Fagor 8025 GP, Operating Manual

Page: 310 / 423

190 8025/8030 CNC PROGRAMMING MANUAL
6.32.8. G87. Rectangular pocket milling canned cycle
The operations and movements of the tool are as follows:
- If the spindle was previously running, it continues to rotate in the same direction. If it
was not running it starts clockwise (M03).
- Rapid movement of the Z axis from the starting plane to the reference (approach) plane.
- Movement a 50% of the working feedrate (F) of the Z axis for a distance equal to (D+B).
D: Distance between the reference plane and the surface of the part.
B: Depth value of each machining pass.
- Milling at working feedrate (F) of the pocket surface by steps defined by C, to a distance
L (finishing pass), of the pocket wall.
- Milling at the working feedrate H, of the finishing pass.
- After completing the finishing pass, the tool withdraws in rapid move to the pocket
center, positioning the Z axis 1 mm higher. In this way, the first penetration is finished.
- Movement at 50% of the working feedrate (F) of the Z axis for a distance equal to B+1.
- Milling at working feedrate (F) of the pocket surface (second penetration).
- The above steps are repeated until the full depth of the pocket is reached.
- Once the pocket is completed, the tool withdraws in rapid (Z axis) to the reference plane
(if G99 has been programmed) or to the starting plane (if G98 has been programmed).
Atention:
To enable a good finish to be achieved in the machining of pockets the
CNC performs a tangential approach and tangential exit in the last pass
of each of thepenetrations. For this purpose, the tool has to withdraw to
the center of the pocket before beginning the milling of the wall. To avoid
problems and possible machining malfunctions, it is mandatory to
program the tool code (T2.2) and to enter in the tool table the value of the
radius of the tool that is to be used. If the radius value entered in the tool
table is RO, the final wall pass is performed like all the others; i.e. with
neither tangential entry nor tangential exit. The value or R must never
be negative. If T2.2 is not programmed, the CNC takes as tool radius the
value of R of the last corrector.