Fagor 8025 GP, Operating Manual

Page: 275 / 423

8025/8030 CNC PROGRAMMING MANUAL 155
I+/-4.3 : It defines the depth of the machining. With G90, the values are absolute, in other
words, they are related to the origin of the axis perpendicular to the main plane. With
G91 the values are incremental, that means, they are related to the reference plane
(approach).
K2.2. : It defines the dwell from reaming the full machining depth until starting its withdrawal.
A value may be programmed either within K0.00 (0.00 sec.) and K99.99 (99.99) or
within 0.00 and 655.35, if it is programmed with a parameter (K P3).
The programming of this parameter is obligatory only in drilling cycle with dwell
G82, if it is not programmed, the CNC will display error 44. In the other, canned
cycles, if K parameter is not programmed, the CNC assumes the value of K0.
N2 : It defines the number of times that the block’s execution is to be repeated.
Any value between N0 and N99 can be programmed, but, if the value is programmed
with a parameter (N P3), the latter can have a value between 0 and 255. If parameter
N is not programmed, the CNC assumes the value N1. Obviously, the programming
of values of N higher than 1 makes sense when operating on G91, in other words, if
the axis movement values are incremental, since otherwise the machinings will be
repeated at the same point. When programming the same canned cycle a number of
times, only F, S and M functions will be executed in the cycle calling block.
A more detailed explanation of the (G81,G82,G84,G85,G86 and G89) canned cycle is
subsequently given, supposing that the main plane is the one formed by X and Y axes and that
Z is the axis of the tool.