Fagor 8025 GP, Operating Manual

Page: 206 / 423

86 8025/8030 CNC PROGRAMMING MANUAL
6.28. G74. MACHINE REFERENCE SEARCH
When G74 is programmed in a block, the CNC moves the axes to the machine-reference
point.
a) REFERENCE SEARCH FOR ALL AXES
* If machine parameter P725 = 0 and G74 is programmed alone in the block. The CNC
moves first the axis which is perpendicular to the plane programmed.
This is Z if operating on G17, Y on G18 ,X on G19. The movements of the remaining
axes then follow.
In four-axis machines, if the active axis when programming G74, is the one
associated to the fourth (W), the axes will be moved as described, (W) being the last.
However, if the active axis is the fourth (W) when G74 is programmed, it will
replace its associated axis in the prescribed order and the associated axis will be the
last on moving.
In 5 axis machines the movement of the 5th axis V, when G74 only G74 is
programmed, this is always done after the movement of the 4th axis W.
* If P725 has a value between 1 and 99 and G74 is programmed alone in the block, the
CNC will automatically execute the subroutine whose number is in P725.
If P725 = 74, subroutine 74 will be executed. For example:
N0 G22 N74
N10 G74 X Y W V (this might be the order required by the user)
N20 G74
b) REFERENCE SEARCH FOR ONE AXIS OR MORE THAN ONE IN A SPECI-
FIC ORDER
If machine-reference search is required in an order other than the above, G74 is
programmed, followed by the axes in the required order.
No other function can be programmed in a block in which G74 is programmed.
In both cases, a) and b), when the axes reach the machine-reference, the distances
between this point and the last part’s datum point programmed are displayed.