Cutting Speed & Feed Rate Calculator

Calculate spindle RPM, feed rate (IPM), chip load, and MRR for any CNC milling operation. SFM auto-fills from material — covers 13 materials.

Free Tool · Instant Results
Tool & Cut Inputs
▤
⚙

Coated carbide adds ~10–15% SFM. HSS runs ~30–35% of carbide values.

SFM
Auto-fills from material selection. Adjust within the range shown.
Ø inches

0.25 = 1/4″  ·  0.5 = 1/2″  ·  1.0 = 1″

#

2–3 flutes for aluminum; 4+ flutes for steel and harder materials

IPT in/tooth
Auto-fills from material + diameter. Stay within range.
⚑
↕ inches
↔ inches

Slotting: WOC = tool diameter  ·  Profiling: 25–50% of diameter

Results

Select material & tool,
then hit Calculate

✓
Spindle Speed
—
RPM
Feed Rate
—
IPM (inches per min)
Confirmed SFM
—
surface feet / min
Chip Load / Tooth
—
inches per tooth
Material Removal Rate (MRR) —
Calculated Output
Spindle Speed—
Feed Rate—
Confirmed SFM—
Chip Load / Tooth—
Cut Efficiency
Material Removal Rate—
DOC × WOC—
Tool Geometry
Tool circumference—
Feed per revolution—

SFM & Chip Load Reference — Carbide End Mills

Starting-point values for solid carbide end mills with flood coolant. Coated carbide (TiAlN/AlTiN): add 10–15%. HSS: use 30–35% of these values. Always verify against your tool manufacturer’s catalog before production runs.

MaterialSFM (Carbide)Chip Load 1/4″Chip Load 1/2″Chip Load 1″Key Notes
Aluminum 6061 / 7075Easy600–1,5000.003–0.005″0.005–0.008″0.008–0.012″2–3 flutes; flood coolant prevents chip welding (BUE)
Aluminum — CastEasy400–9000.002–0.004″0.004–0.007″0.007–0.010″Silicon is abrasive; ZrN or DLC coating preferred
Mild Steel 1018 / A36Medium250–5000.001–0.003″0.002–0.005″0.004–0.007″Baseline material; 4 flutes; TiAlN coating recommended
Alloy Steel 4140 / 4340Medium200–4000.001–0.002″0.002–0.004″0.003–0.006″Reduce 20% for prehardened (+30 HRC); AlTiN coating
Tool Steel D2 / H13Hard100–2500.001–0.0015″0.0015–0.003″0.002–0.004″Over 50 HRC: ceramic or CBN tooling required
Stainless 304 / 316Hard150–3500.001–0.002″0.002–0.004″0.003–0.005″Work-hardens — never rub. Keep IPT > 0.001″. Flood coolant mandatory
Stainless 17-4PHHard100–2500.0008–0.0015″0.001–0.003″0.002–0.004″Precipitation-hardened; AlTiN / nACRo3 coatings required
Brass / BronzeEasy400–9000.003–0.005″0.004–0.007″0.006–0.010″Free-machining; uncoated carbide fine; watch chip gumming in bronze
CopperMedium300–6000.002–0.004″0.003–0.006″0.005–0.008″Gummy — sharp polished flutes; flood coolant
Titanium Ti-6Al-4VHard80–2000.0005–0.001″0.001–0.003″0.002–0.004″Low thermal conductivity — heat at tool tip. Strict SFM limits
Inconel / HastelloyHard30–800.0003–0.0008″0.0008–0.0015″0.001–0.003″Highest forces; nACRo3 / AlTiN essential; high-pressure coolant
Cast Iron (Gray)Medium200–4000.002–0.004″0.003–0.006″0.005–0.009″Dry cutting acceptable; abrasive — TiAlN coated tools
Plastics (Delrin / Nylon)Easy500–1,5000.004–0.007″0.006–0.012″0.010–0.018″O-flute or 2-flute; no coolant or light mist
Aluminum 6061/7075Easy
600–1,500 SFM
Chip Load 1/4″0.003–0.005″
Chip Load 1/2″0.005–0.008″
Chip Load 1″0.008–0.012″
2–3 flutes; flood coolant prevents chip welding (BUE)
Mild Steel 1018/A36Medium
250–500 SFM
Chip Load 1/4″0.001–0.003″
Chip Load 1/2″0.002–0.005″
Chip Load 1″0.004–0.007″
Baseline material; 4 flutes; TiAlN coating recommended
Stainless 304 / 316Hard
150–350 SFM
Chip Load 1/4″0.001–0.002″
Chip Load 1/2″0.002–0.004″
Chip Load 1″0.003–0.005″
Work-hardens rapidly — never rub. Keep IPT > 0.001″. Flood coolant mandatory.
Titanium Ti-6Al-4VHard
80–200 SFM
Chip Load 1/4″0.0005–0.001″
Chip Load 1/2″0.001–0.003″
Chip Load 1″0.002–0.004″
Low thermal conductivity — heat concentrates at tool tip. Strict SFM limits required.
Brass / BronzeEasy
400–900 SFM
Chip Load 1/4″0.003–0.005″
Chip Load 1/2″0.004–0.007″
Chip Load 1″0.006–0.010″
Free-machining; uncoated carbide acceptable; watch for chip gumming in bronze
Inconel / HastelloyHard
30–80 SFM
Chip Load 1/4″0.0003–0.0008″
Chip Load 1/2″0.0008–0.0015″
Chip Load 1″0.001–0.003″
Highest cutting forces. nACRo3 or AlTiN coatings essential; high-pressure coolant required.

How CNC Spindle Speed & Feed Rate Are Calculated

Speeds and feeds are the two most fundamental CNC machining parameters. Getting them wrong is the #1 cause of broken tools, poor surface finish, and scrapped parts in U.S. job shops. The formulas are simple — the challenge is knowing the right SFM and chip load for your material/tool combination.

1 SFM to RPM

SFM is a material constant. Since larger tools cover more distance per revolution, RPM must decrease as diameter increases to maintain the same SFM. 3.82 is simply 12 ÷ π.

RPM = (SFM × 3.82)
÷ Tool Diameter (in)

2 RPM to Feed Rate

Each flute removes one chip per revolution. More flutes = more chips per rev = higher possible feed rate at the same chip load per tooth.

Feed (IPM) =
RPM × Flutes
× Chip Load (IPT)

3 Chip Load (IPT)

The thickness each tooth removes per revolution. Too low: rubbing and heat. Too high: breakage. Most critical in stainless and titanium where rubbing causes rapid work hardening.

IPT = Feed (IPM)
÷ (RPM × Flutes)

4 MRR

Material Removal Rate measures machining efficiency. Higher MRR = faster cycle times = lower cost per part. Key metric for comparing toolpath strategies.

MRR (in³/min) =
Feed × WOC × DOC

Pro Tip — The Cardinal Rule of Chip Load Too light a chip load is worse than too heavy. When chip load is too small, the tool rubs instead of cuts — generating heat, work-hardening the surface (critical in stainless and titanium), causing built-up edge (BUE). If your tool is burning up quickly, try increasing your feed rate before reducing it.

Frequently Asked Questions

SFM (Surface Feet per Minute) is the actual speed of the cutting edge across the workpiece surface. You choose SFM based on what you’re cutting, then calculate RPM from it using your tool diameter. The key insight: SFM stays constant for a given material, but RPM changes with tool size. A 1/4″ end mill in 6061 aluminum requires ~12,200 RPM to hit 800 SFM; a 1″ end mill needs only ~3,056 RPM for the same surface speed.
For aluminum and soft non-ferrous materials, use 2–3 flutes. The large flute valleys provide excellent chip evacuation, preventing aluminum chips from re-cutting and welding to the tool (BUE). For steel, stainless, and harder materials, use 4–6 flutes. Extra cutting edges distribute heat and forces, extending tool life. Never use a 4-flute end mill in aluminum for slotting — poor chip clearance causes rapid tool failure.
Chip thinning occurs when radial width of cut is less than 50% of tool diameter. At reduced engagement, each tooth removes a thinner chip than programmed — meaning the tool is working less than intended. To compensate, increase your feed rate. The thinning factor ≈ 1 ÷ √(WOC ÷ Diameter). At 25% stepover the factor is ~1.41, so you can increase feed by ~41% while maintaining the same actual chip thickness. Trochoidal and adaptive milling rely on this principle.
304 and 316 stainless work-harden — repeated plastic deformation can increase surface hardness by over 30%, making every subsequent pass harder on the tool. Critical rules: never let the tool rub (keep chip load above 0.001″ IPT), use flood coolant at high pressure, and stay within 150–350 SFM for carbide. When in doubt, increase the feed rate rather than decrease it.
Carbide maintains hardness at much higher temperatures, allowing 3–4× the SFM of HSS. For 1018 mild steel: carbide runs 300–500 SFM vs 80–130 SFM for HSS — dramatically shorter cycle times. However, carbide is brittle and needs a rigid machine and solid workholding. HSS is more forgiving in worn or unstable setups. For modern CNC machining centers, solid carbide is almost always the correct choice for production work.

Calculated values are starting points only. Actual parameters depend on machine rigidity, workholding, tool condition, and coolant. Start at 50–70% and increase incrementally. Always verify against your tool manufacturer’s data sheet. © TWC Industrial

Updated 2026 · Free to Use
Scroll to Top