-Shenzhen Guanhong Automation Co.,Ltd.-
SZGH-CNC1000MDb Series
- 76 -
3.28.5 Drilling cycle, Spot Drilling (G81)
This cycle is used for normal drilling, Cutting feed is performed to bottom of the hole. Then
the tool retracted from the bottom of the hole in rapid traverse.
Format:
G81 X_ Y_ Z_ R_ F_ L_ ;
X_Y_ : Hole position data
Z_ :
The distance from point R to bottom of the hole
R_ :
The distance from initial level to point R level
F_ :
Cutting feedrate
L_ :
Number of repeats (if required)
G81 (G98)
G81 (G99)
After positioning along the X axis and Y axis, rapid traverse is performed to point R. Drilling
is performed from point R to point Z. Then the tool is retracted in rapid traverse.
Before specifying G81, use miscellaneous function (M code) to rotate the spindle. When the
G81 command and an M code are specified in the same block, the M code is executed at the time of
the first positioning operation. The system then proceeds to the next drilling operation.
When a tool length offset (G43, G44 or G49) is specified in the canned cycle, the offset is
applied at the time of position to point R.
Note: In the canned cycle mode, tool offsets are ignored.
Example
:
M3 S2000 ;
Cause the spindle to start rotating
G90 G99 G81 X300 Y-250 Z-150 R-100 F120 ;
Position, drill hole 1, then return to point R.
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.
G98 Y-750 ;
Position, drill hole 5, then return to the initial level.
G80 G28 G91 X0 Y0 Z0 ; Return to the reference position
M5 ;
Cause the spindle to stop rotating
