Specifications

_____________________________________________________________________
_____________________________________________________________________
CONCISE GUIDE FANUC 54
The tool, in rapid traverse, reaches the X and Z values indicated in the block before the first G72 (these
values thus determine the point where the tool will start machining: X will be equal to the rough workpiece
diameter plus a small safety margin that facilitates the cut increment, Z will be 0 if the workpiece is
already faced, or 1 or 2 if there is a machining allowance).
The increment will be equal to the value indicated in parameter W of the first G72 block (the increment
may be in rapid mode or working mode – this depends on whether the profile description in the block after
the second G72, starts with G0 or G1).
The tool makes the rough machining automatically performing a series of cuts going from one point
indicated in block P up to the point indicated in block Q.
At the end of each cut the tool separates by 45°, in rapid mode, for a radial value equal to that set in
parameter R and returns in rapid traverse to the Z starting point.
When all the rough machining cuts have been performed the tool makes 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 (which 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 back spindle toward the spindle,
and negative for spindle machining toward the back spindle or for machining on the back spindle (on
machines that have this option)
If the pre-finishing cut is not required it is sufficient to program the block after the second G72, block from
which the finished profile starts, containing in it both X and Z.
When performing the cycle, the tool works with the feed programmed in parameter F of cycle G72, any
feeds set in profile description blocks are only activated during the finishing operations.
NOTE. The rough machining cycle G72 does not include the use of the tool radius offsets (G41, G42,
G40) which can. of course, be activated for finishing (cycle G70).
The finished profile of the part cannot be managed in a sub-program, but only within the cycle itself.