How to use this calculator
- Pick the material and tool. Select the workpiece material and whether your tool is carbide or HSS. The cutting speed comes from the table.
- Enter the tool. Enter the tool diameter and number of flutes, and the chip load (feed per tooth) from your tool maker.
- Enter the cut. Enter the axial depth of cut (ap) and radial width of cut (ae) for the pass.
- Read the results. Read spindle speed, feed rate, feed per rev and material removal rate, then tune by sound and finish.
How it works
Feeds and speeds are two linked calculations. The first sets how fast the cutting
edge moves across the work — the cutting speed Vc — which depends on
the material and tool. Picking a material and tool material below reads Vc straight
from the cutting-speed chart. Converting that surface speed and the tool diameter into
spindle speed:
n = (Vc × 1000) ÷ (π × D)
with Vc in m/min and D in mm — in imperial, n ≈ 3.82 × SFM ÷ D with D in
inches. A bigger tool turns slower for the same surface speed; the standalone
SFM to RPM calculator shows just
that conversion.
The second calculation sets how fast the tool advances — the feed rate
Vf — from the chip load fz (feed per tooth) and the number of flutes Z:
Vf = fz · Z · n. Each cutting edge should take a real chip of thickness
roughly fz; too thin and it rubs and burns, too thick and it overloads. The
feed per revolution is just fz · Z.
Finally, the material removal rate measures how hard the cut works the
machine — depth of cut × width of cut × feed rate:
Q = ap · ae · Vf. It is the best single number for comparing strategies and
for checking you are inside the spindle’s power. Once feed rate is set, the
machining time calculator turns toolpath length
and passes into cycle time, and the machining cost calculator
turns that run time into setup-amortized part cost.
Worked example
Verified against the live calculator
A 10 mm 2-flute carbide end mill in aluminum, chip load 0.05 mm/tooth, cutting 2 mm
deep × 5 mm wide. Aluminum with carbide is 800 SFM in the table, so
Vc = 800 × 0.3048 ≈ 243.8 m/min. The spindle speed is
n = 243.8 × 1000 ÷ (π × 10) ≈ 7,762 RPM. The feed rate is
Vf = 0.05 × 2 × 7,762 ≈ 776 mm/min (feed per rev = 0.05 × 2 = 0.1 mm), and
the material removal rate is Q = 2 × 5 × 776 ≈ 7,762 mm³/min (7.76 cm³/min).
Those are the numbers the calculator shows on load.
Reference data
Starting cutting speeds in surface feet per minute for HSS and uncoated carbide. The calculator multiplies the value for your chosen material and tool by 0.3048 to get m/min, then derives spindle speed. 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. |
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 I calculate CNC speeds and feeds?
Two steps. First, spindle speed from cutting speed and tool diameter: n = (Vc × 1000) ÷ (π × D), with Vc in m/min and D in mm — or n ≈ 3.82 × SFM ÷ D in inches. Then feed rate from chip load and flutes: Vf = fz · Z · n. Pick the cutting speed for your material and tool from the table below.
What is chip load (feed per tooth)?
Chip load, fz, is how much material each cutting edge takes per revolution — the chip thickness. Feed rate is chip load × number of flutes × RPM. Too little chip load rubs and burns the tool; too much overloads it. Tool makers publish a starting fz for each diameter and material.
What is material removal rate (MRR)?
MRR is how fast you cut away material: Q = axial depth × radial width × feed rate (ap · ae · Vf), in cm³/min or in³/min. It is the single best measure of how hard a cut is working the machine, so it is a good way to compare strategies and check you are not exceeding spindle power.
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. Switch the tool material to see the spindle speed and feed change.
How many flutes should I use?
Fewer flutes (2) clear chips better and suit aluminum and plastics; more flutes (3–4+) give a finer finish and higher feed in steel and stainless, where chip room matters less. More flutes raise the feed rate at the same chip load because Vf = fz · Z · n.
Are these numbers safe to run straight away?
Treat them as a starting point. They assume a rigid setup and reasonable engagement. Reduce speed and feed for full-slot cuts, deep pockets, long stick-out or a light machine, and tune by sound, finish and chip colour. Always confirm against your tool maker’s data.
Does it work in metric and imperial?
Yes — toggle SI/Imperial to switch the tool diameter and chip load between mm and inches, feed rate between mm/min and in/min, cutting speed between m/min and SFM, and MRR between cm³/min and in³/min.
Method & assumptions
- Cutting speeds are general starting points for a rigid setup; coatings, high-feed strategies, coolant and tool grade shift them substantially.
- Feed rate assumes the cutting edge actually takes a chip of about fz. At light radial engagement (ae small relative to D) the real chip thins, so you can chip-thin — raise the feed to keep the chip at target thickness.
- Reduce speed and feed for full-slot cuts, deep pockets, long tool stick-out or a light/low-power machine; the MRR is a quick check against spindle power.
- These are spindle-speed and feed targets, not a guarantee of finish or tool life — tune by sound, finish, chip colour and tool wear, and confirm against your tool maker’s data.