Rockwell Automation 8520-MUM 9/Series CNC Mill Operation and Programming Manual Documentation Set - Manual (Page 639)

Milling Fixed Cycles
Chapter 26
26-7
The following section provides a detailed explanation of each parameter
that can be programmed for the milling fixed cycles. Some of these
parameters are not valid with all cycles. Refer to the specific description
of each cycle in section 26.4. To alter milling cycle operation parameters,
refer to section 26.5.
We describe these milling fixed-cycle parameters below.
X__Y__Z__R__ I__J__K__ P__F__L__Q__D__S__;
Where : Is :
X,Y specifies the location of the hole position in the selected plane. In the absolute mode (G90), program
the hole position using the coordinate values in the active coordinate system. In incremental mode (G91),
program the hole position using the distance from the current tool position to the required hole position.
Z defines the hole bottom. In absolute mode (G90), program the hole bottom level using the coordinate
value in the active coordinate system. In the incremental mode (G91), program the distance from the R
point level to the hole bottom level.
R defines the R point level. In the absolute mode (G90), program the R point level as a coordinate value in
the active coordinate system. In the incremental mode (G91), program the R point level by the distance
from the initial point level to the R point level.
I, J, K,
or Q Q defines the infeed amount for each move made in the hole in G83; I, J, and K, or Q defines the shift
amount for G76 and G87.
P defines the dwell period at hole bottom. P programs the dwell in the same way as G04: seconds if in
feedrate mode (G94), spindle revolutions if in revolution mode (G95). (The allowable dwell time range in
seconds is 0.001-99999.99. The allowable dwell range in revolutions is also 0.001-99999.999.) The
P--word does not apply in all milling fixed cycles.
F defines the cutting feedrate. If this parameter is not specified, the control will use the currently active
feedrate for the cutting feedrate. For G74.1 and G84.1, F = tap thread lead in inches/mm per revolution.
L defines the number of times the milling fixed cycle is repeated. The maximum number of repeats is
9999.
• In absolute mode, the control drills in the same location the number of times specified by the L--word.
• In incremental mode, the L--word drills the number of holes specified by the L--word at equally spaced
positions, determined by axis positioning parameters X and Y.
• If an L0 is programmed, the control stores the milling cycle information but does not execute the drilling
cycle. If no L--word is programmed, the control defaults to L1.
Q In G83, Q defines the infeed amount for each move made in the hole.
In G86.1 and G87, Q defines the shift amount (as do I, J, and K).
In G74.1 and G84.1, Q defines the angle at which to orient the spindle before starting the tap. If you
don’t program the Q-word, the spindle is not oriented before the tap begins. This means that the hole is
not re-tappable unless a Q-word is programmed in the cycle block. The spindle is brought to a stop prior to
the initiation of the tapping phase even if Q is not programmed; this happens after the move to the
R-plane.
D defines the return spindle speed so that, if you want, the tap-out move can be performed faster or slower
than the tap-in. Tool selection by D-word is not possible while in the solid tapping mode.
S defines spindle speed in rpm.
26.3
Parameters