Why Do My CNC Router Bits Keep Breaking?

The counter-intuitive part

Almost everyone's instinct after breaking a bit is to slow down. In wood and plastics that instinct is usually wrong and often makes the next break arrive sooner.

A carbide edge is designed to shear a chip of a specific thickness. When the chip is thinner than that, the edge cannot get under the material — it deflects, skids along the surface and converts the spindle's energy into friction instead of cutting. Friction means heat, and heat is what actually kills carbide. Hot carbide loses toughness, the fine edge crumbles, the tool starts cutting on a damaged edge, forces spike, and the shank snaps.

The diagnostic tell is on the broken bit itself. Blue, brown or straw discolouration near the break means it was running hot before it failed — that is a rubbing failure, and the fix is more feed, not less. A clean silver break with no discolouration points to a mechanical overload instead: too deep a pass, too much stickout, or a plunge the bit was not designed for.

Why the chipload you found online may be wrong for your bit

This is the failure mode nobody warns about. Chipload is published per tool series, not per material, and the spread is much wider than most people expect. These are all published figures for a 1/4″ bit in aluminum, and every one of them comes from a single manufacturer's single catalogue:

The top and bottom of that table differ by 4.5×. Run the 63-000 number on a 61-000 straight bit and you are asking a tool rated for 0.002″ to take 0.009″ — roughly four times its design chip. It will break, and slowing down afterwards will not tell you why.

The same pattern appears in wood. A 1/4″ compression spiral in plywood is published at 0.014″–0.016″ by LMT Onsrud for the 60-100MW series and at 0.0031″ by Amana for their compression line — a 5.2× difference between two reputable manufacturers describing the same cut. Neither is wrong. They are different tools.

So the rule is: get your chipload from the series you are actually holding. Every bit we sell lists its own published figures on its product page, and the same numbers drive our Cut Doctor and feed rate calculator.

Stickout is the multiplier

Tool deflection scales with the cube of the unsupported length. Doubling your stickout does not double deflection — it increases it roughly eightfold. That is why the same bit, same feed and same material can run perfectly one day and snap the next after someone re-set the tool a little longer.

Diagnostic table

Small bits are far weaker than their chipload suggests

Published chipload roughly halves between 1/4″ and 1/8″ — for example Onsrud's 65-000 series drops from 0.004″–0.006″ to 0.002″–0.004″ in hardwood. But bending stiffness falls with the fourth power of diameter, so that same halving of diameter makes the tool about sixteen times less rigid.

That mismatch is why 1/8″ and 1/16″ bits feel so much more fragile than the numbers imply. With small tools, reduce depth of cut aggressively, keep stickout to the minimum that clears the work, and treat the published chipload as a ceiling rather than a target.

Depth of cut starting points

Chipload governs feed, not depth. These are general starting points rather than manufacturer data — verify on scrap:

One exception worth knowing: with a compression spiral, the first pass must be deeper than the upcut section — usually about one bit diameter. A shallow first pass engages only the upcut portion, which lifts and chips the top face.

Bits that tolerate a wider parameter window

Browse the full range in CNC router bits, or use the Bit Finder to match a bit to your material and machine.

Common questions

Why do my CNC router bits keep breaking?

The most common cause is feeding too slowly. Below the published chipload the edge rubs instead of cutting, generating heat that embrittles the carbide until the edge chips and the tool snaps. Look for blue or brown discolouration near the break — that confirms a heat failure and means you should increase feed, not reduce it. The other frequent causes are too much depth per pass, excessive stickout, and chip re-cutting in slots.

Should I slow down the feed rate to stop breaking bits?

Usually no. Slowing the feed reduces chip thickness, which is what caused the rubbing and heat in the first place. If you need to reduce cutting force, reduce depth of cut or stepover instead and keep the chipload in range. If your machine cannot hold the required feed, lower RPM rather than feed — 12,000 RPM at 216 IPM produces exactly the same chip as 18,000 RPM at 324 IPM.

How deep can I cut in one pass?

As a starting point, one to two bit diameters in softwood and plywood, half to one diameter in hardwood and acrylic, and only 0.05 to 0.1 diameters when slotting aluminum. With a compression spiral the first pass must be deeper than the upcut section, roughly one bit diameter, or the top face will chip.

Why do small bits break so much more easily?

Bending stiffness falls with the fourth power of diameter while published chipload only roughly halves. Going from 1/4 inch to 1/8 inch makes the tool about sixteen times less rigid but only allows about half the chip, so small bits are far more fragile than the feed numbers suggest. Minimise stickout and reduce depth of cut.

Chipload figures are manufacturer application data stored per product in our catalogue and cited by series. Verify on scrap, and adjust for your machine's rigidity, hold-down and spindle condition. Depth-of-cut figures are general starting points, not manufacturer specifications.