How to use this calculator
- Enter the diameter. Enter the tool diameter (milling/drilling) or work diameter (turning).
- Look up the cutting speed. Find a starting cutting speed for your material in the table, then enter it.
- Read the RPM. Read the spindle speed. Tune for depth of cut, feed, coating and rigidity.
How it works
Spindle speed comes from the cutting speed and the diameter:
RPM = cutting speed ÷ (π × diameter)
In imperial that works out to RPM = 12 × SFM ÷ (π × D) ≈ 3.82 × SFM / D
with D in inches; in metric, RPM = 1000 × Vc ÷ (π × D) with Vc in m/min
and D in mm. Use the tool diameter for milling and drilling, and the work diameter
for turning. The cutting speed itself depends on the material and tool — start from
the cutting speed chart below and adjust. If
you already know RPM and want the actual surface speed, use the
cutting speed calculator; when you also
need chip load and feed rate, use the CNC
speeds and feeds calculator.
Worked example
Verified against the live calculator
A 1-inch end mill running 100 SFM in mild steel:
RPM = 12 × 100 ÷ (π × 1) ≈ 382 RPM. The same in metric — a 25.4 mm tool
at 30.5 m/min — gives the same 382 RPM. The calculator returns this on load.
Reference data
Starting cutting speeds for single-point turning, in surface feet per minute, for HSS and uncoated carbide. Real speeds depend on depth of cut, feed, coating, coolant and rigidity — treat these as a baseline.
| Material | HSS (SFM) | Carbide (SFM) | Notes |
|---|---|---|---|
| Aluminum | 300 | 800 | Free-machining; high speeds, watch built-up edge. |
| Brass | 200 | 600 | Free-cutting brass; very machinable. |
| Bronze | 120 | 350 | Harder than brass. |
| Cast iron (gray) | 60 | 200 | Abrasive; carbide preferred. |
| Mild steel (1018) | 90 | 350 | General low-carbon steel. |
| Alloy steel (4140) | 60 | 250 | Heat-treatable; lower when hardened. |
| Stainless (304) | 50 | 200 | Work-hardens; keep feed up, avoid dwelling. |
| Tool steel | 45 | 175 | Hard; reduce speed as hardness rises. |
| Titanium | 35 | 150 | Low speed; heat builds fast. |
| Plastic | 400 | 800 | Sharp tools; clear chips. |
| Aluminum (cast A356) | 250 | 700 | Silicon content is abrasive; use flood coolant. |
| Magnesium | 400 | 900 | Excellent machinability; fine chips are a fire risk, never use water-based coolant. |
| Copper | 150 | 400 | Gummy; sharp tools and positive rake reduce built-up edge. |
| Free-machining steel (12L14) | 130 | 450 | Leaded/resulfurized; best machinability of the steels. |
| Medium-carbon steel (1045) | 70 | 300 | Tougher than 1018; common shaft steel. |
| Alloy steel (4340) | 50 | 220 | High-strength; reduce speed in the heat-treated condition. |
| Hardened steel (45-55 HRC) | 20 | 100 | Hard turning; carbide or CBN only, light finishing cuts (HSS not suitable). |
| Stainless (303) | 70 | 250 | Free-machining austenitic; the easiest stainless. |
| Stainless (316) | 45 | 180 | Gummier than 304 and work-hardens; keep cuts positive. |
| Stainless (416) | 90 | 280 | Free-machining martensitic stainless. |
| Stainless (17-4 PH) | 40 | 150 | Precipitation-hardening; speed depends on condition (H900 lower). |
| Stainless (410) | 60 | 220 | Martensitic; machine in the annealed condition where possible. |
| Ductile iron (65-45-12) | 50 | 180 | Nodular iron; tougher and less abrasive than gray. |
| Malleable iron | 80 | 250 | Machines more like steel than gray iron. |
| Inconel / nickel superalloy | 15 | 60 | Very tough and work-hardens; low speed, positive rake, rigid setup. |
| Monel (Ni-Cu) | 40 | 120 | Work-hardens; keep the feed up and never dwell. |
| Hastelloy | 15 | 60 | Nickel superalloy; treat like Inconel. |
| Fiberglass / GFRP | 150 | 500 | Abrasive; carbide or diamond tooling and dust extraction. |
Source: Standard machining references (Machinery's Handbook turning-speed tables; common shop practice). Verify against your tooling maker's data.
Frequently asked questions
How do you convert SFM to RPM?
RPM = (SFM × 12) ÷ (π × diameter in inches), which is about 3.82 × SFM ÷ D. In metric, RPM = (1000 × Vc) ÷ (π × diameter in mm), with Vc in m/min.
What is surface feet per minute (SFM)?
SFM is the cutting speed — how fast the cutting edge moves across the workpiece surface, in feet per minute. The metric equivalent is surface metres per minute (m/min).
What SFM should I use for aluminum, steel or stainless?
Use the cutting-speed table below as a starting point: roughly 800 SFM for aluminum, 350 for mild steel and 200 for stainless with carbide; about a third of that with HSS. Then tune for your setup.
Is the diameter the tool or the workpiece?
For milling and drilling, use the tool diameter. For turning, use the workpiece diameter at the cut.
How much faster is carbide than HSS?
Carbide typically runs two to four times the cutting speed of high-speed steel for the same material, because it keeps its hardness at much higher temperatures.
Does it work in metric (m/min)?
Yes — toggle SI/Imperial to switch the cutting speed between SFM and m/min and the diameter between inches and mm.
Method & assumptions
- Cutting speeds are general turning starting points; milling and drilling, coatings and high-feed strategies shift them.
- This finds spindle speed from cutting speed — to go the other way, RPM × π × D gives the surface speed.