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 command (G09).

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 drawing.

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

  • N055 X0

  • N060 Y-0.6

  • 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

  • N050 Y4.0

  • N055 X0

  • 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.


Recent Posts

See All

How does G66 work?

G66 is one of the more misunderstood custom macro B commands. Fanuc calls it a modal custom macro call. It looks just like a G65 command. Consider these two commands: N045 G65 P1000 X3.0 Y3.0 Z0 A45.0

What are directional vectors?

Current model CNC controls make it easy to create circular commands. You simply specify the direction (G02: clockwise or G03: counter clockwise), the end point (usually X and Y), and the radius (with

cnc reverse logo.jpg

44 Little Cahill Road

Cary, IL  60013

Ph: 847-639-8847

  • Facebook Social Icon