โ Machinist Hub ยท Guides ยท Calculator
Feeds & Speeds Basics
Guide ยท Updated October 5, 2026
Feeds and speeds come down to two numbers: how fast the cutting edge moves across the material (surface speed), and how thick a chip each edge takes (chip load). Get those in range for your tool and material, then adjust for rigidity, stickout, and what the chips and finish tell you.
Step 1: Surface speed โ RPM
Inch: RPM = SFM ร 12 รท (ฯ ร D) โ SFM ร 3.82 รท D, with D = tool (or, for turning, work) diameter in inches.
Metric: RPM = Vc ร 1000 รท (ฯ ร D), with Vc in m/min and D in mm.
Step 2: Chip load โ feed rate
Inch: IPM = RPM ร chip load (in/tooth) ร number of flutes
Metric: feed (mm/min) = RPM ร fz (mm/tooth) ร z
Chip load comes from the tool maker's chart and depends on tool diameter, material, and engagement. Small tools take much smaller chips. As an illustration only, a 1/2" carbide end mill in aluminum often starts around 0.002โ0.004" per tooth, and less in steel. Too small a chip rubs and work-hardens; too large chips or breaks the tool.
Worked example (inch)
1/2" 3-flute carbide end mill in 6061 aluminum, using a starting point of 800 SFM and 0.003"/tooth:
- RPM = 800 ร 3.82 รท 0.5 = 6,112 RPM
- IPM = 6,112 ร 0.003 ร 3 = 55 IPM
- If your spindle tops out at 4,000 RPM, keep the chip load and recalculate: 4,000 ร 0.003 ร 3 = 36 IPM. Don't keep 55 IPM at the lower RPM; that's a much heavier chip.
Worked example (metric)
12 mm 3-flute carbide end mill, Vc = 250 m/min, fz = 0.08 mm/tooth:
- RPM = 250 ร 1000 รท (ฯ ร 12) โ 6,630 RPM
- Feed = 6,630 ร 0.08 ร 3 โ 1,590 mm/min
Conservative starting surface speeds (milling)
| Material | HSS (SFM) | Uncoated carbide (SFM) |
|---|---|---|
| Aluminum (e.g., 6061-T6) | 250โ600 | 800โ1,500 (often RPM-limited) |
| Brass (free-machining) | 150โ300 | 400โ800 |
| Low-carbon steel (e.g., 1018) | 80โ120 | 350โ600 |
| Alloy steel, annealed (e.g., 4140) | 50โ80 | 250โ450 |
| Gray cast iron | 50โ80 | 250โ400 |
| Stainless (e.g., 304) | 40โ60 | 200โ350 |
Broad starting ranges, not recommendations for a specific tool. Coated carbide, toolpath strategy, and coolant can push these higher; hardened material, long stickout, or a light machine call for lower. Your tool maker's data and Machinery's Handbook come first.
Radial engagement and chip thinning
When the tool engages less than half its diameter radially (light finishing passes, high-efficiency toolpaths), the actual chip is thinner than the programmed chip load. Tool makers publish chip-thinning factors that let you raise the feed so the edge still cuts instead of rubbing. At full-width slotting, use the maker's slotting numbers, which are usually lower.
Drilling and turning
- Drilling: RPM uses the drill diameter in the same formula. Feed is given per revolution (IPR or mm/rev) from the drill maker's chart and scales with diameter. Peck or use through-coolant when chips pack.
- Turning: RPM uses the work diameter, so it changes as the part gets smaller. Feed is per revolution. Constant-surface-speed (CSS) on a CNC lathe handles the RPM change; set a max-RPM clamp for safety.
Read the cut
- Chatter: shorten stickout, check workholding, try a different RPM, and avoid timid feeds that rub.
- Built-up edge / galling in aluminum: improve chip evacuation and lubrication, and use sharp, polished tools.
- Rubbing / squealing / work-hardening (stainless): the chip load is usually too light. Keep the tool engaged and don't dwell.
- Rapid edge wear: the surface speed is likely too high for the material or coating.
Safety
Safety glasses always. No gloves, loose sleeves, or jewelry near rotating tools or chucks. Never leave a chuck key in the chuck. Clear chips with a brush or hook with the spindle stopped. Clamp work securely. Running feeds and speeds is about the cut, but a loose part or a grabbed sleeve is how people get hurt.
Shop references and tools
- Machinery's Handbook: the standard reference for speeds, feeds, threads and fits.
- Carbide end mill sets
- Cutting & tapping fluid
- ANSI Z87.1 safety glasses
Need a stack for a specific size?
The Gage Block Calculator finds the fewest-block combination for inch and metric sets, with optional wear blocks. Free, no account.
Questions? Ask the AI Machinist.
General shop information only โ follow your gage manufacturer's instructions and your quality system. As an Amazon Associate I earn from qualifying purchases; links marked "sponsored" may earn a commission at no cost to you.