Rockwell Automation 8520 9/Series CNC Lathe - Manual (Page 599)

Compound Turning Routines
Chapter 24
24-35
The G72 finish routine is normally executed after the completion of a
contouring routine (G73, G74 or G75). With the G73, G74, and G75
routines a finish allowance is left on the workpiece if a U- and/or K-word
is specified in the routine. The G72 routine is used to remove this finish
allowance and cut the workpiece to within the specified tolerance of the
actual workpiece finished shape.
The calling block references sequence numbers of the first and last blocks
of the contour blocks defining the final contour of the workpiece. This set
of blocks may be located anywhere after the calling block (even after an
end of program command), as long as the calling block is in the same
program as the set of contour defining blocks. This means that contour
blocks can not be called from a subprogram or a macro unless the calling
block is in that subprogram or macro. This routine actually executes the
set of contour defining blocks as entered in the program.
The G72 finishing routine is usually performed at a lower feedrate to
produce the desired finish results that are not necessary using the other
rough contouring routines for rapid removal of material.
The program format for this finishing routine is indicated below:
G72 P__ Q__;
Where : Is :
P__ The sequence number of the first block in the set of contour blocks that defines
the finished workpiece shape.
Q__ The sequence number of the last block in the set of contour blocks that defines
the finished workpiece shape.
In the G72 finishing routine, the contour of the finished workpiece can be
described by a set of linear and/or circular blocks bounded by the sequence
numbers specified with parameters P and Q. It is assumed that some other
blocks have positioned the cutting tool to some position above the part.
This position should be the start point of the workpiece contour blocks.
The workpiece contour blocks may be at any location within the same
program containing the G72 block (even after an end of program M02 or
M30). They may not be resident in a subprogram or macro that is called
by the program containing the G72 block.
The control recognizes F-, S-, or T-words programmed in this set of
contour blocks and uses these values for the routines execution. These
values are not ignored as in the G73, G74, and G75 routines (F-words are
used in the G73, G74, and G75 routines).
24.4
O.D. and I.D. Finishing
Routine (G72)