Pick the SFM for the material
Start with the material's surface-speed range from the table or the tool manufacturer's data. Harder and gummier materials run slower; aluminum runs fast.
RPM FORMULA • FEED RATE • WORKED EXAMPLES
CARBIDE SPEEDSAND FEEDS BASICS
Three formulas run every carbide cut: RPM from surface speed, feed rate from chip load, and the material removal rate that ties them together. Learn them once, use them forever.
RPM FormulaChip LoadFeed RateBy Material
THE THREE FORMULAS
The math every machinist carries
Speeds and feeds look intimidating until you see that the whole system is three formulas. Everything else is choosing the inputs.
Formula 1: RPM from surface speed
RPM = SFM × 3.82 ÷ tool diameter (inches). SFM — surface feet per minute — is how fast the cutting edge moves through the material, and it is set by the material and the tool. The 3.82 is the unit-conversion constant (12 ÷ π). Example: 400 SFM with a 1/2-inch end mill gives 400 × 3.82 ÷ 0.5 = 3,056 RPM.
Formula 2: Feed rate from chip load
Feed (IPM) = RPM × chip load per tooth × number of flutes. Chip load — inches per tooth — is how much material each cutting edge bites off per revolution, set by the tool size and material. Example: 3,056 RPM × 0.003 inches per tooth × 4 flutes = 36.7 inches per minute.
Formula 3: Material removal rate
MRR = width of cut × depth of cut × feed rate. This is the productivity number: cubic inches per minute leaving the part. It ties speed, feed, and engagement together, and it is the number that actually measures whether a cut is aggressive or timid.
The golden rule: carbide must cut, not rub. Too little chip load and the edge rubs — generating heat, work-hardening the material, and killing the tool faster than pushing too hard. When in doubt, most beginners feed too timidly, not too aggressively.
BY MATERIAL
Starting numbers that work
These are conservative starting ranges for solid carbide end mills. Your tool manufacturer's data always wins over any chart — use these to sanity-check, not to replace it.
| Material | Starting SFM | Chip load per tooth (1/2-in tool) | Notes |
|---|---|---|---|
| Aluminum | 600–1,000+ | 0.003–0.006 in | Run fast; 2–3 flutes; watch chip evacuation |
| Low-carbon steel | 350–550 | 0.002–0.004 in | The baseline most charts are built on |
| Alloy steel | 250–400 | 0.002–0.003 in | Back off as hardness climbs |
| Stainless steel | 200–350 | 0.002–0.003 in | Never let it rub — stainless work-hardens |
| Cast iron | 250–450 | 0.002–0.004 in | Abrasive; dry or with air blast often beats flood |
| Titanium | 100–200 | 0.001–0.002 in | Slow, rigid, and plenty of coolant |
Worked example: 1/2-inch 4-flute in 1018 steel
Pick 400 SFM. RPM = 400 × 3.82 ÷ 0.5 = 3,056 RPM. Pick 0.003 in chip load. Feed = 3,056 × 0.003 × 4 = 36.7 IPM. That is a sane starting cut — then adjust by watching the chips, the sound, and the finish. Blue or straw-colored steel chips mean the heat is about right; dark blue to purple means back off.
Worked example: 1/4-inch 2-flute in aluminum
Pick 800 SFM. RPM = 800 × 3.82 ÷ 0.25 = 12,224 RPM. Pick 0.004 in chip load. Feed = 12,224 × 0.004 × 2 = 97.8 IPM. Aluminum wants speed — if your spindle cannot reach it, take the max RPM you have and set the feed from the real RPM.
THE NUMBER SEQUENCE
Setting a cut in three steps.
Calculate the RPM
RPM = SFM × 3.82 ÷ tool diameter in inches. Set the spindle to the calculated RPM, or the closest your machine reaches.
Pick the chip load and calculate feed
Choose inches per tooth for the tool size and material, then feed = RPM × chip load × flutes. Verify the machine can feed that fast before running.
Prove it with the cut
Run the cut and read the evidence: chip color and shape, sound, finish, and spindle load. Adjust speed and feed in small steps until the cut is stable, the chips look right, and the tool is happy.
READING THE CUT
What the chips and the sound tell you
The formulas get you close. The cut itself gets you right.
Chips: in steel, short curled chips with a straw-to-blue temper color mean the heat is in the chip where it belongs. Long stringy chips mean the feed is too light or the chipbreaker is wrong. Dust-like chips mean the tool is rubbing — increase the chip load.
Sound: a steady cutting hum is right. Chatter — the high-pitched squeal — means vibration: reduce stick-out, stiffen the setup, or adjust speed to break the harmonic. A sudden change in sound mid-cut means something changed: check the tool.
Heat: in carbide milling, most heat should leave with the chip. If the part is getting hot and the chips are cool, the cut is wrong — usually too little feed. Hot chips and a cool part is the signature of a correct carbide cut.
COMMON QUESTIONS
Asked by shops working with this every day.
What is SFM?
Surface feet per minute: how fast the cutting edge travels through the material. It is the speed number that belongs to the material and the tool — RPM is just SFM translated for a specific tool diameter.
What is chip load?
Inches per tooth: the thickness of material each cutting edge removes per revolution. Too little and the tool rubs; too much and it overloads. It scales with tool diameter — bigger tools take bigger bites.
Why do my tools keep breaking at the calculated feeds?
The math assumes a rigid setup. Excessive stick-out, weak workholding, or a worn spindle turns correct numbers into broken tools. Fix the rigidity before blaming the formula — and check runout, which multiplies the load on one flute.
Should I use coolant with carbide?
Usually yes for steel and stainless — it controls heat and clears chips. Some operations (cast iron, certain high-heat cuts with the right coatings) run dry or with air blast. Match the coolant strategy to the material, not to habit.
How do speeds change for coated vs uncoated tools?
Coatings like TiAlN tolerate more heat, so coated tools can often run 20–50% higher SFM than uncoated in the same material. The coating manufacturer's data gives the real multiplier.
Do wrong feeds really kill tools that fast?
Yes — wrong feeds kill tools fast, and every dead tool is still worth money. Run them right, sell them when they are done. There are no minimums: every bucket counts. Call 312-880-8174.
WHEN THE TOOL IS DONE
When the Tool Is Done
Wrong feeds kill tools fast — and every dead tool is still worth money. Run them right, sell them when they are done. Whether it is a handful of snapped end mills from a bad program or a drum of worn production tooling, there are no minimums: every bucket counts. On bigger lots, we handle the freight so you do not lift a finger. Call 312-880-8174.