CNC Chip Load Chart for Wood: Feeds and Speeds

A chip load chart is not a table of magic numbers. It is a way of stating one target: how thick a shaving each cutting edge should take. Everything else on a desktop CNC router, feed rate, spindle RPM, flute count, is arithmetic wrapped around that target.

This page gives starting ranges by bit diameter and material, shows the formula that connects them, and then covers the part most charts leave out: what to do when a desktop machine physically cannot reach the number the chart asks for.

The formula

Chip load, also written as feed per tooth, is the thickness of material one cutting edge removes per revolution.

Feed rate (IPM) = RPM x number of flutes x chip load (inches)

Rearranged, to check what a program is actually doing:

Chip load = feed rate / (RPM x number of flutes)

That second form is the useful one. Take any job that burned or chattered, divide the feed by the spindle speed and the flute count, and compare the result against the ranges below. In most cases the answer explains the problem without any further diagnosis.

Feed rate is proportional to each of the three terms, so the chip responds in opposite directions depending on which one you touch. Doubling the feed rate at fixed RPM doubles the chip. Doubling RPM at fixed feed halves it. Moving from a two flute to a four flute cutter at the same feed and speed halves it again, which is why four flute cutters cause so much burning in wood.

Feed rate in G-code is the F word and is interpreted in units per minute in the normal G94 feed mode, with S setting spindle speed. Both LinuxCNC and grbl follow that convention, so the number your CAM software emits is the number the machine tries to move at, subject to the limits covered further down.

Starting chip load ranges for wood

These are starting ranges for solid carbide spiral cutters in wood and wood composites, expressed in inches per tooth. They are the ballpark that router tooling manufacturers publish in their cutting data tables; the exact figure for a specific cutter belongs to the company that made it, and their sheet always wins over a generic chart.

Bit diameter	Hardwood (oak, maple, walnut)	Softwood (pine, cedar, poplar)	MDF and plywood
1/8 in (3.175 mm)	0.003 – 0.005 in	0.004 – 0.006 in	0.005 – 0.007 in
1/4 in (6.35 mm)	0.008 – 0.012 in	0.010 – 0.015 in	0.012 – 0.018 in
3/8 in (9.5 mm)	0.012 – 0.016 in	0.014 – 0.019 in	0.016 – 0.022 in
1/2 in (12.7 mm)	0.015 – 0.021 in	0.018 – 0.025 in	0.020 – 0.028 in

Two things about this table matter more than the numbers themselves.

Chip load scales with diameter. A 1/8 inch cutter is not a small version of a 1/4 inch cutter with the same settings. It has a fraction of the cross section, so it takes a fraction of the bite before it snaps. Any chart or calculator that offers a single chip load per material, ignoring diameter, will break small bits and under-drive large ones.

Species matters less than you would expect, and density matters more. The Wood Handbook published by the USDA Forest Products Laboratory catalogues specific gravity and mechanical properties across species, and it is density and moisture content rather than the common name that predict how a species machines. Treat the hardwood column as a proxy for dense stock, not as a botanical classification. Very dense tropical species sit below the hardwood column; light balsa-like stock behaves closer to the softwood column than to anything else.

Composites are their own case. MDF cuts easily and tolerates a thick chip, but its resin binder is abrasive and it dulls edges faster than solid wood. Plywood is a stack of alternating grain directions with glue lines in between, which is a tearout problem rather than a chip load problem, and it is solved with bit geometry rather than feed rate.

Depth of cut and radial engagement

The chart assumes a reasonable cut. Two adjustments apply once the cut stops being reasonable.

Depth of cut. A common rule of thumb caps depth per pass at roughly one bit diameter in softwood and half a diameter in hardwood, and that is a guide about cutting force, not about chip thickness. On a light desktop gantry the frame gives way long before the cutter does, so shallower passes at full feed usually beat one deep pass at reduced feed. Reducing feed to survive a deep pass is the classic way to turn a cut into a burn.

Radial engagement and chip thinning. When a cutter takes a light side pass, less than about half its diameter of radial width, the actual chip comes out thinner than the programmed feed per tooth suggests, because the arc of engagement is short. That is why a light finishing pass at the same feed as the roughing pass can start rubbing. Finishing passes generally want a feed rate increase, not a reduction. Some CAM packages apply this correction automatically under a “chip thinning” or “adaptive” option.

Slotting is the opposite case. A slot is full radial engagement with nowhere for chips to go, so it is the most demanding operation in the program and the one to set conservatively.

For a fuller treatment of how cut direction, depth of cut and stepover interact with frame rigidity, see climb vs conventional and stepover on a CNC router.

Why your machine may not reach the chart

Put realistic numbers into the formula and a problem appears immediately. A 1/4 inch two flute cutter at 18,000 RPM, targeting 0.012 inches per tooth in hardwood, wants:

18,000 x 2 x 0.012 = 432 IPM

Very few hobby class machines will move at 432 inches per minute while cutting. Belt driven gantries are commonly configured somewhere between 100 and 200 IPM of usable cutting feed, and the machine’s own firmware enforces a ceiling: in grbl the $110, $111 and $112 settings define the maximum rate per axis, and any faster feed in the G-code is silently clamped to that value. The controller does not warn you. It just runs slower than the program asked, and the chip load quietly collapses.

There are only two honest ways out.

Drop the spindle speed. This is the fix nearly everyone misses, because the instinct is to treat RPM as a power setting. Rearrange the formula for RPM instead:

RPM = feed rate / (flutes x chip load)

At a 150 IPM machine ceiling with a two flute cutter and a 0.012 inch target, that gives 6,250 RPM. Most compact trim routers cannot go that low; their variable speed dials typically bottom out somewhere around 10,000 RPM, which is exactly why a trim router forces a thinner chip than the chart wants. A VFD spindle that runs down to 6,000 or 8,000 RPM removes the constraint outright, and that single capability is a real reason to prefer one.

Use fewer flutes. A single flute cutter halves the required feed rate compared with a two flute at the same chip load. In wood this costs less than it sounds, because the larger flute valley of a single flute cutter also clears bulky wood chips better.

If neither is available, accept a thinner chip and manage the consequences: take shallower passes, keep the cutter moving, and expect shorter tool life. That is a compromise, and it is worth knowing you are making it.

Run your own numbers through the feed rate and chip load calculator on this site, which cross checks the result against a machine feed ceiling and tells you the RPM you would actually need.

Troubleshooting from the chart

Most cut quality complaints map to a chip load that is wrong in a specific direction.

Symptom	Most likely cause	Correction
Scorched brown edges, fine dust instead of chips	Chip too thin, edge rubbing rather than cutting	Raise feed rate, lower RPM, or move to fewer flutes
Chatter, ridged wavy walls, squealing	Cutting force exceeds frame or workholding rigidity	Reduce depth of cut, shorten tool stickout, check for gantry and workpiece movement
Fuzzy edges and torn top surface	Geometry and grain direction, not feed	Change bit geometry, take a light finishing pass, or score the surface first
Broken small bits	Chip too thick for the cross section, or plunge too aggressive	Use a diameter-specific chip load, ramp or helix into the cut instead of straight plunging
Machine stalls, loses steps, cut shifts mid job	Feed or acceleration beyond what the drive can deliver under load	Lower feed and depth of cut together, verify firmware maximum rate settings
Melted or gummy residue in the flutes	Heat retention, common in resinous softwood and in slots	Thicker chip, better chip evacuation, avoid closed slots at full depth

Note what is missing from that table: “slow down”. Slowing the feed rate is the correct answer only when the failure is a force problem, meaning chatter, deflection or stalling. When the failure is a heat problem, meaning burning, slowing down makes it worse.

Bit geometry decides a large share of the edge quality outcomes above, particularly tearout on the top and bottom faces. Those tradeoffs are covered in upcut vs downcut vs compression CNC router bits.

How to use the chart in practice

Look up the range for your bit diameter and material class, then check the manufacturer’s data sheet for that specific cutter and prefer their number.
Calculate the feed rate at your intended RPM. If it exceeds what your machine can actually sustain, lower RPM until the feed lands inside the machine’s limit.
Cut a test piece in scrap of the same material and thickness, at the depth of cut you plan to use.
Look at the debris. Recognisable chips that leave the cut cool mean you are in range. Fine powder means the chip is too thin.
Adjust one variable at a time and note the setting that worked, by cutter and by material. That record becomes far more useful than any generic chart, including this one.

Machine choice sets the ceiling on all of this, since rigidity and spindle speed range decide how much of the chart you can reach at all. That side of the problem is covered in the desktop CNC router buying guide for woodworking.