Fagor 8025 T CNC, Operating Manual

Page: 239 / 309

8025/8030 CNC PROGRAMMING MANUAL 125
11.8. M19. SPINDLE ORIENTATION
If M19 S4.3 is programmed, the spindle will rotate at the speed and direction set by
machine-parameters P606(2) and P706 and will stop at the point identified by S4.3 in
degrees, referred to the reference zero marker.
When the spindle is positioned within the dead band (P707), the CNC sends out the spindle
blocking signal (decoded M15) and the spindle is kept in closed loop; gain as per P708,
min. analog voltage as per P709.
When programming in a block M19 S4.3, more information is not allowed in that block.
Machine parameters P906 and P907 determine the lower and upper limits, respectively,
of the spindle travel, with M19.
11.9. M41,M42,M43,M44 SPINDLE RANGE SELECTION
When P601(1) has been set to 1, these codes are automatically generated by the CNC,
when an S function is programmed. If this parameter is 0, M41,M42,M43 and M44 must
be programmed.
When operating at constant surface speed (G96) these functions must necessarily be
programmed even if P601(1) is set to 1.
11.10. M45. SELECTION OF ROTATION SPEED OF THE LIVE TOOL AND
THAT OF THE SYNCHRONIZED TOOL.
There are two formats to program an M45 function:
a) Live tool
Programming format: N4 M45 S+/-4
S+/-4 defines the direction and rotation speed of the live tool.
The +/- sign defines the direction of turn, with S+4, it will turn in one direction and with
S-4 will turn in the opposite direction.
The programmable value range is between S0 and S9999 (0-9999 r.p.m.).