One of the first challenges for a new CNC user is to determine the correct feed and speed rates for the machine, and those can vary quite a bit.
When the first router bit breaks (and it will), many new users commit a rookie mistake by dramatically reducing the feed rate. This feels logical because the machine is no longer breaking bits at the slower rate of travel, but the operator has unwittingly created a different and less immediately visible problem. Not only will it take longer to cut the parts, but now the bit is wearing at an accelerated rate. So, slowing down feed rate creates a new set of problems. And that begs the question, how does one determine optimal feeds and speeds?
First off, let’s define that. There are two elements here – how fast the tool is spinning (that is, spindle speed), and how fast the cutter is moving through the material, which is the feed rate. Other factors also matter. For example, how deep is the tool cutting (pass depth, or depth of cut), and how wide is the cut (stepover). Characteristics of the tooling (cutter) and the CNC router also enter in. For example, how many teeth are on the tool? And is this an industrial class CNC router, or a hobbyist machine?
A useful concept for determining appropriate feeds and speeds is the concept of chip load. This in essence describes the amount of work being done each time a tooth or carbide insert passes through the material being cut. Think of hand planes for a minute. The depth that a plane iron extends below the sole determines the thickness of the ribbon of wood (shaving) being removed. In the case of a router bit, the equivalent workload is determined by three factors. The first is the feed rate. The faster the tool is fed to the material, the bigger the bite. Next is the spindle speed. A slower rotation results in a larger bite, while a faster spindle speed results in a smaller bite. And the third factor is how many cutters (flutes) are on the bit. For each revolution of a single flute tool, one chip is produced. If the tool has two flutes, then two chips will be produced each time it rotates. With the same feed rate, depth setting, diameter and spindle speed, a two-flute bit will remove the same amount of material but will produce chips that are half as thick as those made by a single flute tool.
Finding the balance
To maximize productivity, woodshops need to cut parts as quickly as possible. Theoretically, this would encourage larger chip loads. But in the case of a router bit, if the forces become too great the bit can actually snap. A shorter, larger diameter bit is capable of handling greater forces than a longer, smaller diameter one. And, of course, bits can handle the forces of a shallow cut more readily than those of a deeper one.
The power and stiffness of the CNC router is also important. A heavy cut will stress the spindle or router as it tries to maintain speed. An industrial CNC router with a powerful spindle will generally be able to sustain heavy cuts without slowing down, but a hobbyist machine using an over-the-counter portable router will experience reduced spindle speed and flex with a heavy cut. It’s important to avoid reduced spindle speed because it will result in a larger chip load, and likely a broken router bit. Keep in mind, too, that forces are less for soft material such as foam or balsa wood, and greater for more dense materials such as ebony or bamboo.
Chip load is determined by multiplying the spindle speed (rpm) by the number of flutes, and then dividing the feed rate in inches per minute (ipm) by the result.
So, how can one use the concept of chip load to determine feeds and speeds for a job? Tool and bit manufacturers often provide a quick and convenient answer in the form of chip load charts or tables. A woodworker can glean a lot of information from these.
For cuts up to about one tool diameter the chip load from the chart is a good bet. For cut depths of two diameters or three diameters the chip load should be reduced by roughly 25 and 50 percent, respectively.
A consumer router that is cutting at 20,000 rpm can have a high and loud pitch, while the sound level might not be as objectionable at 10,000 to 12,000 rpm. Beyond sound, the spindle speed is also related to safety. Smaller diameter tools are usually specified to operate safely at higher speeds. Larger tools such as facing bits may have specified maximum rpm as low as 8,000 or lower, but these bits also can’t be run too slowly. Routers and spindles usually need to operate at higher spindle speeds to develop their full torque and power. Special commercial spindles are available to run at spindle speeds less that 8,000 rpm, but they are not standard.
Heat is a significant contributor to reduced tool life. A tool will remain sharper and perform for longer if it is operated at lower temperature (and that’s not necessarily at slower speed). The proper chip load requires fewer cutting passes through the material, and thicker chips carry heat away from the cutting process more effectively than thin chips.
So, here’s how to determine the correct feed rate and spindle speed. Pick a chip load based on the tool diameter and material (see the manufacturer’s guidelines). Reduce the chip load if the depth of cut is going to be greater than the tool’s diameter. Make sure the spindle speed is appropriate for the tool, the machine and the material. And then calculate the feed rate based on the chip load, the spindle speed and number of flutes.
Let’s apply this process to two examples. First, let’s imagine that a 1/4” MDF template needs to be made for pattern routing some furniture parts. The shape is such that there are no small internal corners, so the part can be cut with a two-flute, 1/2” diameter square (flat bottom) bit. The Vortex chart specifies a chip load of .025-.027”. The toolpath can be set to cut the part in a single pass without cutting more than the tool diameter. No adjustment is required for depth of cut in this thin material. The CNC router uses an industrial spindle that operates comfortably at 18,000 rpm.
Here’s the calculation: 18,000 rpm x two flutes = 36,000. Multiplying that by the recommended chip load (.026”) suggests a travel speed of 936 inches per minute.
Now, that’s a pretty high feed rate for smaller routers. If one changes the CNC feed rate to 400 ipm, and the spindle speed to 10,000 while retaining the two flutes, the chip load is reduced to .020”.
Again, there’s a problem. The chip load chart says that a .020” chip load is at the low end of the range for MDF with a 3/8” diameter bit. So, the woodworker might choose to switch to a 3/8” bit or proceed at the lower spindle speed with the original 1/2” bit knowing that the chip load is not what it could be. Operating that way for long periods might not deliver the longest bit life, but the operator may decide that this is close enough for this single job.
In the second example, an ebony fret board for a guitar needs to have slots machined for the fret wires (metal inserts that are inlaid along the neck). The slots will be .023” in width and need to be set .076” deep. Here, the woodshop can use a specific bit called a fret-wire kerf cutter. It comes with three flutes and the required .023” diameter. The manufacturer of the bit recommends a chip load of 3 percent of the tool diameter as a conservative starting point for testing.
So, the initial chip load will be .00069”, which is 3 percent of .023”. The manufacturer recommends an initial pass depth of half the tool diameter, which is 0.011” (half of 0.023”). The operator now thinks about the depth and chooses to cut the slots in seven passes, taking .011” per pass. For a clean cut, the manufacturer recommends operating at high rpm, and the spindle goes to 21,000.
21,000 rpm x three flutes x .00069” chip load = 43 ipm.
Compared to the MDF template example above, this is an extremely delicate cut in very hard wood. However, the chip load process for determining the speed and feed for this cut is just as accurate for this delicate cut as it was for the relatively heavy cut in the MDF.
The bottom line here is that chip load is a powerful tool for determining feeds and speeds for CNC routers.
Ted Bruning is a furniture maker and college instructor in Colorado Springs, Colo.
This article originally appeared in the August 2020 issue.