CL2000 FANUC CONTROL TURNING CYCLE PROBLEM

[cutshaw]

I run and im trying to get the turning to operate correctly on a CL2000 turning center,,but when I try to get the program line to run I either get a formatt error or a g-code error,,the g-code I can can figure out ,but dont understand the formatt error,,this works fine on the older mori seiki sl-3 turning center,,heres the program line I used,,

GO T0101;
G50 S1800;
G97 S2500 M03;
G0 X1.4 Z0 M08; { THIS STARTS ABOVE THE PART }
G01 X-.03 F.008;
G0 Z.03;
X1.4;
G71 P10 Q20 U.10 W0.01 D250 F.010 ; { I HAVE TRIED DIFFERENT G-CODES LIKE G72 G74 ,BUT NOTHING,,THE PROGRAM BOOK FOR THIS MACHINE SAYS THE FIXED TURNING CYCLE IS G71,,SO I THINK IT HAS THE BE THE PROGRAM LINE } { PLUS THE FORMATT ERROR OCCURS AT THE G71 LINE }

N10 G0 X.740 ; { START OF BREAKING CHAMFER }
G01 Z0 F.010 ;
X1.0 Z-.015 ; { FINISH 0.D }
Z-.450 ; { TURN STEP }
X1.200 ;
X1.250 Z-.490 ; { BREAKING CHAMFER }
Z-.625 ;
X1.400 ;
N20 X1.4 ;
G0 X8.0 Z8.0 M09 ;
M01;

This is how I thought it was for this machine,,please help anyway you can ,,,thx Eric

[cncsdr]

Change your 250 to .250 if you want quarter in cause g71 is inches 72 is metric.
worth a shot.

[BlueChip]

The canned cycle ... depending on the model Fanuc control ... can either be a 1 line or 2 line command.

Your older SL-3 ... is it a Fanuc 6T control by chance? ... that model uses a the 1 line command. If the other machine is a 0T or similar, it uses a 2 line command.

Not sure if this is it but you might want to check the model of the control and the correct format.

Hope this helps ...

Real World Machine Shop Software ... since 1986 ... at
www.KentechInc.com

Just on case this is true ... here some additional info on the 2 line command for G71

1st Line : G71 U (depth of cut - radius dim. ) R (retract amount )
2nd Line : G71 Pxxxx Qxxxx Uxxx Wxxx Fxxx
The addresses in the 2nd line are the same as in the single line format.

[g-codeguy]

Change your 250 to .250 if you want quarter in cause g71 is inches 72 is metric.
worth a shot.

No it's not. G71 is canned turning cycle, G72 is canned facing cycle.

EDIT: D250 would be .025, but pretty sure D doesn't use a decimal point tho I would have to look that up to be 100% certain as all the lathes I program for use the 2-block call.