CNC Feeds and Speeds, Explained
After reading this you will be able to compute a spindle RPM and feed rate for any router or mill cutter from two catalog numbers, and know how to correct them by ear and by chip color at the machine.
What feeds and speeds actually mean
Two numbers control every cut on a router or mill: how fast the cutter spins (spindle speed, in RPM) and how fast it moves through the material (feed rate, in mm/min). Set them together and you decide the thickness of each chip the tool takes. That chip thickness is the thing that matters. Too thin and the edge rubs and overheats. Too thick and the tool deflects, chatters or snaps.
Here is the hook. A 6 mm two-flute carbide endmill slotting 6061 aluminium wants roughly 17,700 RPM and a feed near 890 mm/min. Drop the feed to a cautious-feeling 200 mm/min and you have not made a safer cut. You have made a worse one: each flute now scrapes a chip so thin it cannot carry heat away, the aluminium welds to the flute, and the tool dulls in minutes. The calculator exists to keep you out of that trap by working backward from the chip.
When to use the calculator, and when not
Use it to get a starting point for a cutter and material you have not run before, or when you change diameter, flute count or tool material and want to keep the cut equally aggressive. The surface speeds and chiploads built in are mid-range values from tooling catalogs, so they land you in a sane zone on the first try.
Do not treat the output as a final answer. The numbers assume a rigid machine, a sharp tool, decent workholding and some way to clear chips. A flexy hobby router, a long stickout, or a cut buried in a deep pocket all shift the right answer downward. The calculator has no way to see your setup. You do.
Surface speed and chipload are properties of a material-and-tool pairing, not of your machine. The machine only enters through its RPM ceiling. That is why two very different routers cutting the same aluminium with the same endmill share the same target chip thickness.
The two formulas and the intuition behind them
Everything comes from two equations. The first turns a desired surface speed into a spindle RPM.
Here n is spindle speed in RPM, V_c is the cutting speed (surface speed) in m/min, and D is the tool diameter in mm. The factor 1000 converts metres to millimetres. The intuition: V_c is how fast the cutting edge should sweep past the work. A bigger tool covers more distance per revolution (its circumference is \pi D), so to hold the same edge speed a bigger tool must spin slower. Double the diameter, halve the RPM.
The second equation turns RPM into a feed rate.
v_f is the feed rate in mm/min, z is the number of flutes, and f_z is the chipload (feed per tooth) in mm. Read it plainly: each flute should cut a chip f_z thick, there are z flutes per revolution, and the tool turns n times a minute. Multiply and you get millimetres of advance per minute.
Two adjustments the calculator applies. First, the built-in chiploads are quoted at 3, 6 and 12 mm diameters, and it interpolates linearly between them, because a thin tool cannot take the same bite as a thick one. Second, slotting engages the full width of the cutter, which loads it far harder than a light side pass, so the chipload is scaled to 70% for a full-width cut.
A worked example you can reproduce
6 mm carbide, two flutes, slotting 6061 aluminium
These are the demo button values: material aluminium, carbide tool, diameter 6 mm, 2 flutes, machine max 24,000 RPM, slotting cut.
- Look up the pairing. Carbide in 6061 uses a cutting speed near V_c = 333 m/min, and at 6 mm the base chipload is about f_z = 0.05 mm/tooth.
- Apply the slotting factor:
0.05 × 0.70 = 0.035mm/tooth. - Compute RPM: n = \frac{1000 \times 333}{\pi \times 6} = 17{,}667 RPM. That is below the 24,000 ceiling, so it stands.
- Compute feed: v_f = 17{,}667 \times 2 \times 0.035 \approx 1{,}237 mm/min.
Round to a spindle setting of 17,700 RPM and a feed near 1,240 mm/min. With no depth of cut entered, the tool applies its rule of thumb of 0.5 \times D, giving a 3 mm depth for the slot. In practice you might split that into two 1.5 mm passes on a light machine.
If you switch that endmill from slotting to a light profiling pass, the chipload jumps back to the full 0.05 mm and the feed rises to about 1,767 mm/min at the same RPM. Same tool, same speed, more feed, because a side cut removes less material per revolution than a full-width slot.
How diameter reshapes the numbers
Diameter pulls the two formulas in opposite directions, which surprises people. A larger tool spins slower (RPM falls as 1/D) but takes a fatter chip (chipload rises with diameter). The chart below holds the aluminium slotting case fixed and sweeps diameter from 3 to 12 mm so you can see both curves at once.
Note the RPM at 3 mm: n = \frac{1000 \times 333}{\pi \times 3} = 35{,}340 RPM. Most hobby spindles top out at 24,000. That is where the cap earns its keep.
Reading the results and the RPM cap
The calculator reports a spindle RPM and a feed rate, and where relevant it caps the RPM. When the physics-ideal RPM exceeds your machine maximum, the tool clamps the speed and recomputes the feed at that lower speed so the chipload stays the same. The chip thickness is what you are protecting, so slowing the spindle means slowing the feed by the same proportion.
Take the 3 mm tool above. Ideal RPM is 35,340, but the machine stops at 24,000. The cap keeps the chipload and scales the feed:
Compare that with the uncapped 1,187 mm/min: capping RPM does not force a slower feed, it forces a faster one relative to the (now lower) spin, because you must still remove the same chip each tooth. Do not read a capped result as "my machine is too weak." Read it as "the chip is fine, only the surface speed is compromised," which usually just means the tool runs a little hotter than ideal.
Common mistakes
The single most common error in wood, plastics and aluminium is feeding too slowly. A slow feed feels careful. It is not. It thins the chip until the edge rubs instead of cutting, and the friction heat has nowhere to go except into the tool and the workpiece. In acrylic you get a melted, gummy edge; in aluminium the chips weld to the flutes and the tool snaps. When unsure, feed harder rather than slower.
Other frequent mistakes:
- Using four flutes in aluminium or plastic. There is no room to clear the chip, so it packs and jams. Use 1 or 2 flutes for those materials, 2 to 4 for wood and steel.
- Forgetting the slotting penalty. A full-width cut is much harder than the side cut the raw chipload assumes. The 70% factor is a starting correction, not a luxury.
- Ignoring depth of cut. The 0.5 \times D default is a rule of thumb. On a light machine or a long tool, take shallower passes and let the feed stay up.
- Running HSS numbers on a carbide tool, or the reverse. Carbide tolerates 2 to 4 times the surface speed. Pick the right tool material in the form or every downstream number is off.
Chip color is your feedback loop. In steel, straw to light-brown chips mean the speed is about right; blue chips mean too hot, so lower RPM or raise feed. In aluminium, chips should fly off dry and silvery. If they smear or stick, you are running too slow, not too fast.
Related tools
Once the cutting parameters are set, the rest of the job is layout and material. To pack parts onto stock with the least waste, use the Cut List Optimizer for lengths of bar or board, and the Sheet Goods Cut Optimizer for nesting rectangles on plywood or MDF. If your project is a 3D print instead of a milled part, the 3D Print Cost & Time Calculator estimates material, energy and time.
Frequently asked questions
Why is my calculated RPM higher than my spindle can reach?
Small tools need high RPM to hit their surface speed. A 3 mm carbide cutter in aluminium wants 35,340 RPM. If your spindle stops at 24,000, the calculator caps there and recomputes the feed to hold the chipload. You cut a little hotter than ideal, which is usually fine for short jobs.
What flute count should I choose?
Match it to chip clearance. Aluminium and plastics want 1 or 2 flutes so chips can escape. Wood runs well on 2. Steel and stainless take 2 to 4, since the chips are short and the extra edges spread the wear.
Do I always take the slotting penalty?
Only for full-width cuts, where the tool is buried on both sides. A profiling or side pass removes less material per revolution, so it uses the full chipload. Selecting the right cut type applies or removes the 70% factor for you.
The feed rate looks scary. Is it wrong?
Probably not. Modern carbide in aluminium genuinely runs at over 1,000 mm/min on a rigid machine. If your router is light or the tool sticks out far, reduce depth of cut first and keep the feed up, rather than crawling the feed and burning the edge.
Metric or imperial?
The formulas here are metric: V_c in m/min, diameter and chipload in mm, feed in mm/min. If your catalog lists SFM and inches, convert those to m/min and mm before comparing, or the numbers will not line up.
Related tools
3D Model Viewer (STL/OBJ)
Preview STL and OBJ files in 3D — orbit, measure and inspect before printing.
3D Print Cost & Time Calculator
Material, time, energy and failure-adjusted print cost.
Cut List Optimizer
Fit your parts onto the fewest boards or bars (1D).
Roof Pitch & Rafter Calculator
Rafter lengths, cut angles and pitch conversions.
Sheet Goods Cut Optimizer
Nest rectangular parts on plywood or MDF sheets (2D).
Stair Calculator
Riser and tread sizes that are safe and comfortable.