What this calculator does
Find how fast to spin your cutter and how fast to feed it into the metal. Every cutting tool has a speed at which its edge likes to meet the metal. Machinists call it the cutting speed or surface speed. It's given in surface feet per minute (SFM) or meters per minute.
A small drill has to spin much faster than a big face mill to move its edge past the work at the same speed. That's why the spindle setting depends on both the material and the tool's diameter.
This speeds and feeds calculator turns a surface speed into spindle rpm (turns per minute). Then it multiplies three things to get the feed rate, how fast the table moves. Those are the chip load (how thick a bite each tooth takes), the number of teeth and the rpm. Pick a workpiece material to get a starting speed for a high-speed steel tool. You can also switch to carbide, or type in the figure from your tooling chart. The numbers are starting points to adjust from, not limits.
Where it's used
Why this math matters outside the classroom:
- Milling aluminum. A machinist runs a 1/2 in end mill at 250 SFM, which works out to 12 × 250 ÷ (π × 0.5), about 1,910 rpm.
- Drilling cast iron. A shop student drills soft cast iron at 100 SFM with a 1/4 in bit, so the drill press is set near 1,528 rpm.
- CNC programming. A programmer sets the feed for a 4-flute cutter at 0.004 in per tooth and 1,910 rpm to 30.56 in/min.
- Metric job shops. An operator runs a 10 mm cutter at 100 m/min, which is 1,000 × 100 ÷ (π × 10), about 3,183 rpm.
- Lathe turning. A turner facing a 2 in bar of mild steel at 100 SFM sets the lathe near 191 rpm.
Grade level and standards: Grades 6–7; Common Core State Standards for Mathematics 7.G.B.4, 6.RP.A.3.d. © Copyright 2010. National Governors Association Center for Best Practices and Council of Chief State School Officers. All rights reserved.
How to use it
- Choose inch or metric units.
- Pick the workpiece material and tool material, or choose to enter your own cutting speed.
- Enter the tool diameter, the number of teeth or flutes (cutting edges), and the chip load per tooth.
- Read the spindle rpm and feed rate. Start at or below them, then adjust by sound, chip color and finish.
What the inputs mean
- Workpiece material
- The listed speeds are general starting values for high-speed steel tools. A university machining lab handout boils them down from handbook guidance. Tool makers publish their own figures for each cutter and coating, so use theirs when you have them.
- Tool material
- Carbide tools handle far more heat than high-speed steel. The same handout multiplies its speeds by 2.5 for carbide, which is a rough rule. Coated carbide can often go faster, and small or long tools slower.
- Cutting speed
- Surface feet per minute from your tool maker's chart.
- Tool diameter (or workpiece diameter when turning)
- For milling and drilling, this is the cutter's diameter. For turning on a lathe, use the diameter of the workpiece where the tool is cutting. That's the surface moving past the edge.
- Number of teeth (flutes)
- A two-flute drill counts as 2. For a lathe, use 1 and enter the feed per turn as the chip load.
- Chip load (feed per tooth)
- Chip load is the thickness of material each tooth removes per turn. Typical milling values for high-speed steel run from about 0.001 in for hard steels to around 0.012 in for aluminum. Those are for cutters 1/2 in and larger; small cutters need less.
Formula and method
rpm = 12 × SFM ÷ (π × D) (D in inches) rpm = 1,000 × V ÷ (π × D) (V in m/min, D in mm) feed rate = rpm × number of teeth × chip load feed per revolution = number of teeth × chip load 1 SFM = 0.3048 m/min
In the formulas, SFM and V are the cutting speed, and D is the tool's diameter. π (pi) is about 3.1416. One turn of a tool moves its edge the distance around it, which is π × D. Dividing the cutting speed by that distance gives the turns per minute. The 12 turns feet into inches, and the 1,000 turns meters into millimeters.
Each tooth removes one chip per turn, so the tool moves forward by teeth × chip load every turn. Multiply by the turns per minute to get the feed in inches or millimeters per minute.
Worked example
A 1/2 in four-flute high-speed steel end mill cuts aluminum at a chip load of 0.004 in per tooth.
- Starting speed for aluminum with a high-speed steel tool: 250 SFM.
- Spindle speed: 12 × 250 ÷ (π × 0.5) = 1,909.86 rpm.
- Feed rate: 1,909.86 × 4 × 0.004 = 30.56 in/min.
Result: Start at about 1,910 rpm and a feed of about 30.56 in/min, then adjust for the machine and the cut.
Understanding the result
If the machine can't reach the calculated rpm, run it at its top speed. Then lower the feed rate by the same percentage the speed dropped, so each tooth still takes the same size bite.
Too little chip load makes a tool rub instead of cut. That dulls it, and it work-hardens (toughens the surface of) some stainless steels. Too much chip load overloads the edges and can snap small cutters. Too much speed shows up as heat: blue chips on steel, smoke, or a burned edge.
Assumptions and limitations
- Material speeds are general starting values for high-speed steel. They assume flood coolant (a steady stream of cutting fluid) and a rigid setup. Carbide is estimated as 2.5 times those.
- The full tool diameter is cutting. A ball end mill or a shallow cut may only touch with a smaller part of the tool. Then the edge moves slower than this assumes.
- It doesn't adjust for several things that change the best values. Those are radial chip thinning (thinner chips in a light side cut), depth of cut, tool stick-out, coatings, coolant and how rigid the machine is.
- Oil put on by hand, deep holes and flimsy setups call for lower speeds and feeds. A common shop habit is to start well below the calculated values and work up.
- The tool or insert maker's advice for the exact cutter always comes first, ahead of these general figures.
Frequently asked questions
How do I convert SFM to rpm?
Multiply the SFM by 12, then divide by π times the diameter in inches. A 1/4 in drill at 100 SFM runs 12 × 100 ÷ (π × 0.25), about 1,528 rpm. The shortcut rpm ≈ 3.82 × SFM ÷ D gives nearly the same number, because 12 ÷ π is about 3.82.
What is chip load?
Chip load, or feed per tooth, is how far the tool moves forward for each cutting edge that passes. It sets the thickness of each chip, and that controls heat, finish and the strain on the tool. It's usually a few thousandths of an inch or a few hundredths of a millimeter.
Why is a lathe speed based on the workpiece diameter?
On a lathe, the work spins and the tool stays put. So the surface speed past the edge is set by the diameter of the part being cut. As you turn a bar down, the same rpm gives a lower surface speed. That's why some lathes offer constant surface speed control.
Can I use these speeds for carbide inserts?
Only as a rough start. This calculator multiplies the high-speed steel figure by 2.5 for carbide. But insert grades and coatings vary widely, so use the insert maker's chart whenever you can.
Sources
- University of Florida, EML2322L Drilling and Milling Speeds and Feeds (Tables 1 and 3) (checked 2026-10-19)
How this calculator is checked
Method: Cutting speed V = π·D·N, solved for N (rpm = 12·SFM/(π·D) inch, 1000·V/(π·D) metric); feed = N × teeth × chip load. Starting speeds from Table 1 of the University of Florida EML2322L handout, with its 2.5× carbide factor. The calculation is covered by automated tests with known reference values and edge cases. Last updated 2026-10-18. Found a problem? Tell us.
Embed this calculator
Put this Speeds and Feeds Calculator on your own website or blog for free. Paste this code where you want it to appear: