§1The three parameters
Speed, feed and depth of cut are the three levers of every cut. They sound interchangeable — all three remove more metal when raised — but each one trades against a different limit, so they are never set alike.
Cutting speed (m/min) is how fast the edge passes the work; it chiefly governs tool life, and steeply (§2). Feed (mm/rev, or per tooth) is how far the tool advances each revolution; it chiefly governs surface finish (§3) and the cutting force. Depth of cut (mm) is how deep the tool is set; it chiefly governs the force and power, and how many passes a job takes (§4). Their product is the metal removal rate. The skill of setting up a cut is to raise the three as far as productivity wants while respecting the different ceiling each runs into — tool life, finish, or machine power — which is why roughing and finishing choose them so differently (§5).
Contents§2Cutting speed
Cutting speed is quoted for the material and tool, and converted to a spindle speed through the diameter; it is the parameter tool life is most sensitive to.
As the cutting-tools page set out, the spindle speed follows from N = 1000 V/(π D), and Taylor’s law V Tⁿ = C makes tool life fall steeply as speed rises — a small increase in speed can halve how long the edge lasts. Speed is therefore chosen first and conservatively: the material and tool fix a recommended cutting speed (carbide runs several times faster than high-speed steel), and that speed sits well below the maximum the edge could briefly survive, because the economic cost of a short tool life outweighs the time saved. Feed and depth are then chosen around it. Speed buys productivity at the sharpest cost in tool life, so it is spent carefully.
Contents§3Feed and surface finish
Feed controls how rough the turned surface is, through a simple geometric relationship with the tool’s nose radius — and because the relationship is quadratic, feed is the strongest lever over finish.
The feed marks leave a scalloped surface whose roughness grows with the square of the feed and falls with a larger nose radius. Turning with a 0.8 mm nose radius at 0.2 mm/rev gives Ra ≈ 0.2²/(32 × 0.8) = 1.56 µm; halve the feed to 0.1 mm/rev and, because Ra depends on f², the roughness quarters to 0.39 µm (the hero shows this for two nose radii). A bigger nose radius smooths further — 0.4 mm radius at that feed gives 0.78 µm — though too large a radius raises cutting force and chatter. The lesson: for a fine finish, reduce the feed and use a generous nose radius; the quadratic means small feed reductions pay large finish gains.
§4Depth of cut
Depth of cut sets how much stock a pass removes and, with feed, how hard the machine is worked; it is limited by cutting force, power and rigidity rather than by finish.
A deep cut removes stock in fewer passes, so roughing takes the deepest cut the machine and setup can stand. What stops it is force and power: cutting force rises with both depth and feed, and the power the spindle must supply rises with the removal rate (its own page), so an over-deep cut stalls the machine, deflects the work or provokes chatter. Depth barely affects surface finish — that is feed’s domain — so the usual strategy is to take the depth heavy for removal and control finish through feed and speed. Where the total stock is large it is shared across several roughing passes at full depth, leaving a thin, light final pass for finishing.
Contents§5Roughing and finishing
The clearest way to see how the three parameters combine is the split between roughing and finishing — two opposite settings for two opposite goals.
| Parameter | Roughing | Finishing |
|---|---|---|
| Depth of cut | heavy — remove stock fast | light — small final skim |
| Feed | high — productivity | low — fine finish (Ra ∝ f²) |
| Speed | moderate — protect tool life | higher — good finish, light load |
| Goal | maximum metal removed | size and surface quality |
| Roughing throws depth and feed at the job to shift metal, accepting a rough surface, while finishing uses a light depth and low feed for size and finish and can afford a higher speed because the light load barely wears the tool. The same three numbers, set oppositely, serve the two ends of every job. | ||
§6Choosing the numbers
In practice the three are set in order, each from what limits it, and adjusted by what the cut tells you.
Begin with speed, read from the material and tool — the figure that protects tool life. Set the depth next, as heavy as rigidity and power allow for roughing, light for the finishing pass. Choose the feed last: high for roughing, and for finishing from the finish wanted through Ra ≈ f²/(32r). Then listen to the cut — chatter means less speed, less overhang or a smaller nose radius; a poor finish means less feed or more speed; a stalling machine or blue chips mean less depth or feed. The starting numbers come from the material and tool; the final numbers come from the cut itself. Speed for life, depth for removal, feed for finish is the order to hold in mind.
Contents§7Quick reference
The working core of the page on one card rack.
Three levers
speed · feed · depth
Speed
→ tool life (Taylor, steep)
set first, conservatively
Feed
→ finish · Ra ≈ f²/(32r)
halve feed → quarter Ra
Depth
→ force & power
heavy rough, light finish
Order
speed → depth → feed
then read the cut