Chipload is the number that matters; RPM and feed are just how you deliver it
A cutting edge is a wedge. It works properly only when it takes a chip thick enough to shear the material cleanly ahead of the edge. Too thin and the edge rubs instead of cutting: the material deflects under the tool, springs back behind it, and the energy goes into heat rather than into chips. That is what burns wood, melts plastic and work-hardens aluminium, and it dulls the cutter far faster than a heavy cut does.
The thickness of that chip is the chipload — feed per tooth per revolution. Every bit manufacturer publishes it for each cutter diameter and each material, and it is the one number you should take from a table rather than guess. Everything else in feeds and speeds is arithmetic around it.
Feed rate is chipload delivered: each revolution presents every flute to the work once, so the tool advances by chipload × flutes per revolution, and RPM converts that into distance per minute. Doubling the RPM without doubling the feed halves the chipload and moves you towards rubbing. Halving the feed to "be gentle" on a burning cut usually makes the burning worse, which is the single most common mistake new router users make.
The three relations, and why the router world starts at a different one
Feed = RPM × flutes × chipload. That is the whole of it in the router world, where you pick a spindle speed you know the machine likes and a chipload from the bit maker's chart.
RPM = SFM × 12 ÷ (π × D) is where metalworking practice starts instead. Surface speed — feet per minute at the outside of the cutter — is a property of the material and the tool coating, not of the tool size, because it governs the temperature at the edge. The 12 converts feet to inches, and πD is the circumference the edge travels per revolution. In metric the same relation is RPM = Vc × 1,000 ÷ (π × Dmm) with Vc in metres per minute.
Routers work from RPM because their spindles run in a narrow band, typically 10,000-24,000 rpm, and small cutters at those speeds already exceed the surface speed limits of the materials involved. Wood tolerates that; aluminium in a router does too, provided the chipload is honest and the chips clear.
Radial chip thinning is the correction that catches people out. When the stepover is less than half the cutter diameter, the edge is only engaged over a short arc, and the chip it takes is thinner than your programmed chipload — geometrically thinner, by the factor D ÷ (2√(ae(D − ae))). At a stepover of D/8 that factor is 1.51, meaning the real chip is only two thirds of what you asked for. To restore it, feed 1.51 times faster. This is why light finishing passes at conservative feeds burn: the pass is light, so the chip is thin, so the tool rubs.
At exactly half the diameter the factor is 1, and above half the diameter chip thinning no longer applies. Full-width slotting is the worst case for heat and chip evacuation but needs no feed correction at all.
Worked example: a 1/4 inch two-flute cutter in hard maple
You are pocketing hard maple with a 0.25 inch two-flute upcut spiral. The bit maker lists a chipload of 0.006 inch per tooth for this diameter in hardwood. Your spindle holds 18,000 rpm comfortably. You plan 0.25 inch depth per pass and a 0.125 inch stepover.
- Feed rate. 18,000 × 2 × 0.006 = 216 in/min, which is 216 × 25.4 = 5,486 mm/min.
- Surface speed check. 18,000 × π × 0.25 ÷ 12 = 1,178 SFM. High by metalworking standards and entirely normal for wood.
- Chip thinning. The stepover of 0.125 inch is exactly half the diameter, so the factor is 1.000 and no compensation is needed.
- Removal rate. 0.25 × 0.125 × 216 = 6.75 in³/min.
Now change one thing: drop the stepover to 0.03125 inch (D/8) for a finishing pass. The thinning factor becomes 0.25 ÷ (2√(0.03125 × 0.21875)) = 0.25 ÷ 0.16536 = 1.512, so to keep the same real chip you must feed 216 × 1.512 = 327 in/min. If instead you slowed to 100 in/min because it is a finishing pass, the actual chip per tooth would be 100 ÷ (18,000 × 2) = 0.0028 inch, and after thinning the true chip is 0.0018 inch — deep in the rubbing regime, and the edge of your pocket will scorch.
If 327 in/min is beyond your machine, the answer is not to feed slower: it is to reduce RPM. At 10,000 rpm the same 0.006 chipload needs only 120 in/min uncompensated, 181 in/min compensated.
Reading the results, and what to change when the cut goes wrong
Burning, melting or a polished tool means the chip is too thin. Raise the feed or lower the RPM; both raise chipload. In plastics, melted chips welding back into the cut are the classic sign, and a single-flute cutter with a large chipload fixes it where a slower feed never will.
Chatter, a rough edge or a snapped bit usually means too much engagement rather than too much chipload. Reduce the depth of cut first, then the stepover; keep the chipload. A long, thin bit deflects, and deflection makes a chattering cut worse the deeper it goes.
Material removal rate is your throughput number and the honest way to compare strategies. A shallow, fast, light-stepover pass and a deep, slow, full-width pass can remove the same cubic inches per minute at very different tool loads. High-efficiency toolpaths — adaptive clearing, trochoidal milling — exploit exactly this: a small stepover with a deep axial engagement and a very high compensated feed, keeping the tool cool because each edge is in the cut briefly.
Surface speed is the sanity check on the tool rather than the machine. Carbide in wood tolerates 1,000-2,000 SFM without complaint. Carbide in aluminium is usually run in the hundreds of SFM, and a 1/4 inch cutter at 18,000 rpm is already at 1,178 SFM — which works only with strong chip evacuation, ideally air blast or mist, and a chipload large enough that the chips carry the heat away.
Router work and 3D printing often share a shop; if you are costing machine time across both, the print job cost calculator uses the same hourly-rate logic, and the board feet calculator handles the material side when you are cutting hardwood.
Typical chipload starting points for a CNC router
| Material | 1/8 in cutter | 1/4 in cutter | 1/2 in cutter |
|---|---|---|---|
| Softwood, pine | 0.003-0.005 | 0.009-0.011 | 0.019-0.021 |
| Hardwood, maple and oak | 0.003-0.005 | 0.005-0.007 | 0.015-0.018 |
| MDF and particleboard | 0.004-0.006 | 0.006-0.009 | 0.017-0.020 |
| Plywood | 0.003-0.005 | 0.005-0.007 | 0.014-0.016 |
| Acrylic (PMMA) | 0.002-0.004 | 0.004-0.006 | 0.008-0.012 |
| HDPE and polycarbonate | 0.003-0.005 | 0.006-0.009 | 0.010-0.014 |
| Aluminium | 0.001-0.002 | 0.002-0.004 | 0.004-0.006 |
Bigger cutters take bigger chips because they are stiffer and their edges are stronger. Halving the diameter roughly halves the chipload the tool will survive.
Start conservative, and listen
Published chiploads assume a rigid machine, a sharp tool and secure workholding. A lightweight hobby gantry flexing under load will chatter at feeds a stout industrial router handles without noise. Take the calculated feed as a target, start at 60-70% of it on a scrap piece, and increase until the cut sounds steady and the chips come off as chips rather than as dust. Dust means rubbing. Long stringy chips in metal mean the chipload is too high or the flutes are packing. Never stand in line with a spinning cutter, and never take a cut you would be unwilling to have go wrong.
Mistakes that ruin bits
- Slowing the feed when a cut burns. Burning is thin-chip rubbing. Slowing down thins the chip further and burns harder. Speed up, or reduce RPM.
- Ignoring chip thinning on light stepovers. Below half-diameter engagement the real chip is thinner than the programmed one, by up to two or three times on very light passes.
- Using the shank diameter instead of the cutting diameter. A 1/4 inch shank often carries a 1/8 inch cutter, and everything derived from D is then wrong by a factor of two.
- Slotting at full depth. A full-width slot has the worst chip evacuation of any cut. Keep slotting depth to a fraction of the diameter and let multiple passes do the work.
- Assuming more flutes means more feed. More flutes means less chip room. In wood and plastic, one or two flutes clear chips where four flutes pack and burn.
- Running a dull bit at book numbers. A worn edge needs more force, deflects more and generates more heat, all of which invalidate the chipload assumption.
Where these numbers come from and where they stop applying
The relations here are the standard machining relations set out in Machinery's Handbook, which has published cutting speeds, feeds per tooth and the geometry of chip formation for over a century. The chipload tables that bit manufacturers publish are their own test data for their own geometry, and they differ between makers for good reasons: rake angle, helix, edge preparation, coating and carbide grade all change how much chip a given edge can take.
Three things this calculator does not model. It has no tool deflection term, so it will happily suggest a feed a long 1/8 inch cutter cannot hold without bending. It has no spindle power limit, so on a heavy removal rate it may exceed what a 1 kW router can deliver — as a rough guide, hogging wood consumes a fraction of a horsepower per cubic inch per minute, and aluminium far more. And it assumes a rigid setup: workholding that lets the part move invalidates every number.
For metal cutting specifically, two refinements matter. Climb versus conventional milling changes where the chip is thickest — climb milling starts thick and ends thin, which is preferred on a rigid machine with no backlash and dangerous on a worn manual mill. And coolant or air blast is not optional in aluminium: without chip evacuation the chips re-cut and weld to the flutes, which is how a good bit becomes a broken bit in one pass.
Finally, treat every calculated number as a starting point that you then verify in the material. The chip is the evidence. If it comes off as a well-formed curl at the size you predicted, your numbers are right; if it comes off as dust, they are not, whatever the arithmetic says.