Last updated: November 2026
Quick answer: A CNC feed and speed calculator turns four numbers (tool diameter, number of flutes, cutting speed and chip load) into two machine settings: spindle speed (RPM) and feed rate. The core formulas are RPM = (Vc × 1000) ÷ (π × D) in metric and Feed = RPM × chip load × flutes. Cutting speed and chip load must come from your tool maker's data sheet, because they depend on your tool and your material.
This guide is for machinists, CNC router and mill operators, hobbyists and students. It explains the cutting speed formula, the feed rate formula, how SFM to RPM conversion works, and how to use the CNC Feed & Speed Calculator as a fast RPM calculator for milling, drilling and lathe work. Every formula is shown in metric and imperial, with worked examples and tables.
Important: All results are theoretical estimates. They do not replace your tool maker's data, your machine manual or your workshop's safety procedures. Start conservatively and test on scrap where possible.
Estimates only. This calculator gives theoretical estimates based on standard, simplified formulas and the values you enter. It is for general information only and is not engineering, manufacturing, safety or professional advice.
Not accounted for. Machine rigidity, tool deflection or runout, tool wear, workholding, material condition, coolant, spindle power and torque, chatter, tool geometry and coating, and any other real-world condition. Actual results will differ.
Your responsibility. You are solely responsible for checking all values against your tool maker's data, your machine manual and your workshop procedures before running any program. Start conservatively, test on scrap where possible, and follow all safety rules, including guarding and protective equipment. Never exceed the limits of your tool, machine or workholding.
No warranty. This tool and its results are provided "as is" and "as available", without warranty of any kind, express or implied, including accuracy, completeness, reliability or fitness for a particular purpose.
Limitation of liability. To the fullest extent permitted by law, the owner, author and publisher of this tool accept no liability for any injury, death, damage to tools, machines, workpieces or property, loss of production, loss of profit, or any other direct or indirect loss arising from the use of, or reliance on, this tool or its results. Nothing here excludes or limits any liability that cannot be excluded or limited under applicable law.
Use at your own risk. By using this tool you confirm that you have read and accept this disclaimer. The tool and this disclaimer may be changed at any time without notice.
Related Tools
Table of Contents
What "feeds and speeds" means
Milling speeds and feeds are the two basic settings of any rotating cutting tool:
- Speed is how fast the tool (or the workpiece, on a lathe) rotates, measured in RPM.
- Feed is how fast the tool moves through the material, measured in mm/min (metric) or in/min (imperial).
The two are linked by cutting speed (how fast the tool's outer edge moves, in m/min or SFM) and chip load (how much material each cutting edge removes per revolution). The trade publication Cutting Tool Engineering describes cutting speed in surface feet per minute as the linear distance the edge travels each minute, and notes that toolmakers publish recommended cutting speeds for different workpiece materials (Cutting Tool Engineering: Understanding Cutting Equations for Feeds and Speeds).
In practice, you read the recommended cutting speed and chip load from your tool maker's data, then use the formulas below to turn them into RPM and feed rate for your specific tool diameter. That is exactly what the calculator automates.
Key terms
| Term | Symbol | Metric unit | Imperial unit | Meaning |
|---|---|---|---|---|
| Tool diameter | D | mm | in | Cutter diameter (part diameter on a lathe) |
| Number of flutes | Z | none | none | Number of cutting edges |
| Cutting speed (surface speed) | Vc | m/min | SFM | Speed of the tool's outer edge |
| Chip load (feed per tooth) | fz | mm/tooth | in/tooth | Material removed per cutting edge per revolution |
| Spindle speed | RPM | rev/min | rev/min | Rotations per minute |
| Feed rate | Vf | mm/min | in/min | Travel speed of the tool through the cut |
| Feed per revolution | fn | mm/rev | in/rev | Distance the tool advances each revolution |
| Radial width of cut | ae | mm | in | How wide the cut is sideways |
| Axial depth of cut | ap | mm | in | How deep the cut is along the tool axis |
The formulas
The calculator uses the standard formulas below and displays each one with your own numbers filled in, so you can check the arithmetic.
| What you want | Metric formula | Imperial formula |
|---|---|---|
| Spindle speed (RPM) | RPM = (Vc × 1000) ÷ (π × D) | RPM = (SFM × 12) ÷ (π × D) |
| Cutting speed from RPM | Vc = (π × D × RPM) ÷ 1000 | SFM = (π × D × RPM) ÷ 12 |
| Feed rate | Vf = RPM × fz × Z | Vf = RPM × fz × Z |
| Feed per revolution | fn = Vf ÷ RPM | fn = Vf ÷ RPM |
| Material removal rate | MRR = (ae × ap × Vf) ÷ 1000 (cm³/min) | MRR = ae × ap × Vf (in³/min) |
| Cutting time (one pass) | T = L ÷ Vf | T = L ÷ Vf |
Why does the cutting speed formula use 1000 and 12?
Diameter is entered in millimetres but cutting speed is in metres per minute, so the metric formula multiplies by 1000. In imperial, diameter is in inches but surface speed is in feet per minute, so the formula multiplies by 12. The well-known shop shortcut RPM = SFM × 3.82 ÷ D comes from 12 ÷ π ≈ 3.82, which the Cutting Tool Engineering article above also explains. The metric version of that constant is 1000 ÷ π ≈ 318.3.
Worked example: metric
The numbers below are arithmetic illustrations only. They are not recommended cutting data for any material or tool. Always take Vc and fz from your tool maker.
Inputs: D = 10 mm, Z = 4, Vc = 100 m/min, fz = 0.05 mm/tooth, ae = 5 mm, ap = 10 mm, L = 300 mm.
| Step | Calculation | Result |
|---|---|---|
| Spindle speed | (100 × 1000) ÷ (π × 10) = 3,183.10 | 3,183 RPM (rounded) |
| Feed rate | 3,183 × 0.05 × 4 | 636.6 mm/min |
| Feed per revolution | 636.6 ÷ 3,183 | 0.2 mm/rev |
| Actual cutting speed at 3,183 RPM | (π × 10 × 3,183) ÷ 1000 | 100.0 m/min |
| Material removal rate | (5 × 10 × 636.6) ÷ 1000 | 31.83 cm³/min |
| Cutting time, one 300 mm pass | 300 ÷ 636.6 | 0.47 min (about 28 s) |
Worked example: imperial
Again, illustration only.
Inputs: D = 0.5 in, Z = 3, SFM = 300, fz = 0.002 in/tooth.
| Step | Calculation | Result |
|---|---|---|
| Spindle speed | (300 × 12) ÷ (π × 0.5) = 2,291.83 | 2,292 RPM (rounded) |
| Feed rate | 2,292 × 0.002 × 3 | 13.75 in/min |
| Feed per revolution | 13.752 ÷ 2,292 | 0.006 in/rev |
| Actual surface speed at 2,292 RPM | (π × 0.5 × 2,292) ÷ 12 | 300.0 SFM |
SFM to RPM: how diameter changes spindle speed
For the same cutting speed, a smaller tool must spin faster. RPM is inversely proportional to diameter, so halving the diameter doubles the RPM. The same logic holds on a lathe: as the part diameter shrinks, RPM must rise to keep the same surface speed.
Metric view. Vc is held at 100 m/min purely to show the relationship.
| Tool diameter (mm) | RPM at Vc = 100 m/min |
|---|---|
| 3 | 10,610 |
| 6 | 5,305 |
| 10 | 3,183 |
| 12 | 2,653 |
| 16 | 1,989 |
| 20 | 1,592 |
Imperial view, same SFM, different diameters. SFM is held at 300 purely to show the relationship.
| Tool diameter (in) | RPM at 300 SFM |
|---|---|
| 0.25 | 4,584 |
| 0.50 | 2,292 |
| 0.75 | 1,528 |
| 1.00 | 1,146 |
Imperial view, same diameter, different SFM. Here D is held at 0.5 in to show that RPM rises in direct proportion to SFM.
| Surface speed (SFM) | RPM on a 0.5 in tool |
|---|---|
| 100 | 764 |
| 200 | 1,528 |
| 300 | 2,292 |
| 400 | 3,056 |
Chip load, feed per revolution and feed rate: what is the difference?
These three values are related but not interchangeable, and mixing them up is one of the most common sources of wrong feed rates.
| Value | Per what? | Formula link | Example from the metric case above |
|---|---|---|---|
| Chip load (fz) | Per tooth, per revolution | The value you take from your tool maker | 0.05 mm/tooth |
| Feed per revolution (fn) | Per full revolution | fn = fz × Z | 0.05 × 4 = 0.2 mm/rev |
| Feed rate (Vf) | Per minute | Vf = fn × RPM | 0.2 × 3,183 = 636.6 mm/min |
If a data sheet gives a feed per revolution, divide by the number of flutes to get chip load per tooth before using any chip load calculator or the feed rate formula.
What happens when your machine cannot reach the calculated values
Real machines have limits. The calculator lets you enter a maximum spindle speed and a maximum machine feed, and it tells you plainly when a limit changes the result.
Example: spindle limit. Using the metric inputs above (D = 10 mm, Z = 4, Vc = 100 m/min, fz = 0.05 mm/tooth) on a machine limited to 2,500 RPM:
| Item | Without limit | With a 2,500 RPM limit |
|---|---|---|
| Spindle speed | 3,183 RPM | 2,500 RPM |
| Actual cutting speed | 100.0 m/min | 78.5 m/min (below target) |
| Feed rate (same chip load) | 636.6 mm/min | 500 mm/min |
Example: feed limit. If the same job is run at 3,183 RPM but the machine can only feed at 500 mm/min, the chip load actually achieved is 500 ÷ (3,183 × 4) ≈ 0.0393 mm/tooth, lower than the planned 0.05 mm/tooth. The calculator shows this as "Feed per tooth used" and warns you that the actual chip load is lower than planned.
How to use the CNC Feed & Speed Calculator
- Choose your units. Switch between Metric and Imperial. Values you have already typed are converted for you.
- Pick a mode. "Feed & Speed" gives RPM and feed rate. "Surface Speed & RPM" converts between cutting speed and RPM for any rotating tool, including drills, face mills and lathe work.
- Enter the required values. Tool diameter, number of flutes, cutting speed and chip load. Take the last two from your tool maker's data sheet, since the calculator contains no preset cutting data.
- Add optional inputs. Radial width of cut and axial depth of cut (for material removal rate), maximum spindle speed, maximum machine feed, and cut path length (for cutting time).
- Read the results. You get spindle speed, feed rate, feed per revolution, the chip load actually used, and optionally material removal rate and cutting time.
- Check the formulas. Every result is shown with the formula and your numbers.
- Copy the result. The copy button saves the inputs, results, formulas and a disclaimer as plain text for your notes or setup sheet.
The calculator runs in your browser, offers a light and a dark theme, and works on phone, tablet and desktop screens.
Input checks built in
The calculator rejects zero, negative and non-numeric values, requires a whole number of flutes, and flags a radial width of cut larger than the tool diameter.
Unit conversions
| From | To | Multiply by |
|---|---|---|
| inches | millimetres | 25.4 (exact) |
| millimetres | inches | 1 ÷ 25.4 ≈ 0.03937 |
| feet | metres | 0.3048 (exact) |
| SFM | m/min | 0.3048 |
| m/min | SFM | 1 ÷ 0.3048 ≈ 3.2808 |
| mm/min | in/min | 1 ÷ 25.4 ≈ 0.03937 |
| in/min | mm/min | 25.4 |
Quick checks: 100 m/min ≈ 328.1 SFM, 300 SFM = 91.44 m/min, 100 in/min = 2,540 mm/min.
Common mistakes
| Mistake | Why it matters | What to do instead |
|---|---|---|
| Mixing metric and imperial values | Results can be wrong by a factor of 25.4 or 3.28 | Pick one unit system and check the unit label on every field |
| Using a made-up chip load | Too little or too much per tooth can harm tool life and finish | Use your tool maker's recommended chip load |
| Entering feed per revolution as chip load per tooth | Feed rate will be off by a factor equal to the flute count | Divide by the number of flutes first |
| Ignoring spindle or feed limits | The programmed values may be impossible on your machine | Enter your machine limits so the calculator warns you |
| Treating the result as final | Rigidity, runout, wear and workholding are not in the formulas | Treat results as a starting point and start conservatively |
| Using tool diameter for a lathe cut | On a lathe the workpiece diameter sets the surface speed | Enter the part diameter as D |
| Rounding RPM too early | Small rounding errors carry into the feed rate | Let the calculator round RPM once, then compute feed from that RPM |
What the formulas do not include
These formulas are simplified. They do not account for machine rigidity, tool deflection or runout, tool wear, workholding, material condition, coolant, spindle power and torque, chatter, or tool geometry and coating. Real results will differ, which is why your tool maker's data and your machine's limits always come first.
Frequently asked questions
What is a CNC feed and speed calculator?
It is a tool that calculates spindle speed (RPM) and feed rate from tool diameter, flute count, cutting speed and chip load, using standard machining formulas.
How do I use an RPM calculator for milling?
Enter the cutter diameter and the cutting speed recommended by your tool maker. The calculator applies the cutting speed formula to give RPM. Add flutes and chip load to also get the feed rate.
What is the cutting speed formula?
In metric, Vc = (π × D × RPM) ÷ 1000, with Vc in m/min and D in mm. In imperial, SFM = (π × D × RPM) ÷ 12, with D in inches.
How do I convert SFM to RPM?
Use RPM = (SFM × 12) ÷ (π × D) with D in inches. For example, 300 SFM on a 0.5 in tool gives about 2,292 RPM.
What is the feed rate formula?
Feed rate = RPM × chip load per tooth × number of flutes. For example, 3,183 RPM × 0.05 mm/tooth × 4 flutes = 636.6 mm/min.
What is chip load, and how does a chip load calculator work?
Chip load, also called feed per tooth, is the thickness of material each cutting edge removes per revolution. A chip load calculator rearranges the feed rate formula. In this tool, the used chip load is shown as Vf ÷ (RPM × Z), which tells you the real value when a machine limit changes your feed.
What is the difference between cutting speed, surface speed and SFM?
They describe the same idea: the speed of the tool's outer edge relative to the workpiece. Metric uses m/min and is usually written Vc. Imperial uses surface feet per minute (SFM).
Does this calculator give recommended cutting speeds for my material?
No. It contains no preset or recommended cutting data. You enter the cutting speed and chip load from your tool maker's data sheet.
Can I use it for drills, face mills and lathe work?
Yes for the speed calculation. The Surface Speed & RPM mode works for any rotating tool, and for lathe work you enter the part diameter as D.
Does it work in both metric and imperial?
Yes. You can switch units at any time, and entered values are converted automatically.
Are the results guaranteed to be safe?
No. They are theoretical estimates. Always verify them against your tool maker's data and your machine's limits, and follow your workshop's safety rules.
Summary
- RPM comes from cutting speed and diameter:
RPM = (Vc × 1000) ÷ (π × D). - Feed rate comes from RPM, chip load and flutes:
Vf = RPM × fz × Z. - Smaller tools need higher RPM for the same cutting speed.
- Chip load is per tooth, feed per revolution is per turn, feed rate is per minute.
- Take cutting speed and chip load from your tool maker, never from guesswork.
- Treat every calculated value as an estimate and start conservatively.
Try the calculator: Open the CNC Feed & Speed Calculator
Disclaimer:
This article and the calculator provide general information and theoretical estimates only. They are not engineering, manufacturing, safety or professional advice. You are responsible for checking all values against your tool maker's data, your machine manual and your workshop procedures before running any program, and for following all safety rules, including guarding and protective equipment.