deep grooving

[eject_21]

Im having good luck pecking my partoff tool, feeding down .100, then retracting .005, feeding down another .100, and so on. Right now, Im typing it in at the machine.There has to be a G-code for this, Deep drilling in X instead of Z,? or, deep grooving. Like: G?? X-.032 D1000 U.005 R0 F.003:??? help please.(Fanuc control, Hwacheon lathe) I only want to retract .005 to break the chip, I dont want to retract all the way out of the part. Any help would be greatly appreciated.

[DAFISHER]

try using your drill peck cycle for mori seiki its g74 x is depth k for amt of peck
r for back off

x1.25 y1. position move
g74 x1.2k.100r.05 f.005 canned groove cycle

[g-codeguy]

On machines in my shop a G74 is for drilling or face grooving. G75 is the cycle for o.d. grooving, c-o, live tool radial drilling, etc.

There are 2 different formats depending on age of machine. Newer ons all use a 2-block format.

G75R.005
G75X-.02Z(OPTIONAL)P1000F.0025

R-value is the retract amount. P-value is the DOC before retracting. Example would peck .1 deep before retracting .005. Making P-value smaller increases cycle time, but breaks chips up better if they are causing a problem. On some internal grooves, I've made the peck depth less than the feedrate for maximum chip breaking.

Older machines use a 1-block call. It has been a while since I programmed one of them so I won't give an example for fear it might not be right. It is similar to your example. I will give you the exact format Tuesday when I get back to work. HTH

[eject_21]

G75 X0 I500 F.002:
Works, retract for G74 and G75 are set with the same parameter.