On the shop floor, the difference between a well-finished part and a smoking disaster usually comes down to two numbers: cutting speed and feed. They are neither magic nor pure instinct; they are calculated, adjusted and corrected with experience. Here is what they mean, how they relate to each other, and how to start from the manufacturer's table so you are not working blind.
The four parameters that rule
Before you touch the spindle, it helps to have the concepts straight. If you are starting out and want the wider picture of the trade, it is worth going over what a machinist is and the role of the CNC lathe and milling machine.
Cutting speed (Vc)
This is the speed at which the cutting edge passes through the material, measured in metres per minute (m/min). It is the reference parameter because it depends above all on the material-tool pairing: cutting aluminium with a carbide insert is not the same as cutting stainless with high-speed steel. The Vc is given by the manufacturer in their table; you do not invent it, you look it up.
Spindle speed (n)
These are the revolutions per minute (rpm) of the spindle. Vc and rpm are not the same thing: Vc is constant for a given material, but the rpm change with the diameter. A large diameter turns slowly to respect the Vc; a small one turns fast. That is where the key formula comes from.
Feed (f and fz)
Feed is how far the tool advances per revolution or per tooth. On the lathe we talk about feed per revolution (f, in mm/rev). In milling we start from feed per tooth (fz, in mm/tooth) because the cutter has several edges. Feed governs the finish and the chip thickness.
Depth of cut (ap)
This is how much material is removed on each pass, measured on the radius (mm). Together with the feed it defines how much you are asking of the machine. In roughing you want a high ap to remove material fast; in finishing, a small ap and a fine feed to leave a good surface.
The formulas you need
Two formulas will see you through 90% of cases.
Spindle speed from cutting speed:
n = Vc · 1000 / (π · D)
Where D is the diameter in mm (of the part on a lathe, or of the cutter in milling). The factor of 1000 converts the metres in Vc to millimetres so the units match. Rearranged the other way: Vc = π · D · n / 1000.
Feed per tooth and per minute (milling):
Vf = fz · z · n
Where Vf is the table feed in mm/min, fz the feed per tooth, z the number of teeth on the cutter and n the rpm. On a lathe the working feed is f directly (mm/rev), which multiplied by n gives the feed in mm/min.
How to start from the manufacturer's table
This is the crux, and where many people go wrong: do not memorise figures, learn to read the table. Every maker of inserts or cutters publishes recommended Vc and feed ranges for each material and each geometry. The sensible procedure is:
- Identify the material of the part and its group (manufacturers use family codes: steels, stainless, cast iron, aluminium and so on).
- Find your tool in the catalogue: insert grade, geometry and feed recommendation.
- Take a mid-range value for Vc and feed as a starting point. The ranges are indicative; the real value depends on your machine and set-up.
- Calculate the rpm with the formula and round to a speed your machine offers.
- Try it, listen, adjust. The sound, the chip and the finish will tell you whether you are running light or over the top.
If you have no catalogue to hand, the tooling distributor usually supplies tables and calculators. Never use figures you heard somewhere without checking them: cutting values depend on the specific material and the specific tool.
Adjusting for the real situation
The table assumes ideal conditions. On the shop floor they almost never are, so correct downwards where you have to:
- Rigidity of the set-up: with a long overhang, a slender part or a tool poorly held, drop the Vc and feed to avoid vibration (the famous chatter). If it starts rattling, back off.
- Cooling: without coolant, or with air only, many materials call for a more conservative Vc so the edge does not burn. With good cooling you can go towards the top of the range.
- Finishing vs roughing: for roughing prioritise ap and feed (removing material); for finishing, raise the Vc a little and drop the feed to leave a good surface.
- Tool condition: a worn edge needs gentler parameters and, above all, to be changed in good time.
A simple worked example
Suppose we are turning a carbon steel bar on the lathe with a carbide insert. The manufacturer's table gives an indicative Vc range and we pick, as a starting point, Vc = 200 m/min. The bar has a diameter D = 40 mm.
We work out the spindle speed:
n = Vc · 1000 / (π · D) = 200 · 1000 / (3.1416 · 40) ≈ 200000 / 125.66 ≈ 1592 rpm
We round to a speed available on the machine, say 1600 rpm. For roughing we pick an indicative feed f = 0.25 mm/rev and a depth ap = 2 mm. The feed in mm/min would be:
Vf = f · n = 0.25 · 1600 = 400 mm/min
With those numbers you start, watch the chip (it should come off in manageable pieces, not in a tangle) and adjust. If the bar chatters because of overhang, drop the rpm and feed. If you are after finish, reduce the feed to 0.10-0.12 mm/rev and raise the Vc slightly.
Keep in mind that as the diameter reduces while you turn, holding the same Vc would mean raising the rpm; that is why CNC lathes offer constant surface speed mode. If you want to get the terminology straight, the glossary is there, and if you are thinking of taking this up, see how to become a machinist.
The shop-floor summary
Vc is set by the material and the tool; the rpm come from the Vc and the diameter; the feed defines the finish and the chip; the depth, how much you remove. Always start from the manufacturer's table, calculate, try it and adjust by listening to the machine. With practice that adjustment becomes automatic.