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_ ;|
|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.
|You may be interested also:|
|“CNC Milling | G86 Cycle | Boring”|
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.