Sample Lathe Programs For Fanuc 10T

[metx]

Could someone please post a couple of simple lathe programs in Fanuc 10T.
I have been programming a Tsugami Mercury with a 6T for years and I now have another lathe to use only it has a 10TF. I don't care to learn the convesational side of it but hope to be able to program it with G code.
I have been using G50 like a G92 with the tool X and Y position at the beginning of the program and always send the tool back to this position before a tool change and then on the next tool G50 again and so on.
This is the way I was shown to program but believe there may be a better way by using the offsets to load my tool home position in and then a G28 at the end of the program? On my new lathe G50 is not for tool presets but for max speed.
Any help would be greatly appreciated.
Thank you,
Keith

Similar Threads:

• Bug in sample programs
• Need Help!- Fanuc T14IA Robodrill Need Sample Programs
• Citizen E32J Fanuc 6T sample programs
• Fanuc oi Mate-TC Lathe (Sample Program)
• Any Sample programs with live tooling for Daewoo 700 with Fanuc 18i

[DryRun]

here is a program that will run on a 10t
O1586
(SUB PROGRAM# 1200)
G54
G28U0W0
G50S1500
G40G20G80G99
M41
N1T0101(ROUGH TURN)
G97S559M3
G54
G0X4.65Z0M8
G96S650M3
G1X1.25F.005
G0Z.1
X4.6
G71P50Q60U.015W.002D0500F.014
N50G0X2.75Z.1
G1Z-.1155
X4.44
X4.5Z-.1455
Z-1.
X4.65
N60
G0Z.1
M9
G97S1000M3
G28U0W0
M01
N3T0303(FINISH TURN)
G97S1107M3
G54
G0X2.71Z.1M8
G96S750M3
G1Z0F.01
G1X2.75Z-.02F.0025
G1Z-.1155F.0035
X4.44
X4.5Z-.1455
Z-1.
X4.6
G0Z.1
M9
G97S1000M3
M01
N6T0606(BORE)
G97S1385M3
G54
G0X1.3Z.1M8
G71P10Q20U0W0D0500F.012
N10G0X2.14Z.1
G1Z0
G1X1.84Z-.15
Z-2.45
X1.25
N20
G0Z.1
M9
G97S1000M3
G28U0W0
M00

(FLIP PART)

N21T0101(ROUGH TURN 2.756 O.D.)
G97S559M3
G55
G0X4.65Z0M8
G1X1.25F.005
G0Z.1
X4.6
G71P55Q65U.015W.002D0500F.014
N55X2.756Z.1
Z-1.526
X4.65
N65
G0Z.1
M9
G97S1000M3
M01
N23T0303(FINISH TURN)
G97S11136M3
G55
G0X2.696Z.1M8
G96S750M3
G1Z0F.01
G1X2.756Z-.03F.0025
G1Z-1.526F.0035
X4.44
X4.5Z-1.556
X4.65
G0Z.1
M9
G97S1000M3
M01
N26T0606(BORE)
G97S1000M3
G55
G0X2.14Z.1M8
G1Z0F.01
G1X1.875Z-.136F.0015
G1Z-2.5F.005
X1.8
G0Z.1
M9
M5
G28U0W0
M01
N2T0202(16-4 B THREAD)
M40
G97S45M4
G55
G0X1.8Z.25M8
G04P2000
M98P1200
G0X1.8Z.5
M98P1200
G0X1.8Z.75
M98P1200
G0X1.8Z1.
M98P1200
G0X1.8Z1.25
M98P1200
G0X1.8Z1.5
M98P1200
G0X1.8Z1.75
M98P1200
G0X1.8Z2.
M98P1200
G0X1.8Z2.25
M98P1200
G0X1.8Z2.5
M98P1200
G0X1.8Z2.75
M98P1200
G0X1.8Z3.
M98P1200
G0X1.8Z3.25
M98P1200
G0X1.8Z3.5
M98P1200
G0X1.8Z3.75
M98P1200
G0X1.8Z4.
M98P1200
M9
M5
G28U0
G28W0
M01
N36T0606(DEBURR)
M40
G97S1000M3
G55
G0X2.14Z.1M8
G1Z0F.01
G1X1.877Z-.136F.0025
G1Z-2.5F.008
X1.8
G0Z.1
M9
M5
G28U0W0
M30

[metx]

Thank you for the example. There are some G codes in it I am not familiar with. G54-G55. I assume these are work shift offsets? I ordered a book for my 10TF and it has the conversational programming in it. I am waiting for the 10TA manual to get here. It is supposed to be for the G code programming side of this control. Hopefully it will help me understand these new(to me) codes and show me how to enter them in the control. What is the purpose of the G28 U0W0 block right after the G54 block at the beginning of the program? I know these must be easy questions for you but please bear with me.
Thanks,
Keith

[Dave Mc]

Hi I run a DSG with 10TF control and from memory G54 / G55 are used as additional workshift commands called within the program. If you need more info let me know and I will check my manuals, its not a function I have used in recent times. I would be happy to assist with your questions if i can.
I agree with your comments on the FAPT system, nice for a salesman but not much use in the shop, we always program direct with G code.

[g-codeguy]

here is a program that will run on a 10t
O1586
(SUB PROGRAM# 1200)
G54
G28U0W0
G50S1500
G40G20G80G99
M41
N1T0101(ROUGH TURN)
G97S559M3
G54
G0X4.65Z0M8
G96S650M3
G1X1.25F.005
G0Z.1
X4.6
G71P50Q60U.015W.002D0500F.014
N50G0X2.75Z.1
G1Z-.1155
X4.44
X4.5Z-.1455
Z-1.
X4.65
N60
G0Z.1
M9
G97S1000M3
G28U0W0
M01
N3T0303(FINISH TURN)
G97S1107M3
G54
G0X2.71Z.1M8
G96S750M3
G1Z0F.01
G1X2.75Z-.02F.0025
G1Z-.1155F.0035
X4.44
X4.5Z-.1455
Z-1.
X4.6
G0Z.1
M9
G97S1000M3
M01
N6T0606(BORE)
G97S1385M3
G54
G0X1.3Z.1M8
G71P10Q20U0W0D0500F.012
N10G0X2.14Z.1
G1Z0
G1X1.84Z-.15
Z-2.45
X1.25
N20
G0Z.1
M9
G97S1000M3
G28U0W0
M00

(FLIP PART)

N21T0101(ROUGH TURN 2.756 O.D.)
G97S559M3
G55
G0X4.65Z0M8
G1X1.25F.005
G0Z.1
X4.6
G71P55Q65U.015W.002D0500F.014
N55X2.756Z.1
Z-1.526
X4.65
N65
G0Z.1
M9
G97S1000M3
M01
N23T0303(FINISH TURN)
G97S11136M3
G55
G0X2.696Z.1M8
G96S750M3
G1Z0F.01
G1X2.756Z-.03F.0025
G1Z-1.526F.0035
X4.44
X4.5Z-1.556
X4.65
G0Z.1
M9
G97S1000M3
M01
N26T0606(BORE)
G97S1000M3
G55
G0X2.14Z.1M8
G1Z0F.01
G1X1.875Z-.136F.0015
G1Z-2.5F.005
X1.8
G0Z.1
M9
M5
G28U0W0
M01
N2T0202(16-4 B THREAD)
M40
G97S45M4
G55
G0X1.8Z.25M8
G04P2000
M98P1200
G0X1.8Z.5
M98P1200
G0X1.8Z.75
M98P1200
G0X1.8Z1.
M98P1200
G0X1.8Z1.25
M98P1200
G0X1.8Z1.5
M98P1200
G0X1.8Z1.75
M98P1200
G0X1.8Z2.
M98P1200
G0X1.8Z2.25
M98P1200
G0X1.8Z2.5
M98P1200
G0X1.8Z2.75
M98P1200
G0X1.8Z3.
M98P1200
G0X1.8Z3.25
M98P1200
G0X1.8Z3.5
M98P1200
G0X1.8Z3.75
M98P1200
G0X1.8Z4.
M98P1200
M9
M5
G28U0
G28W0
M01
N36T0606(DEBURR)
M40
G97S1000M3
G55
G0X2.14Z.1M8
G1Z0F.01
G1X1.877Z-.136F.0025
G1Z-2.5F.008
X1.8
G0Z.1
M9
M5
G28U0W0
M30

And here it is with a few liberties taken. Don't know your machine, but it should still run. Your 2nd rough turn should have alarmed because you need a G-code in the N55 block. G54-G55-G1 are modal. U0W0 are understood. Also many machines will run with a G1 in place of the G0 in the canned G71-G72 cycles, and that is what I use because of the shallow DOCs I take (similar to your cuts). Assumed material 4.6 diameter based on your 1st approach. Personally I wouldn't finish face with my roughing tool. Can you depend on your operators to maintain the .1455 depth? I can't. What kind of material is it, and how critical is the finish on the face? I also swing a small radius on all chamfers to push the burr ahead of the insert. Looks like it is a thru bore. No idea what your 1200 subprogram looks like. Although I have threaded using a subprogram, I have never seen anything like your cycle. A 4 inch start is a lot of lead. I would be interested in seeing your 1200 subprogram. M3s on G96 blocks aren't needed unless you eliminate the G97 block. Added G96 to your rough bore. I see the chamfer move at the 4.5 diameter is .03 x 45 deg. & that the front chamfer is a nice round .02 move. Did you allow for tool compensation?

O1586
(SUB PROGRAM #1200)
G28U0W0
G50S1500
G40G20G80G99M41
N1G54T0101(ROUGH TURN)
G97S559M3
G0X4.65Z0M8
G96S650
G1X1.25F.005
G0X4.6Z.03
G71P50Q60U.015W.002D500F.014
N50G0X2.75
G1Z-.1155
X4.44
X4.5Z-.1455
N60Z-1.
G97S1000M9
G28W0
M1
N3T0303(FINISH TURN)
G97S1107M3
G0X2.71Z.1M8
G96S750
G1Z0F.01
X2.75Z-.02F.0025
Z-.1155F.0035
X4.44
X4.5Z-.1455
Z-1.
X4.53
G0G97Z1.S1000M9
G28W0
M1
N6T0606(BORE)
G97S1385M3
G0X1.3Z1.M8
G96S600
Z.03
G71P10Q20D500F.012
N10G0X2.14
G1Z0
X1.84Z-.15
N20Z-2.45
G97Z1.S700M9
G28U0W0S50
M0

(FLIP PART)

N21G55T0101(ROUGH TURN 2.756 O.D.)
G97S559M3
G0X4.65Z0M8
G1X1.25F.005
G0X4.6Z.03
G71P55Q65U.015W.002D500F.014
N55G0X2.756
N65G1Z-1.526
G97S1000M9
G28W0
M1
N23T0303(FINISH TURN)
G97S11136M3
G0X2.696Z.1M8
G96S750
G1Z0F.01
X2.756Z-.03F.0025
Z-1.526F.0035
X4.44
X4.5Z-1.556
U.004W-.02
G0G97Z1.S1000M9
G28W0
M1
N26T0606(BORE)
G97S1000M3
G0X2.14Z.1M8
G1Z0F.01
X1.875Z-.136F.0015
G1Z-2.5F.005
X1.8 M9
G0Z.1
G28U0W0M5
M1
N2T0202(16-4 B THREAD)
M40
G97S45M4
G0X1.8Z.25M8
G4P2000
M98P1200
G0X1.8Z.5
M98P1200
G0X1.8Z.75
M98P1200
G0X1.8Z1.
M98P1200
G0X1.8Z1.25
M98P1200
G0X1.8Z1.5
M98P1200
G0X1.8Z1.75
M98P1200
G0X1.8Z2.
M98P1200
G0X1.8Z2.25
M98P1200
G0X1.8Z2.5
M98P1200
G0X1.8Z2.75
M98P1200
G0X1.8Z3.
M98P1200
G0X1.8Z3.25
M98P1200
G0X1.8Z3.5
M98P1200
G0X1.8Z3.75
M98P1200
G0X1.8Z4.
M98P1200
M9
G28W0M5
M1
N36T0606(DEBURR)
M40
G97S1500M3
G0X2.14Z.1M8
G1Z0F.01
X1.875Z-.136F.0025
Z-2.5F.008
X1.84F.03M9
G0Z1.S100
G28U0W0M5
M30

[mosesooi]

mosesooi,
I have a moriseiki cnc c/w Fanuc 10T controller,could someone tell me which parameter
to change,so that i don't have to key X-axis in negative sign after work coordinate had
been determined.
Thanks.

[g-codeguy]

mosesooi, try calling Fanuc at 1-800-433-2682. I beleve this number still works. They should give you the parameter without any questions.

Remember that changing this parameter will reverse G-codes for arcs.