Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 558)

Grooving/Cutoff Cycles
Chapter 23
23-4
The format for this cycle is:
G76X__Z__I__K__F__D__;
Where : Is :
X__ the location where the last groove is cut. If only one groove is to be cut do not
program X. This may be programmed as either an incremental or absolute value.
Remember that its value is also affected by diameter or radius modes (G07 and
G08).
Z__ the total depth of the groove from the Z coordinate position of the tool prior to the
execution of the G76 block. If this cycle is to be used as a cut off cycle the depth
programmed here should drive the tool through the face of the part. This value
represents the location of the bottom of the groove cut. This may be
programmed as either an incremental or absolute value.
I__ the distance between each groove. If the distance between the location of the
last groove (programmed with X) and the next to the last groove is less than the
value programmed with I, then the I value is not used to determine the position of
the last groove. The last groove is always cut at the location programmed with
X. The I parameter is always programmed as an incremental, radius value
regardless of the current mode of the control.
K__ the amount that the cutting tool infeeds into the workpiece with each step. The
step is followed by a retract of amount e (set in AMP by the system installer).
The cutting tool then infeeds into the workpiece an amount K + e, retracts an
amount e, infeeds K + e, retracts e, etc. This repeats until the total
programmed depth of the groove Z is reached. When this depth is reached the
cutting tool stops infeeding and either shifts an amount D (if programmed) or
retracts to the starting coordinate at rapid feedrate. The K-word is always
programmed as an incremental value regardless of the current mode of the
control.
F__ the desired feedrate for the grooving infeed moves. The value entered with this
parameter replaces the currently active feedrate. It is optional in the grooving
block. If F is not programmed the currently active feedrate is used.
D__ the size of the incremental shift move made by the tool when the full depth of a
cut off has been reached. This parameter must be programmed even if its value
is zero when not using this cycle as a cutoff. A value other than zero is assigned
to D only if the grooving cycle is being used as a cut off cycle. It is always an
incremental value regardless of the current mode. The sign of the value
programmed with the D parameter determines the shift direction and should
move the tool away from the part. Programming this shift move helps to provide
a good finish since the cutting tool is not touching the part when it is retracted at
the rapid feedrate.
CAUTION: The shift programmed with a D parameter is
executed as a rapid move. Make sure that the cutting tool is
clear to shift at the end of the grooving cycle.