What cutting actually is
Cutting means removing material from a workpiece using a tool that is harder and tougher than the workpiece, through rotation and feed.
On a lathe the workpiece spins and the tool (the insert) is fed into it. So deciding "how to cut" comes down to three numbers:
- How fast it turns — cutting speed V, spindle speed N
- How far the tool advances per revolution — feed F
- How deep it bites each pass — depth of cut
Of these, V and F have values you are expected to respect, set by the material and the insert. Start there.
1. Cutting speed and spindle speed — one formula
Tooling catalogues publish cutting speed V (m/min). What you type into the machine is spindle speed N (rpm). The diameter ties the two together.
318 is simply 1000 ÷ π (and 3.82 is 12 ÷ π for the inch version). Don't overthink it — learn it in this form.
Say you are turning steel at Ø50 mm and the catalogue recommends V = 160:
N = 318 × 160 ÷ 50 = 1017.6 → about S1000
Cutting speed means the right rpm changes as the diameter changes. At the same S1000, the insert sees 2.5× the speed on Ø50 as it does on Ø20. That is why the sound changes as you face in toward the centre.
You can work out the rpm for any diameter with our cutting speed & rpm calculator (that one is still in Japanese). For chamfers, tapers and corner radii, the tool nose radius compensation calculator is in English and works offline from your home screen.
2. Feed rate — surface finish is decided almost entirely here
On a lathe, feed F is millimetres per revolution (mm/rev). That number becomes the finish on the part. These are the figures we work to:
| Feed (mm/rev) | Finish symbol | Rmax | Rz | Ra |
|---|---|---|---|---|
F0.07 | ▽▽▽ | 6.3S | 6.3Z | 1.6a |
F0.14 | ▽▽ | 25S | 25Z | 6.3a |
F0.28 | ▽ | 100S | 100Z | 25a |
| — | ~ | not specified | ||
Rmax, Rz and Ra are the same roughness measured on different scales. (The ▽ triangles are the older JIS finish marks; you still meet them on plenty of drawings.) In practice: if the drawing calls for Ra1.6, start your finishing pass around F0.07.
The theoretical roughness follows from the feed f and the insert's nose radius R:
Rz ≈ f² ÷ (8 × R) × 1000 [µm]
e.g. f = 0.14, R = 0.4
0.0196 ÷ 3.2 × 1000 ≈ 6.1 µm
Real parts come out rougher than the theory because of chatter, built-up edge and tool wear. The table above already allows for that, so it sits on the safe side. Use the formula to grasp the relationship instead: a larger nose radius gives a better finish at the same feed.
3. Cutting speed by workpiece material
The same insert wants a completely different speed depending on what you are cutting. These are the baseline figures for carbide inserts.
| Workpiece material | ISO grade | Cutting speed V (m/min) |
|---|---|---|
| Steel | P | 160 |
| Cast iron | K | 200 |
| Aluminium (non-ferrous) | N | 300 |
| Stainless steel | M | 40 |
Look at stainless at 40 — a quarter of steel. Stainless holds heat and work-hardens, so running it fast destroys the edge in seconds. "Never over-speed stainless" is the one rule to get into your hands early.
P, K, M and N are the ISO material groups, and they are printed on every box of inserts. The basic rule is to match the grade of the insert to the group of the material.
4. Cutting speed by tool grade
The same question from the tool's side. The figures are for turning with inserts, but the thinking is identical for drills and end mills.
| Tool grade | Works on | Cutting speed V (m/min) |
|---|---|---|
| HSS | anything | 10 – 40 |
| Cermet | anything | 60 – 180 |
| Carbide | matched to the material | 40 – 400 |
HSS is slow, but it cuts anything and you can grind the edge yourself. Cermet leaves a beautiful finish. Carbide is fast — but pick the wrong grade and it chips almost immediately, which is why you always read this table together with the one above.
Everything in 1 to 4 applies to drills and end mills too. The only difference is whether the tool spins or the workpiece spins. On a lathe the workpiece turns, so D is the diameter being cut; with a drill or an end mill the tool turns, so D is the tool diameter. Only the number you put in changes — N = 318 × V ÷ D, and the way the material and the grade set V, are exactly the same.
Put 1 to 4 together and the decision is always the same sequence:
① look at the material → ② choose a matching insert → ③ set V for that insert → ④ calculate N from the diameter D → ⑤ set F from the finish on the drawing
Keep that order and you will not be badly wrong, even on a material you have never cut.
5. Setup — external and internal
Speeds and feeds alone do not make parts. Real work splits into preparation you can do while the machine keeps running (external setup) and work that requires the machine to be stopped (internal setup). How well you separate the two decides how many parts you make in a day.
A stopped machine earns nothing. Finish 1–5 while the previous job is still running, and make 6–9 as short as you can — good setup really does come down to that one thing.
Making this something everyone on the floor can do
Everything above is the same in any shop. The problem was that only the experienced hands could follow that order all the way through. You find out at the dry run, at the test cut, or by crashing — because the only place to check was in front of the machine.
With LATHE-NC, that checking moves off the machine and onto a screen.
The sheets run in order, ① GRID through ⑦ G-code. You never have to ask anyone what to decide next.
Every operation plays through in sequence. Each one inherits the shape the last one left, so contact and leftover stock show up before the machine does.
When a rapid move enters the stock, or the tool bites into the finished shape, playback halts and shows you where. You find it on screen, not on the machine.
Choose the insert and the compensation is worked out for you. One reason tapers and radii come out the wrong size, gone.
Checking the path no longer costs machine time. That is exactly what shortens steps 6 to 9 of the setup.
A browser is all it takes — no permissions, no setup, nothing to get approved before it reaches the floor. The beta is free.
Anyone can follow the same order and arrive at the same result.Every operator on the floor can be a CAM operator.
See it cut in 3D, on your phone, before you cut it for real.
Nothing to install — it runs in the browser. The beta is free.