may be worth a
shot.

You could also run your main program as a sub-program and tell it to
repeat ### times.

Matt
Anthony
2005-04-14 05:07:37 UTC
Post by Stan-O
People
Is there a way to trip the parts counter on a looped program? I know
that M30 trips the counter, but what if i'm using a bar puller with a
M99. With the M99, the parts counter doesn't trip. I thought about
macros, but the M30 still has to be in there at some point.
Any help would be greatly appreciated.
Thanks
-S
If it's a Mazak, put a M198 Q1 on the line before the M99.

If it's a Fanuc, see Dan's post.
If it's a Siemens, set up an R parameter to count (R100=R100+1), then Set
say R101=max #parts, and
If R100=R101 THEN GOTOF MARK 10
rest of program
M99
MARK 10
M30

(
--
Anthony

You can't 'idiot proof' anything....every time you try, they just make
better idiots.

Remove sp to reply via email
DanL
2005-04-14 10:28:12 UTC
Post by Stan-O
People
Is there a way to trip the parts counter on a looped program? I know
that M30 trips the counter, but what if i'm using a bar puller with a
M99. With the M99, the parts counter doesn't trip. I thought about
macros, but the M30 still has to be in there at some point.
Any help would be greatly appreciated.
Thanks
-S
We have a couple of machines with Fanuc controls in our shop that use the
following format:

M89 - somewhere near the top of the program increments the counter by one
each time the cycle is run.

/M99
M30 - Obviously the last two lines of the program

When the parts counter reaches the preset value it throws the block delete
allowing the program to run to M30 and stop. The parts counter is an option
on most Fanuc controls.


DanL
MachineTools
2005-04-14 23:02:00 UTC
on the other hand, MTB made new M code to restart a program.

O100
...
...
Mxxx(for restart program after M30);
M30

so, parts is counted by M30, Mxxx do restart a program like M99.
this M code is not a option. call your MTB.
Stan-O
2005-04-15 00:08:08 UTC
The machines are Hyundai with a fanuc 0T and 16T

I have not looked into the books yet, but i like the M89 Idea, it's
simple.

Thanks I'll give it a try.

-S
Stan-O
2005-04-15 00:08:11 UTC
The machines are Hyundai with a fanuc 0T and 16T

I have not looked into the books yet, but i like the M89 Idea, it's
simple.

Thanks I'll give it a try.

-S
Stan-O
2005-04-15 00:34:09 UTC
the problem is running a subprogram loop is i still can't tell how many
parts i have made. and i need to trip the counter, not the other.

-S
Stan-O
2005-04-15 00:34:20 UTC
the problem is running a subprogram loop is i still can't tell how many
parts i have made. and i need to trip the counter, not the other.

-S
Matt Stawicki
2005-04-15 15:31:39 UTC
Post by Stan-O
The machines are Hyundai with a fanuc 0T and 16T
I have not looked into the books yet, but i like the M89 Idea, it's
simple.
Thanks I'll give it a try.
-S
Stan,

There are a only a few M-codes that are reserved by Fanuc. Those are
M0, M1, M3, M30, M98, & M99. Any other M-codes, up to 3 digits, are
set by the OEM. M89 is only going to work if the OEM has configured
the control accordingly.

The Fanuc 0tt book shows that M2 and M30 advance the counter by 1.
Since M30 doesn't work, maybe M2 will.


Matt
Stan-O
2005-04-17 00:04:15 UTC
actually both machines are 0T, don't know what i was thinking, also
they do not have macro on them.

Any other ideas?

-S
Stan-O
2005-04-24 22:45:15 UTC
Got it working guys, the parameter 219 (M code for parts counter) was
set to 99, so I assume that it would loop before it caught the parts
counter. So I tried M89 and the machine did not like it, it would
kinda lock up, so i set both Hyndai's to M55, and it all works great!

Thanks guys

-S