F - Feedrate
*I - Shift value along the X Axis before retracting, if Q
is not specified
*J - Shift value along the Y Axis before retracting, if Q
is not specified
*L - Number of holes to bore if G91 (Incremental Mode) is
*Q - The shift value, always incremental
*R - Position of the R plane
*X - X-Axis location of hole
*Y - Y-Axis location of hole
*Z - Z-Axis position to cut to
* indicates optional
caution: Unless you specify otherwise, this canned cycle uses the most recently
commanded spindle direction (M03, M04, or
M05). If the program did not specify a spindle direction before it
commands this canned cycle, the default is M03 (clockwise). If you
command M05, the canned cycle will run as a “no-spin” cycle. This lets
you run applications with self-driven tools, but it can also cause a crash. Be sure of
the spindle direction command when you use this canned cycle.
In addition to boring the hole, this cycle shifts the X and Y Axis before and after
the cut, to clear the tool while it enters and exits the workpiece (refer to
G76 for an example of a shift move). Setting 27 defines the shift
direction. If you do not specify a Q value, the control uses the
optional I and J values to determine the shift
direction and distance.
G77 Back Boring Canned Cycle Example
O60077 (G77 CYCLE-WORKPIECE IS 1.0" THICK) ;
T5 M06 (BACK COUNTERBORE TOOL) ;
G90 G54 G00 X0 Y0 (INITIAL POSITION) ;
S1200 M03 (SPINDLE START) ;
G43 H05 Z.1 (TOOL LENGTH COMPENSATION) ;
G77 Z-1. R-1.6 Q0.1 F10. (1ST HOLE) ;
X-2. (2ND HOLE) ;
G80 G00 Z.1 M09 (CANCEL CANNED CYCLE) ;
G28 G91 Z0. M05 ;
G77 Approximate Toolpath Example. This example shows the entrance motion only.
Dimensions are not to scale.
note: For this example, the “top” of the workpiece is the surface defined as
Z0. in the current work offset. The “bottom” of the workpiece is
the opposite surface.
In this example, when the tool reaches the R depth, it then moves 0.1"
in X (the Q value and Setting 27 define this movement; in this example,
Setting 27 is X+). The tool then feeds to the Z
value at the given feedrate. When the cut is finished, the tool shifts back toward the
center of the hole and retracts out of it. The cycle repeats at the next commanded
position until the G80 command.
note: The R value is negative, and it must go past the bottom
of the part for clearance.
note: The Z value is commanded from the active Z work
note: You do not need to command an initial point return (G98)
after a G77 cycle; the control assumes this automatically.