Fagor 8055 EN, Руководство по программированию

Страница: 172 / 482

·172·
Programming manual
CNC 8055
CNC 8055i
9.
CANN
ED
CYCLES
·M· & ·EN· M
ODELS
S
OFT
: V02.2
X
G84. Ta
ppin
g
ca
nne
d cycl
e
9.10 G84. Tapping canned cycle
This cycle taps at the point indicated until the final programmed coordinate is reached. General logic
output "TAPPING" (M5517) stays active while executing this cycle.
Due to the fact that the tapping tool turns in two directions (one when tapping and the other when
withdrawing from the thread), by means of the machine parameter of the spindle "SREVM05" it is
possible to select whether the change in turning direction is made with the intermediate spindle stop,
or directly.
General machine parameter "STOPAP(P116)" indicates whether general inputs /STOP, /FEEDHOL
and /XFERINH are enabled or not while executing function G84.
It is possible to program a dwell before each reversal of the spindle turning direction, i.e., at the
bottom of the thread hole and when returning to the reference plane.
Using parameters B and H, the threading may be done with relief for chip breakage.
The tapping with relief is done in successive approaches until the programmed total depth is
reached. After every approach, it withdraws for chip relief. In this case, the dwell (K) is only applied
on the last pass, not on the relief passes.
Working in Cartesian coordinates, the basic structure of the block is as follows:
G84 G98/G99 X Y Z I K R J B H
[ G98/G99 ] Withdrawal plane
G98 The tool withdraws to the Initial Plane, once the hole has tapped.
G99 The tool withdraws to the Reference Plane, once the hole has tapped.
[ X/Y±5.5 ] Machining coordinates
These are optional and define the movement of the axes of the main plane to position the tool at
the machining point.
This point can be programmed in Cartesian coordinates or in polar coordinates, and the coordinates
may be absolute or incremental, according to whether the machine is operating in G90 or G91.
[ Z±5.5 ] Reference plane
Defines the reference plane coordinate. It can be programmed in absolute coordinates or
incremental coordinates, in which case it will be referred to the initial plane.
If not programmed, it assumes as reference plane the current position of the tool.
[ I±5.5 ] Thread depth.
Defines tapping depth. It can be programmed in absolute coordinates or incremental coordinates
and in this case will be referred to the reference plane.
[ K5 ] Dwell
Defines the dwell, in hundredths of a second, after the tapping until the withdrawal begins. If not
programmed, the CNC will take the value of "K0".