Fagor 8025 GP, Operating Manual

Page: 352 / 423

232 8025/8030 CNC PROGRAMMING MANUAL
11.8. M06. TOOL CHANGE CODE
a) MACHINE WITHOUT AUTOMATIC TOOL CHANGER
- If P601(1) and P601(5) are set to zero(MACHINE WITHOUT AUTOMATIC TOOL
CHANGE), the CNC sends out codes M05 and M06 when code M06 is read.
According to the value assigned to P601(8), it will stop or not the program (like M00).
P601(8)= 1 It stops the program
P601(8)= 0 It does not stop the program
b) MACHINE WITH AUTOMATIC TOOL CHANGER
- If P601(1) or P601(5) are set to 1, the code M06 has to be programmed alone in a block.
When reading this code the CNC, in modes: AUTOMATIC, SINGLE BLOCK,
TEACH- IN, will execute the following sequence:
- It will send out the code M19 and will apply a residual S analog output (defined by
P601(7) and P700) to the spindle.
- It will move the axes X,Y,Z,(W) to the positions fixed by P900, P901, P902 and P903,
according to the order defined by P702, P703, P704 and P705.
- It will send out the code M06, cancelling the residual S analog output afterwards.
- If parameter P709 has a value between 1 and 99, the CNC will automatically jump to
a subroutine identified by P709. If P709 is zero, there is no jump.
In SINGLE BLOCK mode, the CYCLE START key must be pressed as many times
as different functions are involved with M06. In JOG mode, the CNC will send the
code M19, will apply to the spindle the residual analog output and will send M06,
previously cancelling the residual analog output if the axes have been correctly
positioned for the tool change. If any axis is out of position, the CNC will give error
code 51.
- Same as in the previous section, it will stop the program or not, according to status of
parameter P601(8).
Atention:
It is recommended that M06 be set so that the CNC executes it at the end
of the block in which it is programmed.