Haas CNC Lathe Help

See the below program. It goes thru and runs everything just fine and as it should all the way to the last part and the cut off cycle is to run. When it goes to run that we have the feeds and speeds set at F0.003 and S960. For some reason it is maintaining the S960 but the feed rate is barely crawling. If you stop the program and hit reset and start it at the cut off portion it runs at the correct feed and speed. Any ideas where its picking up the really slow feed rate at for that last cycle?

This is on a Haas SL30T machine.

Thanks for any help or advice....

Andy


O00226

T202 (2967-785 R&D)
(FACING)
G50 S2000 M31
G97 S509 M03
G96 S984 M08

G00 G54 Z0.05


G00 G54 X2.025 Z0.075 (TOTAL MAT. REMOVED FACE)
G72 G54 P101 Q102 D0.025 (DEPTOFCUT) U0. (ALLOWANCE ON X) W0.004 (ALLOWANCE ON Z) F0.006



N101 G00 Z0
G01 X-0.03
N102 G00 W0.1

G53 X0. Z-15




T1111 (BORING BAR)
G97 S800 M03
G00 G54 Z1.
G54 G00 X1. Z1. M08
G85 Z-2.6 R0.1 F0.008
G54 G00 X1.062 Z0.05
G85 Z-2.6 R0.1 F0.008
G54 G00 X1.101 Z0.05
G85 Z-2.6 R0.1 F0.008
G00 Z1.
G80 G54 X1.225 Z1. M09



T1111 (BORING BAR CHAMFER)
G97 S800 M03
G00 G54 Z1.
G54 G00 X1.225 Z0.05 M08
G01 X1.225 Z0. F0.003
G01 X1.125 Z-0.063 F0.002

G00 Z1.
G80 G53 X0. Z-15. M09




N100 (** Live Tooling Operation **)
G53 G00 X0 T0
G53 G00 Z-18. T0
T505 (T)

G98 (FPM)
M05
G00 G54 Z-1.25
G00 X2.03 M08
M133 P1500
M19 P270
M14

G75 X0.9 I0.05 F3.
G00 U0 Z1. M09
G97 S1200
G80 G00 G53 X0. Z-18.




T303 M08 (CUTT OFF)
G97 S960 M03
G00 G54 X2.05 Z-2.5

G75 G54 X0.95 I0.05 F0.003
G00 G53 X0. Z-18. M09




M30
%

Looks like you still have feed per minute on.

edit: I don't see another G96 either for the cutoff... (unless that is by design)

chevelless502 said:

O00226

T202 (2967-785 R&D)
(FACING)
G50 S2000 M31
G97 S509 M03
G96 S984 M08

G00 G54 Z0.05


G00 G54 X2.025 Z0.075 (TOTAL MAT. REMOVED FACE)
G72 G54 P101 Q102 D0.025 (DEPTOFCUT) U0. (ALLOWANCE ON X) W0.004 (ALLOWANCE ON Z) F0.006



N101 G00 Z0
G01 X-0.03
N102 G00 W0.1

G53 X0. Z-15




T1111 (BORING BAR)
G97 S800 M03
G00 G54 Z1.
G54 G00 X1. Z1. M08
G85 Z-2.6 R0.1 F0.008
G54 G00 X1.062 Z0.05
G85 Z-2.6 R0.1 F0.008
G54 G00 X1.101 Z0.05
G85 Z-2.6 R0.1 F0.008
G00 Z1.
G80 G54 X1.225 Z1. M09



T1111 (BORING BAR CHAMFER)
G97 S800 M03
G00 G54 Z1.
G54 G00 X1.225 Z0.05 M08
G01 X1.225 Z0. F0.003
G01 X1.125 Z-0.063 F0.002

G00 Z1.
G80 G53 X0. Z-15. M09




N100 (** Live Tooling Operation **)
G53 G00 X0 T0
G53 G00 Z-18. T0
T505 (T)

G98 (FPM)<
M05
G00 G54 Z-1.25
G00 X2.03 M08
M133 P1500
M19 P270
M14

G75 X0.9 I0.05 F3.
G00 U0 Z1. M09
G97 S1200
G80 G00 G53 X0. Z-18.




T303 M08 (CUTT OFF)
G97 S960 M03
Insert G99 for FPR here
G00 G54 X2.05 Z-2.5

G75 G54 X0.95 I0.05 F0.003
G00 G53 X0. Z-18. M09




M30
%

Click to expand...

It's a lathe so the default is going to be G99 after reset, but if you insert it into the program where indicated it will run fine.

R

Looking above, looks like you have some stuff in inches per minute, right? If you feed .003 per minute, going to be sorta slow..... Inch per rev might be mo' bettuh.....
(others beat me to it, got distracted during reply, and I type slow)

litlerob1 That fixed it. Thanks for the fast response and help!!

Andy