CNC Milling | G76 Cycle | Fine Boring


G76 Cycle Introduction

The fine boring cycle bores a hole precisely. When the bottom of the hole has been reached, the spindle stops, and the tool is moved away from the machined surface of the workpiece and retracted.

G76 Cycle Format

G76 X_ Y_ Z_ R_ Q_ P_ F_ K_ ;

Parameters

X_ : Hole position data
Y_ : Hole position data
Z_ : The distance from point R to the bottom of the hole
R_ : The distance from the initial level to point R level
Q_ : Shift amount at the bottom of a hole
P_ : Dwell time at the bottom of a hole
F_ : Cutting feedrate
K_ : Number of repeats (if required)

Things to Know

  • Be sure to specify a positive value in Q. If Q is specified with a negative value, the sign is ignored. Set the direction of shift in the parameter No.5148 for Fanuc CNC Controller.
  • Specify P and Q in a block that performs drilling. If they are specified in a block that does not perform drilling, they are not stored as modal data.
  • Always cancel cycle with G80 code when finished.


When the bottom of the hole has been reached, the spindle is stopped at the fixed rotation position, and the tool is moved in the direction opposite to the tool nose and retracted. This ensures that the machined surface is not damaged and enables precise and efficient boring to be performed.

G76 Cycle Examples

G76 CNC Program Example – 1

M3 S500 ; Cause the spindle to start rotating.
G90 G99 G76 X300. Y-250. Z-150. R-120. Q5. P1000 F120. ; Position, bore hole 1, then return to point R. Orient at the bottom of the hole, then shift by 5 mm. Stop at the bottom of the hole for 1 s.
Y-550. ; Position, drill hole 2, then return to point R.
Y-750. ; Position, drill hole 3, then return to point R.
X1000. ; Position, drill hole 4, then return to point R.
Y-550. ; Position, drill hole 5, then return to point R.
G98 Y-750. ; Position, drill hole 6, then return to the initial level.
G80 G28 G91 X0 Y0 Z0 ; Return to the reference position
M5 ; Cause the spindle to stop rotating.