G88 Cycle Introduction
This cycle is used to bore a hole. After positioning along the X- and Y-axes, rapid traverse is performed to point R. Boring is performed from point R to point Z.
When boring is completed, a dwell is performed at the bottom of the hole, then the spindle is stopped and enters the hold state. At this time, you can switch to the manual mode and move the tool manually. Any manual operations are available; it is desirable to finally retract the tool from the hole for safety, though. At the restart of machining in the DNC operation or memory mode, the tool returns to the initial level or point R level according to G98 or G99 and the spindle rotates clockwise. Then, operation is restarted according to the programmed commands in the next block.
G88 Cycle Format
|G88 X_ Y_ Z_ R_ 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|
|P_ : Dwell time at the bottom of a hole|
|F_ : Cutting feed rate|
|K_ : Number of repeats (if required)|
G88 Cycle Examples
G88 CNC Program Example – 1
M3 S2000 ; Cause the spindle to start rotating.
G90 G99 G88 X300. Y-250. Z-150. R-100. P1000 F120. ; Position, drill hole 1, return to point R then 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.