SFM Calculator and Speeds and Feeds Chart: RPM, IPM, and chip load formulas for CNC
Surface feet per minute (SFM) to RPM calculator, chip load to IPM, and starting SFM ranges by material for milling and turning. Complete formulas with worked examples — same math as ShopCalc, offline on your phone.
RPM = (SFM × 3.82) / tool diameter, and feed (IPM) = RPM × chip load × flutes. Example: a 1/2" 4-flute carbide end mill in 6061 aluminum at 800 SFM → (800 × 3.82) / 0.5 = 6,112 RPM, and at 0.002 ipt chip load → 6,112 × 0.002 × 4 = 48.9 IPM. That's the entire calculation - everything below is picking the right SFM and chip load for your material and tool.
Treat this page as a feeds and speeds calculator cheat sheet: SFM to RPM, chip load to IPM, MRR, and starter surface-speed ranges for common materials. The math matches what ShopCalc runs offline on your phone (mill, lathe, drilling, threading).
Speeds and feeds is the math that gets a tool through material without burning it up, breaking it, or producing a finish that looks chewed. The formulas are simple. The judgment isn't - but you have to start with the math.
The four numbers
- SFM - surface feet per minute (material × tool grade)
- RPM - spindle speed
- IPM - inches per minute (feed rate)
- MRR - material removal rate (cubic inches per minute)
The formulas
RPM = (SFM × 12) / (π × D) IPM = RPM × Z × Fz MRR = IPM × DOC × WOC D = tool diameter (inches) Z = number of flutes Fz = chip load per tooth (in/tooth) DOC = depth of cut (inches) WOC = width of cut (inches)
Carbide endmill SFM starting points
Material Carbide SFM 6061 aluminum 600–1200 (0.002–0.004 ipt for a 1/2" tool) Mild steel (A36) 300–500 4140 pre-hard 250–400 304 stainless 150–300 Titanium 6Al4V 100–200 Cast iron 250–450 Brass 360 300–600
HSS runs at roughly 1/4 to 1/3 of these carbide numbers. Small tools (1/8" and under) need chip load cut roughly in half - more on that below. Coatings (TiN, TiAlN, AlTiN) push the high end further if you have rigidity and coolant.
Chip load - the easy way
- Tool ≤ 1/8" - start at 0.001 in/tooth
- 1/8" – 1/4" - start at 0.002 in/tooth
- 1/4" – 1/2" - start at 0.003 in/tooth
- 1/2" – 3/4" - start at 0.004 in/tooth
- Above 3/4" - start at 0.005+ in/tooth
Small endmills (the 1/8" question)
Below about 1/4" the RPM formula outruns most spindles: a 1/8" carbide end mill in aluminum at 800 SFM wants (800 × 3.82) / 0.125 = 24,448 RPM. On a 10k or 15k spindle, just run max RPM and drop chip load to 0.0005–0.001 ipt. Deflection, not heat, is what kills small tools - keep depth of cut light and the feed honest instead of chasing surface speed you can't reach.
Worked example: 1/2" 3-flute end mill in aluminum
Material: 6061 → SFM ≈ 1000
Tool: 1/2" Ø, 3 flutes
Chip: 0.003 in/tooth
RPM = (1000 × 12) / (π × 0.5)
= 12000 / 1.5708
≈ 7,640 RPM
IPM = 7640 × 3 × 0.003
≈ 68.8 IPM
For DOC = 0.25, WOC = 0.5:
MRR = 68.8 × 0.25 × 0.5
= 8.6 in³/minStop pulling numbers from forum threads
These formulas are easy. The slow part is doing them by hand for every job - looking up SFM ranges, converting units, second-guessing chip load, recalculating when you change tool diameter. ShopCalc does the math instantly with material presets and chip-thinning built in. Free on iOS and Android, fully offline, no signup.
SFM calculator
Want the arithmetic done for you? The free SFM calculator takes diameter and RPM and returns surface speed instantly, with recommended HSS and carbide ranges per material. For conversions the other way, use the SFM to RPM calculator, and for feed rate the IPM calculator covers chip load × flutes × RPM. All three run in the browser; ShopCalc (free, offline, iOS and Android) has the full 30+ machinist calculator set.
Related
- 1/4" 4-flute carbide in 4140 prehard — full speeds/feeds example
- G-code: face a 2.5" bar on a CNC lathe (Fanuc/Haas)
- Tap drill chart: UNC, UNF, NPT, and metric sizes
- All four trade calculator apps (hub)
- ShopCalc — full feature list and screenshots
- Ace & Alan Tool — carbide and end mills
Note: Use as a starting point. Always validate with your machine, fixture, and tooling.
Frequently asked questions
How do you convert SFM to RPM?
RPM = (SFM x 12) / (pi x D), where D is the tool diameter in inches. The simplified version is RPM = (SFM x 3.82) / D. For example, a 1/2" carbide end mill in 6061 aluminum at 800 SFM gives (800 x 3.82) / 0.5 = 6,112 RPM.
How do you calculate feed rate (IPM) from RPM and chip load?
IPM = RPM x chip load per tooth x number of flutes. Using the 6,112 RPM example above with a 4-flute end mill at 0.002 in/tooth chip load: 6,112 x 0.002 x 4 = 48.9 IPM.
What SFM should I use for carbide end mills in aluminum?
600 to 1200 SFM for 6061 aluminum with carbide tooling. Start in the middle of the range and adjust based on finish and spindle sound. HSS runs at roughly 1/4 to 1/3 of these carbide numbers.
What is a safe starting chip load for a 1/4" end mill?
0.002 in/tooth is a reasonable starting chip load for a 1/4" end mill. The general guide: under 1/8" use 0.001 ipt, 1/8" to 1/4" use 0.002 ipt, 1/4" to 1/2" use 0.003 ipt, and 1/2" to 3/4" use 0.004 ipt.
What SFM should I use for carbide in 4140 or mild steel?
250 to 400 SFM for 4140 pre-hard, 300 to 500 SFM for mild steel (A36), with carbide tooling. Run 304 stainless at 150 to 300 SFM and titanium 6Al4V at 100 to 200 SFM.