canned cycle for lathe with fanuc control

[JPann]

Can someone give me an example for turning an o.d and/ or id. using canned text?

[Kookaburra]

Depending on your control the normal calls are:
G70 (Finishing Cycle)
G71 (OD or ID turning cycle)
G72 (Facing Cycle)

Depending on your control the cycles are sometimes different in their build up.

Fanuc 6T Cycle Line requires a one line cycle as follows:

G71 P1 Q7 D4000 R2.0 U0.5 W0.2 F0.1

G71 - Is the cycle type
P1 - is the first profile line sequence number
Q7 - is the last prifile line sequence number
D4000 - is the depth of cut in microns
R2.0 - is the clearance of the X axis when rapid traversing back for the next cut in mm
U0.5 - is the amount of material to be left on the OD (X) incremental
W0.2 - is the material to be left on the shoulders (Z) incremental
F0.1 - is the feed rate (either in mm/rev or mm/min depending on your feed type)

On later controls a two line cycle is required as follows:

G71 U4.0 R2.0
G71 P1 Q7 F0.1 U0.5 W0.2

LINE 1

G71 - Is the cycle type
U4.0 - is the depth of cut in mm
R2.0 - is the clearance of the X axis when rapid traversing back for the next cut in mm
F0.1 - is the feed rate (either in mm/rev or mm/min depending on your feed type)

LINE 2

G71 - Is the cycle type
P1 - is the first profile line sequence number
Q7 - is the last prifile line sequence number
U0.5 - is the amount of material to be left on the OD (X) incremental
W0.2 - is the material to be left on the shoulders (Z) incremental

Excuse me for being a metric type person.

You must first move to your start position eg: Z clearance from the face of you billet and X to the outside diameter of your billet.

I might be a bit rusty here as it was a while ago but it is something like this->>

ONE LINE CYCLE (Fanuc 6T)

Billet diameter is 80mm

G0 X80.0 Z2.0 (Start Position before commanding the cycle)
G71 P1 Q7 D4000 R2.0 U0.5 W0.2 F0.1
N1 G0 X32.0
N2 G1 Z0.0
N3 G1 X40.0 Z-4.0
N4 G1 Z-30.0
N5 G1 X60.0 Z-60.0
N6 G1 Z-75.0
N7 G1 X80.0
G70 P1 Q7 F0.02 (This line is optional - If you command this line after the roughing cycle it will read sequence number N1 - N7 and do one complete finish profile cut)


TWO LINE CYCLE

Billet diameter is 80mm

G0 X80.0 Z2.0 (Start Position before commanding the cycle)
G71 U4.0 R2.0
G71 P1 Q7 F0.1 U0.5 W0.2
N1 G0 X32.0
N2 G1 Z0.0
N3 G1 X40.0 Z-4.0
N4 G1 Z-30.0
N5 G1 X60.0 Z-60.0
N6 G1 Z-75.0
N7 G1 X80.0
G70 P1 Q7 F0.02 (This line is optional - If you command this line after the roughing cycle it will read sequence number N1 - N7 and do one complete finish profile cut)

The build up of an ID profile is the same but you start at your drill hole diameter prior to executing the cycle and your R, U and W figures are negitive figures.

I hope this helps

[extrem89]

N1(ROUGH AND FINISH TURN CYCLE)
G97 S2500 M13
M98 P1
T0101
G50 S5500
G96 S1000
G0 X.550 Z.050
G71 U.060 R.010
G71 P21 Q22 U.030 W.005 F.008
N21 G0 X0
G1 G99 Z0 F.OO8
X.375 C-.015 F.003
Z-1.250 F.005
N22 X.550
G70 P21 Q22 (Finish cycle)
M98P1
M1
M30

[CNC PGMR]

Need help with a G71 canned cycle.
When I program the part to leave .08 stock in X & Z, part is cutting .08 too small.

[CNCRim]

Originally Posted by CNC PGMR Need help with a G71 canned cycle. When I program the part to leave .08 stock in X & Z, part is cutting .08 too small.

The post is 5 years old, what is your program look like post it on here.

[g-codeguy]

Originally Posted by CNCRim The post is 5 years old, what is your program look like post it on here.

Either he figured it out or doesn't want our help.

Probably was trying to leave .08 stock boring without the minus sign.

One of the reasons I don't visit the machining sites very often anymore, is you offer help, and never get a reply. Did it work? Still having a problem? Personally I like to know if my suggestions helped or not. I'm not looking for a pat on the back if they work, I just want to know if they got the job running okay. If my suggestion didn't work, then what did they have to do to get the job running? I like learning myself. It should be a 2-way street. I offer a suggestion. It works. Fine. It doesn't, but you found out what was needed to make it run, then share that information. Maybe I can use it later.

[tanvon]

Originally Posted by JPann Can someone give me an example for turning an o.d and/ or id. using canned text?

hi, this blog post might help you CNC Blog | CNC Cycle G72 or Facing Cycle for Fanuc CNC Machine Control with CNC Programming Example*|*CNC Blog