Fagor 8025 GP, Operating Manual

Page: 277 / 423

8025/8030 CNC PROGRAMMING MANUAL 157
Example G81
Drilling four holes 20 mm deep (polar coordinates).
Let us suppose that:
. The distance between the reference plane and the surface of the part is 2 mm.
. The starting point is X0,Y0,Z0 and the spindle is not running.
N0 G81 G98 G00 G91 X250 Y350 Z-98 I-22 F100 S500 N1
N5 G93 I250 J250
N10 A-45 N3
N15 G80 G90 X0 Y0
N20 M30
First block (N0)
G81 : Defines the drilling canned cycle.
G98 : Defines the tool withdrawal (Z axis) to the starting plane.
G00 : Defines the movement of the X and Y axes as being rapid.
G91 : Defines the dimensions as being incremental.
X( ) : Movement in millimeters on these axes.
Y( )
Z( ) : Tool movement in millimeters (Z axis) from the starting plane to the reference
plane.
I( ) : Movement in millimeters from the reference plane to the full machining depth.
F( ) : Working feedrate in mm/min.
S( ) : Spindle rotation speed in rev/min.
N( ) : Number of times the block is repeated.