Fagor 8025 GP, Operating Manual

Page: 319 / 423

8025/8030 CNC PROGRAMMING MANUAL 199
Example:
Machining of a circular pocket of radius 70 mm and depth 40 mm.
Let us suppose that:
. The distance between the reference plane and the part’s surface is 2 mm.
. The tool starting point is X0 Y0 Z0 and the spindle is not running.
. The tool has 7.5 mm radius and it is number 1 (T.1).
N0 G88 G98 G00 G90 X90 Y80 Z-48 I-90 J70 B12 C10 D2 H100 L5 F300 S1000 T.1
M3
N5 G80 X0 Y0
N10 M30
Block N0
G88 : Identifies the circular pocket cycle.
G98 : Identifies the withdrawal of the tool (Z axis) to the starting plane after completing
the pocket machining.
G00 : Identifies the X and Y axes movement as being in rapid move.
G90 : Identifies the X,Y,Z and I dimensions as being absolute coordinate values.
X,Y : Movement of the mentioned axes to the center of the pocket.
Z : Movement of the tool (Z axis), from the starting plane to the reference one (always
in rapid move).
I : Movement to the pocket bottom (Absolute coordinate value referred to Z0).
J : Identifies the pocket radius. The milling direction will depend on the sign (positive
or negative) programmed.
B : Depth of each milling pass ( always positive).