Two equations, and everything else is judgement
Spindle speed comes from surface speed and diameter. The cutting edge wants to travel through the metal at a particular number of surface feet per minute, and how fast the spindle has to turn to deliver that depends entirely on how far the edge is from the centre. The exact form is RPM = SFM x 12 / (pi x diameter). The shop shorthand is RPM = SFM x 3.82 / diameter, which is the same thing with 12/pi collapsed into a constant, and it agrees with the exact form to better than a tenth of a percent.
Feed rate comes from chip load. Every tooth on the cutter is supposed to peel off a chip of a certain thickness, and the table has to move fast enough to present that much material to each tooth as it comes around. Inches per minute equals RPM times the chip load per tooth times the number of teeth. Drilling and turning use one number per revolution instead of per tooth, so the flute count drops out.
That is the whole calculation. What is not in it is rigidity, coolant, tool overhang, how sharp the tool is, whether the workpiece is clamped or hanging, and what the specific alloy and heat treatment actually are. Published surface speeds are starting points collected from tools running in conditions that are not yours. The machine and the cut tell the truth: a chatter you can hear, a chip that comes off blue, an edge that dulls in ten minutes. Move one variable at a time and let the evidence set the numbers.
Starting surface speeds
These are the figures behind the material dropdown. Carbide runs three to four times faster than high speed steel because it keeps its hardness at temperatures that would anneal HSS, which is also why carbide dislikes interrupted cuts and light dwelling passes.
| Material | HSS (SFM) | Carbide (SFM) |
|---|---|---|
| Mild steel 1018 / A36 | 90 | 350 |
| Alloy steel 4140 annealed | 60 | 250 |
| Tool steel hardened | 30 | 150 |
| Stainless 304 / 316 | 50 | 200 |
| Gray cast iron | 80 | 300 |
| Aluminum 6061 | 300 | 800 |
| Brass and bronze | 200 | 600 |
| Titanium alloy | 30 | 120 |
Cobalt HSS is credited with about 25 percent more than plain HSS here, and coated carbide about 30 percent more than uncoated. Those multipliers are conventions rather than measurements, and a specific coating on a specific tool in a specific alloy can beat or miss them by a wide margin. The tool manufacturer publishes numbers for their own product; those beat anything generic.
Chip load, and why it scales with diameter
A chip load has to be small enough that the tooth can carry the chip out and large enough that the edge gets under the material rather than rubbing across it. The upper bound is set by how much load the cutter can take without deflecting or snapping, which scales with its cross-section, so a half inch end mill tolerates several times the chip load of an eighth inch one. This page starts from a chip load for a half inch cutter and scales it linearly with diameter, clamped so that very small and very large tools do not run away from reality.
Too light is the more common mistake and the more expensive one. A cutter fed too slowly does not cut, it burnishes, and the heat goes into the edge instead of leaving with the chip. In stainless it work hardens the surface so the next pass has to cut through a harder skin than the one before. If the chips coming off look like dust rather than curls, the feed is the first thing to raise.
Radial engagement changes the answer
When the cutter is engaged less than half its diameter radially, the chip it actually takes is thinner than the feed per tooth you programmed, because the arc of engagement no longer reaches the full width. This is radial chip thinning, and the correction is to increase the feed so the real chip thickness lands back where you wanted it. High speed machining strategies lean on this heavily: very light radial engagement, deep axial cut, feed cranked well past what the table above suggests.
The calculator flags the condition but does not apply the correction, because the right compensation depends on the strategy and on what your controller and machine can actually keep up with. Treat the feed it gives as a conservative floor for a light radial cut.
Where this sits next to the rest of the shop
Speeds and feeds decide how the cut goes. What you are cutting into and how much of it there is are separate questions: the metal weight calculator handles stock weight and cost, the tap drill size calculator handles the hole before the tap goes in, and the cut list optimizer handles getting parts out of sticks with the least waste. For thermal growth between a cold measurement and a hot cut, the thermal expansion calculator covers it.
Questions people ask
What RPM should I run a 1/4 inch end mill at?
In aluminum with a carbide cutter, around 12,000 RPM if your spindle will do it, from 800 SFM divided by a quarter inch. In mild steel with the same cutter, around 5,300. In 304 stainless, around 3,000. In all three cases the arithmetic is identical and only the surface speed changed. If your machine tops out below the ideal figure, run at the maximum you have and reduce the feed rate in the same proportion, which keeps the chip load per tooth where it belongs. A cut that is slower than optimal finishes the part. A cut at the right RPM with the feed left too high snaps the cutter.
What is the difference between chip load and feed rate?
Chip load is the thickness of material one tooth removes on one pass, measured in thousandths of an inch. Feed rate is how fast the table moves, in inches per minute. Feed rate is what you type into the machine and chip load is what the cutter actually experiences, and the bridge between them is the spindle speed and the flute count. A four flute cutter at 3,000 RPM taking 0.002 per tooth needs 24 inches per minute. The same cutter with two flutes needs 12. People who change cutters without changing the feed are quietly halving or doubling the load on every edge.
Should I use more flutes or fewer?
Fewer flutes give each chip more room to escape, which matters enormously in aluminum where a packed flute welds the chip to the cutter and ends the tool. Two and three flute cutters are the aluminum standard for that reason. More flutes put more edges in the cut per revolution, which gives a better finish and a higher feed rate at the same chip load, and steel and cast iron produce short chips that clear easily, so four flutes and more are normal there. Flute count also changes rigidity: a four flute cutter has a thicker core than a two flute of the same diameter and deflects less.
Why do my numbers not match the tool manufacturer's catalogue?
Because theirs are measured on their product and these are generic starting points for a material family. A specific coated carbide end mill in a specific alloy may be rated at double the surface speed used here, and the manufacturer has the test data to back it. Their figures also assume the depth of cut, coolant and rigidity they tested at, which is why their tables have several columns. Use the manufacturer figure when you have one for the tool in your hand. Use this when you have an unmarked cutter out of a drawer and need somewhere sensible to start.
Does this work for a router or a hobby CNC?
The arithmetic is the same and the constraints are not. A trim router spindle will happily produce the RPM that a small cutter in aluminum wants, but the machine underneath it usually cannot deliver the feed rate that pairs with it, and cannot resist the cutting forces without deflecting. On a light machine the practical approach is to reduce the depth and width of cut hard, keep the chip load in range rather than dropping it, and accept a lower removal rate. Chatter, a poor finish and broken cutters on a light gantry are almost always a rigidity problem being treated as a speeds problem.