Fagor 8025 T CNC, Operating Manual

Page: 234 / 309

120 8025/8030 CNC PROGRAMMING MANUAL
10. (T) TOOL PROGRAMMING
The tool to be used is programmed by means of code T2.2
- Tool number. The two digits to the left of the decimal point may have any value
between 00 and 99. This value is used for selecting the required tool in the case of a
machine with automatic turret, and may be limited to a value lower than 99 according
to the machine parameter. This value is used to select the required tool.
- Tool compensation (tool offset table). The two digits to the right of the decimal point
may have any value between 01 and 32. With these figures the desired values are
selected in the tool offset table.
As soon as T2.2 is read, the CNC applies the X,Z,I,K values stored in the table except when
P604(5) is 1, in which case these values will be applied after an M06.
When G41 or G42 is programmed, the CNC applies the value stored at the programmed
T address (01-32) as radius compensation value.
If no T has been programmed, the CNC applies the address T00.00, which corresponds to
a tool of zero dimensions.
The following values are recorded in every tool offset table address (01-32).
X : Tool length along X axis.
Z : Tool length along Z axis.
F : Location code.
R : Tool nose radius.
I : Tool wear offset along X axis. This value must always be entered in diameters.
K : Tool wear offset along Z axis.
The max. values are:
X,Z (tool length) +/-8388.607 mm (+/-330.2599 inches).
I,K (tool length offset) +/-32.766 mm (+/-1.2900 inches).
R (Radius) 1000.000 mm (39.3700 inches).
To offset the tool nose radius the location code (F) of the tool must also be stored. Possible
codes are: F0-F9 (see figure).