·286·
Programming manual
CNC 8055
CNC 8055i
12.
PROBING
·M· & ·EN· MODELS
SOFT: V02.2X
Probing (G75, G76)
12.1 Probing (G75, G76)
The G75 function allows movements to be programmed that will end after the CNC receives the
signal from the measuring probe used.
The G76 function allows movements to be programmed that will end after the CNC no longer
receives the signal from the measuring probe used.
Their definition format is:
G75 X..C ±5.5
G76 X..C ±5.5
After G75 or G76, the required axis or axes will be programmed, as well as the coordinates of these
axes that will define the end point of the programmed movement.
The machine will move according to the programmed path until it receives the signal from the probe
(G75) or until it no longer receives the probe signal (G76). At this time, the CNC will consider the
block finished, taking as the theoretical position of the axes the real position they have at that time.
If the axes reach the programmed position before receiving or while receiving the external signal
from the probe, the CNC will stop the movement of the axes.
This type of movement with probing blocks are very useful when it is required to generate
measurement or verification programs for tools and parts.
Functions G75 and G76 are not modal and, therefore, must be programmed whenever it is wished
to probe.
Functions G75 and G76 are incompatible with each other and with G00, G02, G03, G33, G34, G41
and G42 functions. In addition, once this has been performed, the CNC will assume functions G01
and G40.
During G75 or G76 moves, the operation of the feedrate override switch depends on the setting of
OEM machine parameter FOVRG75.
To Next Page
Loading...
