How to Calculate Speed and Feed CNC Settings
This guide is for engineers and machinists who need real numbers at the machine, not a catalog of formulas. It walks through surface speed, rpm, chipload and feed rate in the order you use them, then shows how to adjust when the cut sounds wrong. After reading, you should be able to calculate speed and feed CNC values for aluminum, steel and titanium and know which variable to change first.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
- 8
Key takeaways
What you actually need before you calculate speed and feed CNC values
Every speed and feed number comes from four inputs: tool diameter, tooth count, workpiece material and cutter material. Nothing else matters until you have those. Write them down before touching a calculator, because a single wrong tooth count turns a good cut into a broken end mill.
The cutting speed, written Vc, is the surface speed of the tool edge relative to the material. It is measured in meters per minute (m/min) or surface feet per minute (sfm). It is not a machine setting. It is a property of the material pair you are cutting: carbide in 6061 aluminum runs far faster than carbide in Ti-6Al-4V.
The feed per tooth, written fz, is how much material each cutting edge removes per revolution. Multiply it by the number of teeth and by rpm and you get the table feed in mm/min. That is the value you type into the control.
One warning before we start. Catalog values assume a rigid setup with short tool overhang and a machine in good condition. A part held in a vise on a 4,000 mm gantry machine behaves differently from a Ø12 mm end mill in a collet holder 40 mm from the spindle nose. Treat every catalog number as an upper bound, not a target.
- 1Tool diameter (Ø)Measure it. A reground tool is no longer the size printed on the shank.
- 2Tooth count (z)Count the flutes. A 3-flute and a 6-flute tool of the same Ø need different feeds.
- 3Workpiece materialGrade matters. 6061-T6 and 7075 cut differently even though both are aluminum.
- 4Cutter material and coatingUncoated HSS, TiAlN carbide and AlTiN carbide all have different Vc ranges.
Pick the cutting speed for the material pair
Start with a Vc range, not a single number. For carbide tooling, aluminum 6061 sits around 300–500 m/min (1,000–1,650 sfm). Mild steel 1018 sits around 100–150 m/min (330–500 sfm). Stainless 304 drops to 60–100 m/min (200–330 sfm). Titanium Ti-6Al-4V is much slower at 30–60 m/min (100–200 sfm).
These ranges are wide on purpose. The low end is for roughing with a long tool, deep axial depth or a light machine. The high end is for finishing with a short, rigid setup and good coolant.
Coating changes the ceiling. An AlTiN-coated carbide tool in steel can run 20–30% faster than an uncoated one. In aluminum, a polished or ZrN-coated tool resists built-up edge better than TiAlN, which is why many shops keep separate tool sets for aluminum and steel.
If you are unsure, start at the low end of the range. You can always increase rpm after the first pass. You cannot un-break a tool.
- 1Aluminum 6061, carbide300–500 m/min. Slotting and deep pockets stay near 300.
- 2Steel 1018, carbide100–150 m/min. Hardness above 30 HRC pulls it lower.
- 3Stainless 304, carbide60–100 m/min. Work hardening punishes a stationary tool.
- 4Titanium Ti-6Al-4V, carbide30–60 m/min. Heat stays in the cut, so coolant flow matters.
Convert Vc to spindle rpm
The formula is rpm = (Vc × 1000) ÷ (π × Ø). With Vc in m/min and Ø in mm, the result is revolutions per minute. For imperial work, rpm = (sfm × 3.82) ÷ Ø in inches. The constant 3.82 is just 12 ÷ π.
Worked example. A Ø10 mm carbide end mill in 6061 aluminum at Vc = 400 m/min: rpm = (400 × 1000) ÷ (3.1416 × 10) = 12,732 rpm. Round to 12,700 rpm. If your spindle tops out at 10,000 rpm, you run 10,000 rpm and accept the lower surface speed. That is normal on a 40-taper machine.
Worked example in steel. A Ø12 mm carbide end mill in 1018 at Vc = 120 m/min: rpm = (120 × 1000) ÷ (3.1416 × 12) = 3,183 rpm. On a Ø50 mm face mill at the same Vc: rpm = (120 × 1000) ÷ (3.1416 × 50) = 764 rpm.
Notice how much the diameter matters. Doubling the tool diameter halves the rpm for the same surface speed. This is the single most common mistake we see in customer programs: a face mill running at small-tool rpm, which burns the inserts in minutes.
- 1Metric formrpm = (Vc × 1000) ÷ (π × Ø)
- 2Imperial formrpm = (sfm × 3.82) ÷ Ø
- 3Spindle limitIf the formula exceeds max rpm, cap it and log the real surface speed.
Calculate feed rate from chipload
The feed formula is vf = fz × z × rpm, where vf is the table feed in mm/min, fz is feed per tooth in mm, z is the number of flutes, and rpm is the spindle speed you just calculated. For imperial, feed in ipm = fz (in) × z × rpm.
Feed per tooth is the chip thickness the edge is designed to take. Too small and the edge rubs instead of cutting, which work-hardens stainless and burns the tool. Too large and the edge chips or the tool deflects. Most carbide end mills in aluminum want 0.05–0.15 mm per tooth depending on diameter. In steel, 0.03–0.08 mm per tooth. In titanium, 0.02–0.05 mm per tooth.
Chip thinning is the correction most people skip. When radial engagement is less than half the tool diameter, the actual chip is thinner than fz, so you can raise the feed. A common rule: at 10% radial engagement, multiply fz by about 1.3. At 25%, multiply by about 1.1. At 50% and above, use the base value.
Worked example. Ø8 mm, 4 flutes, 13,900 rpm, fz = 0.06 mm: vf = 0.06 × 4 × 13,900 = 3,336 mm/min. If the radial stepover is only 10% of the diameter, raise fz to about 0.078 mm and the feed to roughly 4,340 mm/min. Same tool, same rpm, better chip formation.
- 1Aluminum, carbide0.05–0.15 mm per tooth, scaled by tool diameter.
- 2Steel, carbide0.03–0.08 mm per tooth; lower for small tools.
- 3Titanium, carbide0.02–0.05 mm per tooth; never let the edge rub.
When the calculated numbers do not work
The formula gives you a starting point. The machine, the holder and the part decide whether you can use it. Three things override the math: tool overhang, workpiece rigidity and spindle power.
Tool overhang is the first limit. A Ø6 mm end mill sticking 60 mm out of the holder has roughly a quarter of the stiffness of the same tool at 20 mm overhang. Reduce axial depth of cut and rpm before you reduce feed. Cutting rpm reduces the cutting force, but it also reduces chip thickness, which can lead to rubbing. Reducing depth of cut is usually the safer first move.
Thin walls and tall parts behave like a tuning fork. If the workpiece rings, no tool change will fix it. Support the part, reduce radial engagement, or switch to a smaller stepover with a higher feed to keep the cutting force low and steady.
Spindle power is the hard ceiling. If spindle load sits above 85% on a roughing pass, reduce axial depth or feed. On our 5-axis centers we aim for 60–80% load on roughing, which leaves headroom for tool wear and material variation.
- 1ChatterReduce radial engagement first, then rpm by 10%.
- 2Short tool lifeReduce Vc by 10–15% and check coolant aim.
- 3Poor surface finishRaise rpm slightly or reduce fz; check for built-up edge.
- 4Spindle overloadReduce axial depth of cut, not just rpm.
Step by step: calculate speed and feed CNC values
Work through these in sequence. Each step feeds the next.
- 1Write down Ø, z, material and cutter coatingExample: Ø8 mm, 4 flutes, AlTiN carbide, 6061-T6. No calculation is valid without all four.
- 2Choose Vc from the material pair6061 aluminum with carbide: start at 350 m/min for a conservative first pass, up to 500 m/min if the setup is rigid.
- 3Calculate rpmrpm = (350 × 1000) ÷ (3.1416 × 8) = 13,926. Round to 13,900 rpm. Cap at the spindle maximum if needed.
- 4Choose feed per tooth fzFor a Ø8 mm carbide tool in aluminum, 0.05–0.10 mm per tooth is a normal band. Start at 0.06 mm.
- 5Calculate table feedvf = fz × z × rpm = 0.06 × 4 × 13,900 = 3,336 mm/min. Round to 3,300 mm/min.
- 6Check the chip load against radial engagementAt 10% radial stepover you can raise fz by 20–30%. At full-width slotting, stay at the low end.
- 7Run a test cut and read the signsListen for chatter, check chip shape and color, watch spindle load. Aim for 60–80% of spindle load on a roughing pass.
- 8Adjust one variable at a timeChatter: reduce radial engagement or axial depth first, then rpm. Short tool life: reduce Vc by 10–15%. Bad finish: raise rpm slightly or reduce fz.
Starting Vc and fz by material and tool
Carbide tooling, rigid setup, flood coolant. Use the low end for long overhang or deep slots.
| Material | Vc (m/min) | fz for Ø8 mm (mm) | Notes |
|---|---|---|---|
| Aluminum 6061-T6 | 300–500 | 0.06–0.12 | Watch built-up edge; keep coolant flowing |
| Aluminum 7075 | 250–400 | 0.05–0.10 | Harder than 6061, slightly lower Vc |
| Steel 1018 | 100–150 | 0.04–0.08 | Chips should be gray-blue, not purple |
| Steel 4140 | 80–120 | 0.03–0.07 | Above 30 HRC pull Vc down 20% |
| Stainless 304 | 60–100 | 0.03–0.06 | Never dwell; keep the edge moving |
| Stainless 17-4PH | 50–80 | 0.03–0.05 | Heat treat condition changes the range |
| Titanium Ti-6Al-4V | 30–60 | 0.02–0.05 | High-pressure coolant helps a lot |
| Brass C36000 | 200–400 | 0.06–0.12 | Free-cutting; avoid too-fine feed |
Get the first pass right, then tune
Calculate speed and feed from Vc and fz, start at the low end of the range, and change one variable at a time. That beats guessing every time.
Common questions
Should I use rpm or surface speed when programming?
Program rpm, but choose it from surface speed. The control only understands rpm and feed, so the surface speed calculation is a design step, not a machine setting.
Keep the Vc value in your setup sheet so the next operator can recalculate for a different tool diameter without guessing.
What is a good chipload for a small end mill?
For carbide tools under Ø3 mm, stay around 0.01–0.03 mm per tooth in aluminum and 0.008–0.02 mm in steel. Very small tools break from deflection more often than from heat.
If the tool squeals at the calculated feed, check runout first. More than 0.01 mm TIR will break small tools no matter what feed you use.
Does coolant change the speed and feed?
Yes, mainly for stainless, titanium and deep pockets. Flood coolant lets you hold the middle of the Vc range. Dry machining in steel usually means dropping Vc by 10–20% unless you use air blast and coated tools rated for it.
In aluminum, coolant is mostly about chip evacuation and preventing built-up edge rather than cooling the edge.
How do I handle a tool with variable helix or uneven flutes?
Use the effective tooth count the manufacturer lists, not the number of flutes you can see. A 4-flute variable helix tool may be rated as a 3-tooth cutter for feed calculation.
Start 10% below the calculated feed and raise it after the first pass. Variable helix tools are more forgiving on chatter but less forgiving on overload.
Why does the same program cut differently on two machines?
Spindle stiffness, taper condition, holder runout and coolant pressure all vary. A worn spindle bearing shows up as chatter at rpm values that worked on a newer machine.
Recalculate for the actual maximum rpm of each machine, and keep a per-machine setup sheet rather than one universal program.
Can I just use the tool manufacturer's app?
Use it as a cross-check, not a replacement. Apps usually assume a rigid setup and ideal coolant. If your setup is long, thin or lightly held, the app will give you numbers that break tools.
Compare the app output with the manual calculation. If they differ by more than 20%, find out why before pressing cycle start.
Send us your drawing and material
We quote and return a DFM analysis within 12 hours, and we will tell you if the geometry or tolerance needs a different setup before you commit to a run.
12-hour quote100% inspectionNo minimum order quantity
More machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
