CNC chipload & feed rate calculator

The formulas

The first two lines are printed on every Amana and Onsrud chart. The spindle limit just turns the same formula around. The depth factor is the one the charts give; between 1, 2 and 3 × D we draw a straight line, which is our assumption. The chip-thinning line is the standard radial chip-thinning geometry that Harvey Performance describes: once the stepover falls below half the diameter, the thickest chip gets thinner than the feed per tooth, so the feed per tooth can go up to keep the same chip.

Why small bits rub on hobby machines

Tool makers write their charts for industrial routers: Amana’s 2-flute spiral chart was made at 18,000 rpm, and its solid-wood chart allows up to 24,000. A hobby machine has a trim router whose dial does not go very low, and a frame with a modest top feed. Put the two together and the feed the chart asks for can be faster than the machine can move.

Take a 1/8" (3.175 mm) 2-flute bit in MDF. Amana’s chart says 0.005–0.007" per tooth (0.127–0.178 mm). At 18,000 rpm the feed must be at least 18,000 × 2 × 0.127 = 4,572 mm/min. Sienci lists the LongMill MK2 at 4,000 mm/min in X and Y, so the machine moves at 4,000 and each tooth takes 4,000 ÷ 36,000 = 0.111 mm — below the chart. At the Makita RT0701C’s lowest 10,000 rpm, the same chip load needs only 2,540–3,556 mm/min, which fits. The DeWalt DWP611 cannot go below 16,000 rpm, where the minimum is 4,064 mm/min: just over that machine’s limit.

That is the case for single-flute bits on small machines: one flute at the same rpm and feed takes twice the chip. It is also why the calculator shows the fastest spindle speed that still works, not only the feed.

Router speeds and machine feeds we used

Machine limits are the maker’s figures for cutting moves. On a GRBL controller your real limit is whatever $110 and $111 are set to; type that into the calculator.

Chart chip loads for 1/8" and 1/4" bits

Sizes between chart rows are interpolated by us on a log scale; sizes below the smallest row (the wood charts start at 1/8") are scaled down in proportion to the diameter, which is our estimate, and the calculator labels both. Onsrud’s MDF chart for small bits in its 64-000/65-000 series is lower again — 0.001–0.003" at 1/16" — so treat tiny bits with care.

Depth and stepover

Deep passes load the bit more: both Amana and Onsrud cut the chip load by 25 % at a depth of twice the diameter and by 50 % at three times. Light stepovers do the opposite. When the bit only engages a narrow strip on the side, each tooth enters and leaves the material quickly and the chip never reaches the full feed per tooth; that is why adaptive and finishing passes can run a higher feed per tooth. The calculator applies both and shows the chip the tooth really takes.

For V-carving depths and ball-nose finishing stepovers, see the V-bit depth and scallop calculator. More calculators are on the tools page.

Where to buy a desktop CNC

TwoTrees sells the TTC series of desktop CNC routers. We have not tested them; check the listing for the spindle speed range and top feed, then put those numbers into the calculator above. Affiliate link: it goes to TwoTrees’ store through Awin, and we may earn a commission if you buy, at no extra cost to you.

FAQ

How do I calculate the feed rate for a CNC router?

Feed rate = spindle rpm × number of flutes × chip load. A 1/8" 2-flute bit in MDF at Amana’s 0.005" chip load and 18,000 rpm needs 18,000 × 2 × 0.005 = 180 in/min (about 4,570 mm/min). Turn it around to check a setting: chip load = feed ÷ (rpm × flutes).

What chip load should I use for MDF and wood with a 1/8" bit?

Amana’s 2-flute spiral charts give 0.005–0.007" (0.13–0.18 mm) for MDF, 0.003–0.005" (0.08–0.13 mm) for hardwood and plywood, and 0.006–0.008" for softwood in its solid-wood chart. Those are written for industrial routers at 18,000–24,000 rpm; on a light hobby machine start at the low end and cut shallower.

Why does my CNC bit burn the wood?

Usually the chip is too thin: the bit spins fast while the machine moves slowly, so each edge rubs instead of cutting. ToolsToday notes that too little chip load causes rubbing, heat and early dulling. On a hobby machine the feed is often capped by the machine’s top speed, so the fix is to turn the spindle down, not just to feed faster.

Should I use a single-flute bit on a hobby CNC?

Often, yes. At the same rpm and feed, one flute takes twice the chip of two flutes. If your router cannot turn slower than about 10,000–16,000 rpm and your machine tops out at a few thousand mm/min, a single flute is the easiest way to get a real chip. Amana also publishes single O-flute charts for plastic and aluminum (written at 18,000 rpm, like its other charts).

Sources

• Amana Tool, Spektra coated spiral plunge 2-flute chart (18,000 rpm; depth factors), 2-flute spiral for solid wood (DLC), plastic single O-flute (v9) and aluminum single O-flute (v9).
• Onsrud Cutter, MDF cutting data (chip load by series and diameter; depth factors).
• ToolsToday, Understanding CNC feeds and speeds (rubbing, heat and breakage; single-flute bits).
• Harvey Performance, Combat chip thinning (below 50 % stepover the chip gets thinner).
• Makita, RT0701C; DeWalt, DWP611; Sienci, LongMill MK2 specifications; SainSmart, PROVerXL 4030 V2.

Last checked 2026-11-01 · Calculated from the tool makers’ charts; no CNC machine was used to make this page.