Fagor 8025 GP, Operating Manual

Page: 294 / 423

174 8025/8030 CNC PROGRAMMING MANUAL
6.32.6. Deep hole drilling canned cycle definition. G83
This canned cycle may be programmed in two different ways:
Format a) N4 G83 G98/G99 (v+/-4.3)(W+/-4.3) X+/-4.3 Y+/- 4.3 Z+/-4.3 I+/-4.3
J2 N2
Format b) N4 G83 G98/G99 (W+/-4.3) X+/-4.3 Y+/-4.3 Z+/- 4.3 I+/-4.3 B+/-4.3
C+/-4.3 D+/-4.3 H4.3 J2 K2.2 L4.3 R(0.000/500) N2
The meaning of the values of the format a) is as follows:
N4 :Block number (0/9999).
G83 :Code of the deep drilling canned cycle.
G98 :Withdrawal of the axis perpendicular to the main plane, to the starting
plane,after completing the machining.
G99 :Withdrawal of the axis perpendicular to the main plane, to the reference
plane, after completing the machining.
X+/-4.3 :These values have different meaning, depending on the main plane in
which the cycle is being carried out.
Y+/-4.3 :
Z+/-4.3 :
*(W+/-4.3):
*(V+/-4.3) :
X+/-4.3
Y+/-4.3
X/Z
G18 X+/-4.3
Z+/-4.3
Y/Z
G19
Y+/-4.3
Z+/-4.3
X/Y
G17
X/Z
G18
Y/Z
G19
Z+/-4.3
Y+/-4.3
X+/-4.3
X/Y
G17
MAIN PLANE VALUE MEANING
They define the movement of the axes of the main plane necessary
to position the tool in the center of the first machining. The values
will be either absolute or incremental depending on the function on
which we are operating (G90 or G91).
The movements will be carried out either in rapid or in F operation
feedrate, depending on the function on which we are operating (G00
or G01).
That point can be also programmed in polar coordina
tes.
It identifies the movement of the axis perpendicular to the main
plane, from the starting plane up to the reference plane (approach).
This movement will be executed in rapid (G00). The values will be
either absolute or incremental, depending on the function on which
we are operating (G90 or G91).
This value must necessarily be programmed.
* If the 4th W axis or the 5th V axis are perpendicular to the main plane, it must be a
linear axis. But if it is one of the axis of the main plane, it may also be a rotary axis.