Specifications

_____________________________________________________________________
_____________________________________________________________________
CONCISE GUIDE FANUC 48
• U => Diametric machining allowance on axis X value indicated with sign
• W => Machining allowance on axis Z value indicated with sign
• F => Work feed in rough machining
In rapid traverse the tool reaches the X and Z values indicated in the block before the first G71 (these
values therefore determine the point where the tool will start to machine: X will be equal to the diameter of
the blank workpiece, Z will be the safety distance that facilitates the cut increment).
An increment takes place that is equal to the radial value indicated in parameter U of the first G71 block
(the increment can take place in rapid mode or work mode, depending on whether the profile description,
block after the second G71, starts with a G0 or a G1).
The tool performs the rough machining automatically making several cuts, going from the point indicated
in block P to the point indicated in block Q.
At the end of each cut the tool separates in rapid mode, by 45° by a radial value equal to that indicated in
parameter R and returns in rapid mode to the Z starting point.
After all the rough machining cuts have been made, the tool performs a pre-finishing cut to leave even
machining allowances (parameters U and W indicated with sign), and returns in rapid traverse to the
starting point. Value U (that determines the diametrical machining allowance along axis X) will be positive
for external machining and negative for internal machining. Parameter W (that determines the machining
allowance along axis Z) will be positive for machining from the tailstock toward the spindle and negative
for machining from the spindle toward the tailstock or for machining on the back spindle (on machines with
this option installed)
If the pre-finishing cut is not required, just program the block after the second G71, (block that starts the
finished profile) to contain both X and Z.
When running the cycle the tool works with the feed programmed in parameter F of the G71 cycle, any
feeds programmed in the profile description blocks are only activated during the finishing operation (see
G70 cycle further on).
NOTE. The G71 rough machining cycle does not use the tool radius offset (G41, G42, G40) which can, of
course, be activated in finishing (G70 cycle).
The finished profile of the workpiece cannot be managed in a sub-program, but only within the cycle itself.