Disclaimer: CNC Concepts, Inc. accepts no responsibility for the use
or misuse of techniques shown in this web page. We simply publish information
we feel will be of interest to CNC users. In all cases, the reader is totally
responsible for considering the implications, good and bad, of implementing one
or more of the techniques we show.
How does G61 work?
Can you explain the use of G61 for machining centers and turning centers?
Thank you, Art.
For Fanuc and Fanuc-compatible controls, G61 is the modal exact stop
check command. Note that G61 is cancelled by G64, which places the machine
back in the normal cutting mode. There is also a non-modal exact stop check
The exact stop check function is used whenever you want the machine to come
to a complete stop between motion commands. Exact stop check is most commonly
used when a programmer wants the tool to machine "sharp outside
corners" when milling a workpiece. In the normal cutting mode, the
cutting tool will flow through its series of motions smoothly (without
stopping). This is usually very desirable since witness marks will be left on
the workpiece in many cases if the tool comes to a stop between motions.
However, you must understand that milling cutters will have a natural
tendency to round corners in the normal cutting mode. The larger the machine
and the faster the feedrate, the more corner rounding that will occur. Using
exact stop check will force the machine to stop between motion commands, which
in turn, forces sharp corners to be machined.
For most applications, remember that a slightly rounded corner is desirable.
Most machinists are told to always break sharp corners to avoid the possibility
of cutting someone on a sharp edge. So many CNC users will never be concerned
with the small amount of corner rounding a CNC machining center will naturally
produce. However, there are times when sharp corners are required.
In the next drawing, notice that the tool is machining the right side and
upper side of a rectangular shape. The upper right hand corner of this
workpiece is supposed to be "sharp" - that is - having no corner
radius or chamfer. And if the milling cutter moves as shown in the drawing, of
course, the corner will be sharp.
When machining a hard material, like steel, it's
likely that the programmed feedrate will be so slow that the tool will
truly machine this corner in such a way that there is no radius in the corner
(assuming the program is correct). However, when machining softer materials,
like aluminum - the programmed feedrate will be much faster. The faster the
feedrate (and the larger the machine) the more likely it will be that the
cutting tool will "round" the corner, as is shown in the next
Again, this undesired corner rounding will only
occur when feedrate is very fast and/or with larger machines. Also note that
certain machine parameters can be adjusted to "tighten up" the axes
movements - so no corner rounding will occur even at faster feedrates. And,
machine tools can be designed to minimize this tendency for rounding (many
current model high speed machining machines" can make precise movements at
very fast feedrates in excess of 100 inches per minute).
For general purpose machining centers, and when this problem presents
itself, one way to ensure that the corner will be sharp is to use the exact
stop check function. In essence, using G09 or G61 is much like using a
dwell command (G04) between the two motion commands. But the time for the pause
with G09 or G61 is set by a parameter, meaning it does not have to be specified
in the program. Consider these commands.
N035 G00 X-0.6 Y-0.6
N040 G43 H01 Z-0.85
N045 G01 X4.0 F5.0
N050 G09 Y4.0
N065 G00 Z0.1
We're milling an outside rectangular shape. Look at line N050. This is the
command that machines the right side (X plus side) of the rectangle. The G09
will cause the machine to pause after making the motion to Y4.0. Since
the tool is forced to move all the way to Y4.0 and stop, this will cause a
sharp corner (no corner rounding) to be machined in the upper right corner of
the rectangle. However, the lower right and upper left corners will experience
the effects of corner rounding (again, G09 is a non-modal G code).
Now consider these commands.
N035G00 X-0.6 Y-0.6
N040 G43 H01 Z-0.85
N045 G01 G61 X4.0 F5.0
N060 G64 Y-0.6
N065 G00 Z0.1
The G61 in line N045 places the machine in the exact stop check mode. The
cutting tool will continue to come to a stop after each motion until the G64 in
line N060 is executed. This will force sharp corners in every case.