Fanuc Part Counter

[DavidSV]

In my manual it says that a M95 will trip the part counter. I would like to use this while the program is in a loop to maintain counts. It doesn't seem to work. I put an M95 in and it does nothing to the part count. Does anyone know how to make a fanuc control trip the part counter without ending the program? I know Haas has a setting that trips the part counter at an M99.

 

David

[Gerry Badger]

Hello

 

I use G10. example G10 P5 U0.0001. wear offset 5 increases by 1 every time it it read. I put right before the M99. The "P" can be wear offset. Just aplly it to a tool that you are NOT using otherwise you will have problems. Hope this is helpful

 

Gerry

[DavidSV]

So then you use the wear offset to indicate how many parts have been ran.... I got you... I might have to try this some time.

[YoDoug®]

I use this at the end of programs in our Haas lathes, it should work in a Fanuc, Haas macro and Fanuc are almost the same. It adds 1 to the variable count every cycle then M99 until the desired count (16. in the example below). When it reaches the desired count it resets the variable to 0 and M30.

 

(PART COUNTER)

#599= [ #599 + 1 ]

G04 P1.

IF [ #599 EQ 16. ] GOTO100

IF [ #599 GT 16. ] GOTO100

M99

N100 #599= 0

M30

[Gerry Badger]

yup

 

i have a job going in our little lathe, in the main prgm, just before the M98 i have G10 P5 W0.0001; this counts the # of 6 foot lengths done and then in the sub prgm G10 P5 U0.0001; this counts my total parts. I found out the "hard" way that it will only work up to 5000 pcs or 0.5000 in the offset. Nothing crashed or wrecked, just scratched my head for a while and the zeroed out the 0.5000 and then holy cow, back in business. enjoy the day

 

Gerry

[DavidSV]

Doug,

 

Where do you go to read the #599? I have never used a macro before, so I want to be sure that everything before I try.

[YoDoug®]

David, We only have Haas machines here. Our Fanuc controlled machines are in China so I can't look at one right this moment

 

I am sure one of our resident forum Fanuc guys can tell you where to check variables in the controller.

[Charlie Pierson]

if you have custom macro then you could read #599 by looking at the variable page or you can use #599 in a test statement such as : IF [#599 LE 212O] GOTO 345

 

or

WHILE [#599 LE 2125] DO 1

|

|

|

#599=[#599+1]

END 1

 

If you have a Fanuc control , check in the operators manual, programming section, for Custom Macro B and learn it from there

[GoetzInd]

There is usally a parameter to tell the parts count to trip on M99 or M55. You might just want to try m55 instead of m99.

 

Mike

[DavidSV]

I found where to read the variable number from. I just wrote:

 

#500=[#500+1]

 

It works for what I need it to do.

 

The macros look very interesting. I can think of several programs we have where I can use a macro to count cycles for certain tools.

 

Charlie,

How would you use the WHILE statement like above? For what purpose?

 

Thanks

David

[YoDoug®]

once you understand Macro B a whole world of possibilities opens to you.

[Tom Dorgan from American Precision]

My 18i controls use #3901 to set the counter & I chose to use Variable #104 to load the counter.

I have this at start of program

#104=#3901

N2 G20

N4 G0 G17 G90 G40 G49 G80 G90

I use this code at end of program

#104=#104+1

N600 G94 G04 X.5

#3901=#104

N602 M00

/GOTO10

N604 M20

N606 M5

#104=#104-1

#3901=#104

N608 M30

The purpose is so that it counts while it is in the loop but when you skip the loop and go to the M30, it will add 1 to the counter when it reads the M30 so I subtract 1 before that so the count stays correct.

[DavidSV]

Where did you find out where the control stores the part count number. I am using a Leadwell with a Fanuc 0i-MC control.

 

Thanks

David

[robk]

David, please check your mailbox

[Goldorak]

Here , fanuc 18T , simply put a M90

 

it will increase part counter