Obscure CNC Features That Can Help (or Hurt) You

Metalcutting CNC machines are used for all kinds of applications. This makes CNC users quite a diverse group. What is obvious and important for one user will have no meaning or value for another. Combine this usage diversity with a CNC control manufacturer’s desire to please everyone and you end up with lots of CNC features that are not appropriate for everyone.

That said, you cannot begin to take advantage of an available feature if you do not know it exists. Conversely, you will not know how to avoid CNC features which may be detrimental to your efforts. With this article, I intend to expose a few lesser-known CNC features and provide some dos and don’ts.

Understanding least input increment and sizing adjustments

There was a time many years ago when a CNC machine’s least input increment (the smallest value the CNC could display, or that you could enter or program) was the same as its resolution (smallest motion departure amount for each axis). When working in the imperial measurement system, each was 0.0001 in. In the metric system, each was 0.001 mm.

Over time, CNC manufacturers dramatically improved resolution. With today’s machines, resolution is measured in nanometers. Though CNC manufacturers do provide (optional) increment systems that allow CNCs to display and users to enter smaller values (like 0.00001-in or 0.0001-mm), the standard for current machining and turning centers remains 0.0001 in and 0.001 mm.

This is totally acceptable for most applications. But there is one time, when very small tolerances are involved, that you need a smaller least input increment. Consider a dimension of 3.0 in, +0.0003, -0.0002, the mean value of which (your programmed coordinate) is 3.00005 in.

Though it is not common knowledge, today’s CNCs allow you to program values smaller than the least input increment (like X3.00005), even though the CNC cannot display them. And when making sizing adjustments, you can also enter imperial measurement system values into offset registers out to five places (or metric values out to four places).

Here is a quick test you can use if you are wondering whether a particular machine allows this: In inch mode, set an unused offset register to zero. Now, enter a value of 0.00001. The display will continue showing zero. But when you enter 0.00006, the register will display 0.0001. The CNC simply rounds the display to the nearest four places. The CNC will correctly detect and use the small value, even though it cannot display it.

Rapid using linear or nonlinear motion

Traditionally, when more than one axis is commanded in a rapid motion command (G00), all commanded axes will move at their rapid rates. If one axis must move further than another, it will take longer to reach its destination and the motion will not be along a straight line. If you are not careful, this can result in a collision since the cutting tool will “dogleg” into position.

Newer CNCs allow you to specify with a parameter setting that you want rapid motion to occur in a linear manner. With a FANUC 30 series control, for example, parameter 1401, bit 1 (second bit from the right) provides this choice. If set to zero (0), rapid motion will occur in a nonlinear (dogleg) fashion. If this bit is set to one (1), rapid motion will be linear.

Be careful with machine lock

There was a time when most FANUC operation panels included an on/off switch labeled “Machine Lock” — and possibly another labeled “Z-Axis Feed Neglect.” If turned on, axes would be kept from moving — all axes with Machine Lock or just the Z-axis with Z Axis Feed Neglect. While these functions could be helpful during a program’s verification to test a program for syntax errors, they are also the cause of mishaps (crashes) if not used properly.

When either of these switches is on, the CNC thinks the axes are moving even though they are not. If the axes are not left at the same position where they started, the coordinate system will be out of sync with the CNC. In essence, the machine loses position.

Older machines actually required cycling the power to reset the coordinate system. Newer CNCs do so when you perform a manual reference return. If any of your machines has either of these switches, be sure you fully understand how it works before you use it.

When maximum feedrate isn’t fast enough

Most CNCs have very fast and highly publicized rapid rates. What is not so well documented is how fast they can move axes when in a cutting mode. In most cases, the maximum feedrate will be fast enough, but there is one possible exception related to chasing very coarse threads on a turning center.

Consider a four-start thread having a pitch or 0.125 in. The lead of this thread is 0.5 in, meaning the threading tool must feed at 0.5 ipr when threading. Say this thread is machined into a 1.5-in diameter and the recommend speed is 500 sfm. The resulting speed will be 1,273 rpm, and at 0.5 ipr, a feedrate of 686 ipm will be required to accurately machine the thread’s lead.

Most turning centers cannot feed this fast, but no alarm will be sounded. The machine will do its best, but the thread lead will not be correct. This can be a difficult issue to diagnose.