CNC Speeds and Feeds: What They Are and How to Calculate Them
Ask a new CNC user what “speeds and feeds” means and you will usually get back a number they copied from somewhere. Ask what those numbers are — what each one measures, and why a machine that cut aluminium beautifully burns a tool in steel with the same settings — and the confidence drops sharply. Speeds and feeds look like a list of values to look up. They are actually three different things wearing confusingly similar names, and once you can tell them apart, the numbers stop being magic and become arithmetic.
This is the fundamentals page of the speeds-and-feeds topic. It teaches the vocabulary and the two calculations you will do on every job, with full worked examples in imperial and metric, and it shows how to read the numbers a chart gives you without treating them as gospel. If you want the complete system — how every operation (roughing, finishing, slotting, drilling, turning) changes the recipe, and how to tune it — that is the machining parameters guide. If you want to understand why materials sit where they do on the difficulty scale, that is the materials machinability reference. Definitions of every term below are in the CNC glossary.
Three different “speeds” — and only two are calculated
The single biggest source of beginner confusion is that machining uses the word “speed” for three different quantities. They are not the same thing, they have different units, and they are set by completely different things:
| Quantity | What it measures | Typical unit | What sets it |
|---|---|---|---|
| Cutting speed (surface speed) | How fast the cutting edge moves through the material | SFM (ft/min) or m/min | The material and the tool — chosen first |
| Spindle speed | How fast the spindle (and tool) rotates | RPM | Calculated from cutting speed and tool diameter |
| Feed rate | How fast the tool advances through the work | in/min or mm/min | Calculated from chip load, RPM and flutes |
The mental model that makes everything else obvious: cutting speed is chosen, and spindle speed and feed are derived from it. Cutting speed is set by the material — aluminium wants a high cutting speed, steel a much lower one, titanium lower still. That choice is the whole “which material am I cutting” question, and it is where the materials reference takes over. Spindle speed and feed rate are then pure arithmetic: you convert the cutting speed into an RPM using the tool’s diameter, and you convert a target chip thickness into a feed rate using the RPM and the tool’s flute count. Nothing is “looked up” at the RPM or feed stage if you are doing it properly — those two are computed.
Hold that model and the classic beginner error disappears: beginners ask “what RPM should I use?” as if RPM were the thing the material dictates. It is not. The material dictates the cutting speed. RPM is whatever makes that cutting speed true for the tool you happen to have in the spindle.
Cutting speed: the constant that is independent of tool size
Cutting speed — surface feet per minute (SFM) in imperial, metres per minute (m/min) in metric — is the velocity of the cutting edge relative to the material surface, regardless of how big the tool is. Two different-diameter tools cutting the same material at the same cutting speed are experiencing the same edge temperature and wear, even though one spins much faster than the other.
Why the tool diameter forces the RPM is easiest to picture with wheels. A small wheel and a large wheel on the same axle complete the same number of rotations, but their rims travel very different distances per minute — the large wheel’s rim moves faster. To make both rims travel at the same surface speed, the small wheel must spin faster. So a 3 mm end mill needs several times the RPM of a 25 mm end mill to cut the same material at the same cutting speed. This is the single fact that makes small tools feel scary: they demand spindle speed a machine may not have.
The conversion is the first formula you will use constantly. Turning a cutting speed into a spindle speed:
- Imperial: RPM = (SFM × 12) ÷ (π × tool diameter in inches) — or its everyday shortcut, RPM = SFM × 3.82 ÷ tool diameter in inches
- Metric: RPM = (cutting speed in m/min × 1000) ÷ (π × tool diameter in mm)
The 3.82 is just 12 ÷ π — a convenience constant so you only remember one division.
Worked example, imperial. A ½-inch (0.5”) carbide end mill in aluminium, at a cutting speed of 800 SFM:
RPM = 800 × 3.82 ÷ 0.5 = 6,112 RPM
Worked example, metric. A 10 mm carbide end mill in aluminium, at a cutting speed of 200 m/min (the same material, about the same edge velocity — 800 SFM ≈ 244 m/min):
RPM = (200 × 1000) ÷ (π × 10) = 200,000 ÷ 31.4 = 6,366 RPM
Same material, same cutting speed, nearly the same RPM — because the tool diameters (0.5” ≈ 12.7 mm vs 10 mm) are comparable. Now imagine a 3 mm end mill in that same aluminium: at 200 m/min it wants 200,000 ÷ 9.4 ≈ 21,000 RPM. If your spindle tops out lower, you have hit the machine limit before you have chosen anything — which is why small tools are where beginners break cutters. (More on ceilings below.)
Feed rate: chip load is the number that actually matters
If cutting speed sets the temperature, the feed rate sets the chip thickness — and chip thickness is the true health of the cut. Machinists talk about feed as “chip load,” meaning the thickness of material each cutting edge removes per revolution. A tool that cuts a proper, thick-enough chip is cutting. A tool whose chip is too thin is not cutting at all — it is rubbing, dragging a dull-ish edge across the surface, generating friction heat in the tool instead of chips, and (with work-hardening materials such as stainless and titanium) hardening the very surface it must next cut.
This is why “feed too slow” is a real failure mode and not a safe fallback. Beginners, told that gentler is safer, drop the feed and keep the RPM — and manufacture the worst possible condition: a tool spinning fast enough to burn, feeding too slowly to make a real chip. Reducing feed without reducing speed is how stainless and titanium get work-hardened and burnt-edge failures.
Chip load is expressed per tooth (feed per tooth, sometimes written fz), because a multi-flute tool cuts with all its edges in turn. Feed rate then follows from the second formula:
Feed (in/min or mm/min) = RPM × feed per tooth × number of flutes
Two details make this concrete. First, flute count is not a free multiplier — it is a way to divide the same total feed across more edges. A 4-flute tool can be fed about twice as fast as a 2-flute of the same diameter at the same chip load per tooth, which is why more flutes mean more throughput; but soft, gummy materials like aluminium clog multi-flute tools with big chips, so aluminium work often prefers 2–3 flutes with polished flutes. Second, chip load scales with tool size: tiny tools take a small feed per tooth, big tools a heavier one. The value comes from the toolmaker’s data for the tool diameter — general tables are a starting proxy only.
Worked example, continued. Back to the ½” 4-flute end mill in aluminium at 6,112 RPM. If the toolmaker calls for 0.003 in/tooth:
Feed = 6,112 × 4 × 0.003 = 73 in/min (IPM)
Metric. The 10 mm, 4-flute tool at 6,366 RPM with a chip load of 0.05 mm/tooth:
Feed = 6,366 × 4 × 0.05 = 1,273 mm/min
Turn the formula around and you have the sanity check that catches most mistakes: chip load = feed ÷ (RPM × flutes). If the result is implausibly thin — below roughly a third of the tool’s edge radius — the tool is rubbing, and the fix is to raise the feed, not lower it.
Reading a feeds-and-speeds chart without being misled
Every chart and calculator on the internet is doing the same two-step above: they give you a cutting speed for the material and a chip load for the tool, then they compute the RPM and feed. Understand that pipeline and a chart becomes transparent instead of authoritative. Three caveats matter before you trust any row:
- The numbers assume a tool and a condition. Typical charts assume a plain carbide end mill in a rigid machine. High-speed steel runs at roughly half the carbide cutting speed; coatings raise it by a third or more; and every toolmaker’s own data for their specific tool overrides any general table.
- Different charts disagree by a factor of two. One source’s “mild steel 300–600 SFM” is another’s “80–400”. Neither is lying — they assume different tooling, rigidity, coolant and risk tolerance. Use charts for the shape of the answer and start low.
- The material row is a direction, not a law. The full reasoning about why each material behaves as it does — and where the engineering plastics sit — is in the materials reference. Here is the starting-point version for a typical carbide end mill, deliberately rounded so the ordering is what sticks:
| Material | Carbide cutting speed (starting) |
|---|---|
| Aluminium alloys | 500–1,000 SFM (150–300 m/min) |
| Engineering plastics | 400–800 SFM (120–250 m/min) — heat-limited, needs sharp tools |
| Brass / bronze | 300–600 SFM (90–180 m/min) |
| Mild / low-carbon steel | 200–400 SFM (60–120 m/min) |
| Alloy steel, annealed | 200–300 SFM (60–90 m/min) |
| Cast iron | 150–300 SFM (45–90 m/min) |
| Stainless (300-series) | 100–200 SFM (30–60 m/min) |
| Titanium alloys | 60–120 SFM (20–40 m/min) |
| Nickel alloys | 40–80 SFM (12–25 m/min) |
Rounded starting points for a carbide end mill in a rigid setup. HSS ≈ half; coated carbide can go higher; toolmaker data wins. Start at the low end and tune.
Notice what the ordering teaches: the SFM ladder is the machinability ladder. Aluminium and the plastics sit at the top because they conduct heat away or soften before they can hurt the tool; steel, stainless, titanium and nickel descend as heat retention, work hardening and hot strength take over. That is exactly the spectrum the materials reference explains in physical terms.
Two jobs, end to end
To see the model work, run two real cases through it.
A slot in aluminium, ½” 4-flute carbide. Aluminium calls for 800 SFM; from the table, a reasonable starting chip load for a ½” tool is about 0.003 in/tooth. That gives 6,112 RPM and 73 IPM — the arithmetic above. But a slot is the worst case in milling: the tool is fully buried, its whole diameter engaged, so it cannot shed chips and the load peaks. The beginner’s answer is to keep the RPM but fear the feed; the machinist’s answer is to keep the chip load honest and reduce the engagement — lighter axial passes, or a peel/HEM-style path that engages a fraction of the diameter. If you must slot conventionally, drop the cutting speed toward the low end (and the RPM and feed with it, keeping the chip load constant) rather than starving the feed.
A small tool in steel, where the machine is the limit. A ⅛” (0.125”) 4-flute carbide end mill in mild steel at 300 SFM wants RPM = 300 × 3.82 ÷ 0.125 ≈ 9,200 RPM — beyond many machines’ ceiling. Now the machine limit becomes part of the calculation: run at the spindle’s maximum (say 8,000 RPM), which delivers an actual cutting speed of 8000 × 0.125 ÷ 3.82 ≈ 262 SFM — a little lower than ideal, perfectly workable. Keep the chip load (say 0.0015 in/tooth for a small tool) and the feed follows: 8000 × 4 × 0.0015 = 48 IPM. The chip load stayed honest, so the tool cuts rather than rubs, even though the surface speed is not what the chart wanted.
When the machine and setup cap the numbers
The chart assumes a machine that can deliver. The real ceiling is the weakest link: spindle top RPM (which silently caps the cutting speed of small tools, above), low-speed torque and power (steel and titanium need torque at modest RPM, not just speed), the rigidity of the machine and holder, and the strength of the workholding. A long tool in a light holder on a thin-walled part will chatter at a fraction of the speed the same tool manages stub-held in a stout vise. Chatter is the signal you have hit a structural limit — and the fix is usually to change the engagement or the setup, not to keep lowering the speed. The parameters guide covers exactly how each operation and each weak link bends the recipe; the principle to carry out of here is that every number you compute is only as good as the stiffness behind it.
Reading the cut: chips are the report card
When you finally run the job, the cut tells you whether your arithmetic was right:
- Chips. Thick, curled, even chips mean the tool is cutting. Fine dust or powder means it is rubbing — and dust also means the heat is staying in the tool instead of leaving in the chips. Chips that are blue or burnt mean the cutting speed is too high (or the tool is dull).
- Sound. A steady cut has a rhythm. Chatter — a harsh, rattling tone — is a stiffness or engagement problem. A squeal is usually rubbing.
- Surface and tool wear. A rough or burned finish, and visible edge wear, both point back to which number was wrong.
Then change one variable at a time, cut again, and let the evidence decide. Too much heat → lower the cutting speed. Rubbing → raise the feed (or the chip load), not the speed. Chatter → lighten the engagement or shorten the tool before you touch RPM. The parameters guide’s tuning loop is the full version of this; the habit to start here is never changing two numbers at once, because then you cannot tell which one fixed it.
Six mistakes that will mislead you
- Looking up RPM instead of cutting speed. The material dictates the cutting speed; RPM is computed from it and the tool diameter. If the tool changes, the RPM changes even though the material did not.
- Dropping the feed “to be safe.” A feed too slow makes the tool rub, and rubbing generates heat and work-hardens stainless, titanium and nickel. Thin chips are not gentle — they are destructive.
- Forgetting that chips carry the heat. A tool making proper chips sheds heat with them; a tool making dust keeps the heat in itself. This is why “feed too low” overheats a tool faster than speed does.
- Using one set of numbers for every tool size. Same material, different diameter → different RPM (smaller tool spins faster), and usually a different chip load too.
- Trusting one chart. Charts disagree by up to a factor of two because they assume different tooling and machines. Use them for ordering and starting points; your toolmaker’s data for the specific tool is the better number.
- Ignoring the machine ceiling. If the spindle cannot reach the RPM the arithmetic wants, the machine has just lowered your effective cutting speed — recompute the feed for the RPM you can actually run, keeping the chip load honest.
Frequently asked questions
What is the difference between spindle speed and cutting speed? Cutting speed (SFM or m/min) is how fast the cutting edge moves through the material, and it is set by the material. Spindle speed (RPM) is how fast the tool rotates, and it is calculated from the cutting speed and the tool diameter. Smaller tools need higher RPM to reach the same cutting speed — that is the whole reason RPM changes when the tool does.
How do I calculate RPM and feed rate? RPM = cutting speed ÷ (π × tool diameter), with units consistent — imperial shortcut RPM = SFM × 3.82 ÷ inches, metric RPM = (m/min × 1000) ÷ (π × mm). Feed = RPM × feed per tooth × number of flutes. Feed per tooth (chip load) comes from the toolmaker for the tool diameter, not from a guess.
Why is feeding too slow bad for the tool? Because at a very low feed per tooth the chip thickness falls below what the edge needs to actually cut, and the tool rubs instead. Rubbing generates friction heat in the tool (not the chips) and work-hardens the material surface. The fix is a higher feed, not a lower one — with work-hardening alloys it is one of the most common causes of burnt edges.
What SFM should I use for aluminium vs steel? As rounded starting points for carbide end mills: aluminium 500–1,000 SFM, mild steel 200–400 SFM, stainless 100–200 SFM — aluminium runs several times faster because it conducts heat away in the chips. Your toolmaker’s data for the specific tool, and the chip-and-sound evidence from the actual cut, should refine those starting points.
Do feeds and speeds go in CAM or on the machine? In CAM — the tool, material and operation are defined there, and you can simulate the result. The machine runs what the program says. The skill is the same in either place: know which number is chosen (cutting speed, chip load), compute the rest, and tune one variable at a time until the chips tell you the cut is right.
Bottom line
Speeds and feeds are not a table of magic numbers — they are three different quantities and two pieces of arithmetic. The material chooses the cutting speed; the tool’s diameter converts it into a spindle RPM; the tool’s chip load and flutes convert it into a feed rate. Keep the chip thick enough to cut rather than rub, respect the machine’s spindle and rigidity as the real ceiling, start at the low end of any chart and let the chips and the sound tune the last 20%. Get those fundamentals straight and the same model carries you from a first aluminium slot to the hardest nickel alloy — the difficulty ladder, material by material, is the one the materials reference explains, and the operation-by-operation recipes are in the parameters guide.
This guide is part of the CNC Media guides library — the fundamentals page of the machining-parameters topic, deliberately free of prices and of any single supplier’s numbers to sell.