Newbie- Fanuc 0TC, drilling, newbie

[emonje]

I'm new to Fanuc lathes, just starting with this Ajax with Fanuc 0T-C. For drilling at the end face of a stock I put like this (in mm):

G74 R1.0
G74 Z-20 Q5 F150.0

The drill retracts 1.0 mm from bottom of the hole each time, but I need it to retract to 1.0 mm from end face of the stock where I have set Z zero.
In milling I use G83 to retract entirely out of hole after each peck. Can I use G83 on lathe in similar manner?
I will have to work the machine tomorrow and very little time for experiment. Can anyone please help me out?

[dcoupar]

G83 is an option but it may be turned on in your control... worth a try.

G00 X0 Z1.
G83 Z-20. R0 Q5 F150.

Q = .005mm in this example
R is incremental on T series

[stevo1]

Do the lathes not have a G-code like the machining centers to retract to the R-plane or initial level (G98,G99) I know they are fpm and fpr on the lathes.

Stevo

[Perfect Circle]

Here are some samples drilling a hole with diff. controls.

(Fanuc0T) "inches"
O0001
(JOB 1 DRILLING CYCLE )
(TOOL #7 1.000 dia )
G80 G93 G40 G54 G18
T0707 M06
M40
G50 S400
G97 S400 M04
M08
G00 X0. Z.1
G74 R.1
G74 Q.2 E.1 V.1 R.1 Z-3. P0 F.01
M01
M09
G00 Z5.
G00 X10.
M05
M30
(Fanuc0iTC)"MM"
%
O00001 (PROGRAM NUMBER)
(PROGRAM START - TURNING CYCLES)
(PROGRAM NAME - CNCZONE.NC)
(POST - FANUC 0iTC metric)
(DATE - FRI. 12/03/2010)
(TIME - 12:59PM)
N01 G18 G21 G40 G80 G90 G98
(JOB 1 DRILLING CYCLE )
(TOOL #7 1.000 dia )
N02 T0707 G54 M43 M42 (MANAULLY EDIT GEAR RANGE)
N03 G50 S400
N04 G97 S400 M04
N05 G00 X0. Z.1 M08
(DRILL FACE - G74)
N06 G74 R.1
N07 G74 X0. Z-3. P0. Q.2 R0. F.01
N08 G40
N09 X5. Z5.
N10 X0.
N11 X5.
N12 M09
N13 M05
N14 G28 U0. W0.
N15 M30
%
(Fanuc0iT)"inches"
%
O00001 ( PROGRAM NUMBER )
( PROGRAM START - TURNING CYCLES )
( PROGRAM NAME: CNCZONE.NC)
( POST: FANUC 0iT )
( DATE: FRI. 12/03/2010)
( TIME: 01:00PM)
N01 G99 G90 G80 G40 G20
N02 G00 G28 U0. W0.
(JOB 1 DRILLING CYCLE )
(TOOL #7 1.000 dia )
N03 G54 G97 T0707 M04
N04 G50 S400
N05 G97 S400
N06 G00 X0. Z.1 M08
N07 G74 R.1
N08 G74 X0. Z-3. I0. K.2 R0. F.01
N09M09
N10 G97
N11 T0700
N12 M01
N13 G00 Z5.
N14 X5.
N15 M05
N16 G28 U0. W0.
N17 M30
%
(Fanuc0T)"MM"
%
O00001 (PROGRAM NUMBER)
(PROGRAM START - TURNING CYCLES)
(PROGRAM NAME - CNCZONE.NC)
(POST - FANUC 0T metric)
(DATE - FRI. 12/03/2010)
(TIME - 01:04PM)
N01 G18 G21 G40 G80 G90 G98
N02 G00 G28 U0. W0.
(JOB 1 DRILLING CYCLE )
(TOOL #7 1.000 dia )
N03 T0707
N04 M01
N05 G50 S400
N06 G97 M04
N07 G54 X0. Z.1 M08
N08 G97 S400
(DRILL FACE - G74)
N09 G74 R.1
N10 G74 X0. Z-3. P0. Q.2 R0. F.01
N11 G40
N12 X5. Z5.
N13 G97
N14 T0700
N15 X0.
N16 X5.
N17 M09
N18 M05
N19 G28 U0. W0.
(END OF PROGRAM)
N20 M30
%
Hope that all that can help you in some way...
Good Luck~!

[Perfect Circle]

I'm sorry for all the space being used ...
I almost forgot this info...

Standard Drill cycle live tool face "G81"
Peck drill cycle live tool face "G83"
High speed peck cycle live tool face "G83"
Tap cycle live tool face "G84"
Boring cycle 1 live tool face "G85"
Boring cycle 2 live tool face "G86"
Boring cycle 3 live tool face "G89"

Standard Drill cycle live tool diameter "G81"
Peck drill cycle live tool diameter "G83"
High speed peck cycle live tool diameter "G83"
Tap cycle live tool diameter "G84"
Boring cycle 1 live tool diameter "G85"
Boring cycle 2 live tool diameter "G86"
Boring cycle 3 live tool diameter "G89"

[dcoupar]

Originally Posted by stevo1 Do the lathes not have a G-code like the machining centers to retract to the R-plane or initial level (G98,G99) I know they are fpm and fpr on the lathes. Stevo

No, they don't. I believe the intended use for G98/G99 on a mill was to jump over obstructions between holes. I guess there's not much use for that on a lathe.