Fanuc 18T peck drill cycle

[Mark Storkamp]

I'm converting a program from one style Fanuc control to an 18T (don't have
a programming manual for it) and don't know how to program a peck drill
cycle.

A sample threading cycle (the only canned cycle I've got any notes on):

G76 P021060 Q0035 R0010
G76 X1.593 Z-0.43 P0440 Q0050 F0.076923

If this looks familiar to someone, can you please tell me how to program the
following drill cycle on this control:

G74 X0 Z-1.120 D.2 L.2 F.004 E.5

Thanks.

[Bill Roberto]

Post by Mark Storkamp
I'm converting a program from one style Fanuc control to an 18T (don't have
a programming manual for it) and don't know how to program a peck drill
cycle.
G76 P021060 Q0035 R0010
G76 X1.593 Z-0.43 P0440 Q0050 F0.076923
If this looks familiar to someone, can you please tell me how to program the
G74 X0 Z-1.120 D.2 L.2 F.004 E.5
Thanks.
--
Mark

G74 R.01
G74 X0 Z-1.12 Q2000 F.004

The 18T is double line execution, your example is single line execution. I
am not sure of the L or the E variable, but the D is peck increment. In
double line execution Q is the peck increment, and you have to use the 4
place numeric system not decimals. The drill cycle can also be an axial
groove cycle. P is the step over amount in X.

[ff]

Post by Bill Roberto

Post by Mark Storkamp
I'm converting a program from one style Fanuc control to an 18T (don't

have

Post by Mark Storkamp
a programming manual for it) and don't know how to program a peck drill
cycle.
G76 P021060 Q0035 R0010
G76 X1.593 Z-0.43 P0440 Q0050 F0.076923
If this looks familiar to someone, can you please tell me how to program

the

Post by Mark Storkamp
G74 X0 Z-1.120 D.2 L.2 F.004 E.5
Thanks.
--
Mark

G74 R.01
G74 X0 Z-1.12 Q2000 F.004
The 18T is double line execution, your example is single line execution. I
am not sure of the L or the E variable, but the D is peck increment. In
double line execution Q is the peck increment, and you have to use the 4
place numeric system not decimals. The drill cycle can also be an axial
groove cycle. P is the step over amount in X.

The G74 command line given by the OP looks like an Okuma drill cycle where:
The G74 command signals the start of the drilling cycle. The Z
value is the depth value, the D value is the dwell increment (for chip
break), the L value is the retraction increment (clearance for the
broken chips), the F value is the feedreate in inches per revolution
(IPR), and the E value is the dwell time (in seconds).

ff