Last month, I introduced some unique CNC features that can surprise you — in either a positive or negative way. I’d like to expand the discussion to include oddities in the ways a CNC naturally behaves in hopes of helping you understand some rather unusual situations. As with issues previously mentioned, I discovered most of these conditions while helping CNC users over the years.

When linear motion (G01) is faster than rapid motion (G00)

A good rule of thumb for choosing to use rapid motion is, if the machine is not cutting, it should be moving at rapid motion. This minimizes program execution time by moving axes from place to place as quickly as possible.

There is one situation, however, when moving axes in linear interpolation mode (G01) using a fast feed rate might render faster overall positioning time. CNCs deal with rapid mode acceleration and deceleration differently than linear interpolation mode acceleration and deceleration.

Machines typically take longer to ramp up to speed and slow to a stop when in rapid mode. When making short motions, say 0.5 inch (about 13 millimeters) or under, most machines fall well short of reaching their rapid rate.

Perform this simple test to judge whether you should start using G01 for short positioning movements. First, create and run this program. It assumes the machine has at least 30.0 inches of X-axis travel.

• O0001 (Test for rapid motion)
• G91 G00 Z-0.5
• Z0.5
• X0.5
• Z-0.5
• Z0.5
• X0.5
• (Repeat the bolded three commands 48 times).
• M30

Move the X-axis close to its negative limit and run (and time) this program. 

Now modify the first command as follows to create this new program:

• O0001 (Test for linear interpolation motion)
• G91 G01 Z-0.5 F50.0 (change G00 to G01 and add F50.0 word)
• Z0.5
• X0.5
• Z-0.5
• Z0.5
• X0.5
• (Repeat the bolded three commands 48 times).
• M30

Run and time this new version of the program. Which program executed faster? You may be surprised by the results.

Milling internal fillets versus external radii

Circular motion, commanded by G02 and G03, is used on a very regular basis. Even so, feed rate for circular motion is widely misunderstood. You must understand that the feed rate specified in a circular motion command is the motion rate for the cutting tool’s centerline tool path.

You may never notice an issue with lathe work. With single-point cutting tools used on turning centers, the tool nose radius is usually very small (usually under 0.100 inch). For this reason, the centerline tool path is always very close to the work surface being machined. Note, however, that the machining rate when machining internal filets will be slightly faster than the machining rate when machining external radii.

This issue is much more obvious when milling. Milling cutters used on machining centers can be quite large. Now the distance between the milling cutter’s centerline path and the work surface being machined is more substantial. If you use the same feed rate for circular motions as you do for linear motions, you may notice surface finish differences between straight and circular surfaces.

The larger the milling cutter, the more noticeable the difference in surface finishes will be. It is not unusual, for instance, for a large milling cutter to chatter (vibrate) when machining an internal (fillet) radius since its periphery is moving much faster than it should.

Where’s my thread?

There is a feature called thread chamfering that directly affects how threads are machined when using the G76 multiple repetitive cycles with FANUC CNCs. With older controls, the thread chamfering amount is specified by a parameter setting. With newer controls, it can be specified in the (two-line) G76 command using the six-digit P word. The second two digits of the P word specify the thread chamfer amount in 0.1-pitch increments. A value of P001000, for instance, specifies a 1.0-pitch chamfer amount.

When a thread chamfering amount is specified (by the parameter setting or with the P word), the threading tool will chase the thread to within the thread chamfer amount of the thread’s end point and then start pulling out (chamfering) out at a 45-degree angle. This is not required when threading is done into a recess.

If the thread chamfer amount is set excessively, say to a value of three pitch amounts (P003000 or in the parameter), and with a coarse, short thread, the threading tool will begin its chamfering movement before it even starts chasing the thread. There will be no thread when the threading tool is finished.

This can be a difficult issue to diagnose, especially if you have not specified a chamfering amount in the P word of the G76 command. You may not know about the (excessively set) parameter that specifies the thread chamfering value. You may simply think the G76 command does not work on your machine.

Why did the tool drill two holes in the same location?

Once a hole machining canned cycle is commanded (like G81), the CNC will machine a hole in every command until the cycle is canceled with a G80. Consider these commands:

• .
• .
• N040 G81 X1.0 Y1.0 R0.1 Z-0.75 F3.0 (Drill first hole)
• N045 X2.0 (Drill second hole)
• N050 X3.0 (Drill third hole)
•  
• N055 X4.0 (Drill fourth hole)
• N060 G80 (Cancel cycle
• .
• .

Note the skipped line between N050 and N055. Even though there is nothing in this “command,” the CNC will drill a hole. It will be in the same location as the third hole.