Fagor 8025 T CNC, Operating Manual

Page: 163 / 309

8025/8030 CNC PROGRAMMING MANUAL 49
If parameter P600(1) = 0 and axes
or parameter P600(1) = 1 and axes
G41 operates as G42 and vice versa.
The CNC has a table of up to 32 tool offsets comprising for each tool length (X,Z,I,K) and
radius (R) values plus location codes (F). The compensation values must be stored in the
tool offsets mode (8). The values of I,K can also be checked and modified, without
stopping the execution of a program (see Operation Manual). The tool table can also be
loaded by using G50 in the program.
The max. values are:
X,Z (tool length) +/- 8388.607 mm (+/-330.2599 inches)
I,K (tool length offsets) +/-32.766 mm (+/-1.2900 inches)
R (Radius) 1000.000 mm (39.3700 inches)
The location code of the tool (F) is also necessary to perform radius compensation.
Possible codes are F0-F9 (see figure).
The compensation is made effective by means of G41 or G42 and acquires the table value
selected by code Txx.xx (Txx.01-Txx.32). If Txx.xx has not been programmed, the CNC
assumes the value T00.00 which corresponds to a tool whose dimensions are zero.
Functions G41 and G42 are modal (persistent) and are cancelled by G40,M02,M30 as well
as by an EMERGENCY or by a general RESET.
The CNC applies tool length compensation (X,Z,I,K) as soon as a tool (Txx.01) is
programmed, unless P604(5) is 1. In this case the compensation is effective after M06.
Atention:
The values of I, used to offset tool wear, must be entered in diameters.