Chipload: the CNC feeds and speeds number that matters most
Chipload is how thick a chip one flute cuts in one revolution. Feed rate divided by (RPM times number of flutes). Too thin and the bit rubs instead of cutting, which makes heat, burning and dull edges. Too thick and it deflects, chatters or breaks.
What it actually is
Picture the bit spinning and moving forward at the same time. Every time a cutting edge comes around, the bit has moved forward slightly since the last edge passed. That small distance is how much material this edge has to remove, and that is the chipload.
Feed rate in inches or millimetres per minute, RPM in revolutions per minute, flutes as a plain count. The answer is a distance per tooth: inches per tooth or millimetres per tooth.
Pick the chipload you want from your bit maker's chart, choose an RPM your machine is happy at, and this tells you how fast to drive it.
Why it matters more than any other single number
A cutting edge is a wedge. To cut, it has to bite into material thicker than the tiny radius of its own edge. If the chip is thinner than that, the edge cannot get under the material, so it skids across the surface instead, pressing and heating rather than slicing.
That one mechanism explains most beginner problems at once:
- Burning. Rubbing turns cutting energy into heat. See burning.
- Bits going dull fast. Heat is what destroys a carbide edge, and rubbing makes heat.
- Broken small bits. A dull hot bit takes more force to push, which is what snaps a 1/8 inch cutter.
- Fine dust instead of chips. A visible, checkable symptom of the same thing.
- A cut that sounds like screaming. The pitch of a rubbing cut is distinctive once you have heard it.
What chips should look like
Chips are free feedback and they are lying on the table in front of you. Look at them at the end of every unfamiliar cut, and you will learn faster than any chart can teach you.
Where the starting numbers come from
Spec Router bit manufacturers publish chipload ranges by material and cutting diameter. Those are the numbers to start from, because they were determined with that specific tool geometry. Onsrud, Amana, Whiteside, Vortex and others all publish charts, and most bit listings will tell you the recommended range if you look.
Rule of thumb In the absence of a chart, the pattern is simply that chipload scales with cutting diameter. Small bits take small chips. Published wood ranges run from thousandths of an inch for very small cutters up to a couple of hundredths for large ones. The calculator below flags whether your number is in the ballpark for your diameter.
Working example
A two flute 1/4 inch upcut in hard maple. Your bit chart says 0.008 to 0.011 inches per tooth for this diameter in hardwood. You pick 0.009. Your router runs comfortably at 16,000 rpm.
Which is a real number on a rigid machine and an unreachable one on a light hobby gantry. That is the moment to notice that the problem is not the maths, it is the machine.
If 288 inches per minute is beyond your machine, you have three honest options, and one dishonest one:
- Drop the RPM. At 10,000 rpm the same chipload needs 180 in/min. Still fast, but closer.
- Use a single flute bit. Halves the required feed for the same chip thickness. This is why single flute cutters are so common on hobby machines.
- Accept a lower chipload and manage the heat. Shallower passes, good chip clearing, and watch for burning.
- The dishonest one: run 60 in/min at 20,000 rpm, get a chipload of 0.0015, and wonder why everything burns.
What chipload does not tell you
Chipload says nothing about how much of the tool is buried. You can have a perfect chipload and still stall the machine by taking a full depth slot with a 1/2 inch bit. For that side of the picture see depth per pass, stepover and material removal rate.