Cutting Data & Units

Cutting speed, RPM, feed per tooth and feed rate are one linked chain — not four separate numbers. This page fixes the formulas with worked examples you can reuse, and names the unit errors that most often cause scrap or edge failure.

Concept

Cutting speed (vc) is the surface speed of the edge past the work, in m/min. It is what the tool material can tolerate — set by the catalog, not by the spindle. Spindle speed (n, RPM) is what the machine actually turns; it is derived from vc and the tool/work diameter. Feed per tooth (fz) is how far the edge advances each tooth, in mm. Feed rate (vf) is how fast the tool travels through the cut, in mm/min — derived from n, number of teeth and fz.

The chain is: choose vc from the catalog for the material → compute n from the diameter → choose fz for the edge → compute vf. Speed and feed are independent levers: speed mainly drives heat and tool life; feed mainly drives force, chip thickness and surface finish.

Why It Matters

A new operator often sets RPM directly — “last time 3000 RPM worked” — which throws away the whole point of cutting speed. Change the diameter and 3000 RPM means a completely different surface speed. Working from vc keeps the edge in its comfort window regardless of tool size. The second trap is units: mixing mm/min with in/min, or mm per tooth with inches per tooth, changes a feed by a factor of ~25.4 and either rubs (too light) or overloads the edge (too heavy). This page locks the arithmetic so those mistakes are visible.

How It Works

Cutting speed to RPM

For milling and drilling (rotating tool), where D is tool diameter in mm:

n [RPM] = 1000 × vc [m/min] / (π × D [mm])

For turning (rotating workpiece), D is the current cutting diameter; the same formula applies. The 1000 converts metres to millimetres.

Feed per tooth to feed rate

vf [mm/min] = n × zc × fz

where zc is the number of effective cutting teeth (flutes or inserts engaged), and fz is feed per tooth in mm. In turning there is one edge in the cut, so feed rate reduces to vf = n × f (feed per revolution).

The three formulas locked to this course

The roughness formula uses the factor 32 (a geometric average for a sharp rounded nose); it predicts the ideal best-case Ra, never the real finish, which is worse due to wear, built-up edge and vibration.

Worked Example

1 — Cutting speed to RPM (locked: n = 3819.72)

A Ø10 mm end mill is run at a classroom cutting speed of vc = 120 m/min. Then:

n = 1000 × 120 / (π × 10)
  = 120000 / 31.4159
  = 3819.72 RPM

2 — Feed per tooth to feed rate (locked: vf = 608)

Take n = 3800 RPM, zc = 4 teeth, fz = 0.04 mm/tooth:

vf = 3800 × 4 × 0.04 = 608 mm/min

Note this deliberately rounds RPM to a realistic 3800 rather than the exact 3819.72 — you cannot set .72 RPM on a controller. The exact value is for calculation; the programmed value is what you choose on the machine.

3 — Theoretical roughness (locked: Ra ≈ 0.781 µm)

A turning finish pass uses feed f = 0.10 mm/rev and nose radius rε = 0.4 mm:

Ra = 0.10² / (32 × 0.4) = 0.010 / 12.8 = 0.000781 mm = 0.781 µm

This is the ideal floor. Real measured Ra will be higher — often several times higher — once wear and vibration appear.

4 — Drill point height (locked: h = 3.004 mm)

A Ø10 mm drill has a standard 118° included point angle. Half-angle = 59°:

h = 10 / (2 × tan 59°) = 10 / (2 × 1.6643) = 3.004 mm

Why the same RPM means a different cut on a bigger tool

The reason to work from vc rather than a remembered RPM is geometry: the edge speed past the work is the circumference per revolution, so at a fixed spindle speed a larger tool runs its edge faster than a small one. Run the locked baseline Ø10 at 3820 RPM and the edge sees about 120 m/min. Swap to a Ø20 cutter and leave the dial at 3820 RPM, and the same edge now sees ~240 m/min — double the surface speed, double the heat, and a very short tool life, even though "the RPM is the one that worked last time". This is the whole point of n = 1000·vc/(πD): the catalog tells you the surface speed the edge can survive, and you back-calculate the RPM for whatever diameter is in the holder. When you change tools, recompute n; never carry the RPM over. The same logic runs in reverse for turning, where the cutting diameter shrinks as you face or bore, which is why constant surface speed (CSS) keeps the edge temperature in a window instead of letting the part-edge speed explode at small diameters.

Why speed and feed are independent levers

It is worth saying explicitly, because new operators treat them as one "the cut is too aggressive" knob: cutting speed and feed do different jobs and cause different failures. Speed (vc) sets the edge temperature and therefore mainly drives tool life and crater wear — too hot and the edge softens or erodes. Feed (fz or f) sets the chip thickness and the force on the edge, and therefore mainly drives roughness, edge strength and chip formation — too light and the tool rubs and builds up edge material, too heavy and it overloads the corner. This is why the corrections in this course always distinguish them: a crater on the rake face is a speed problem (lower vc or a hotter grade), while a long unbroken chip or a torn finish is usually a feed problem (raise fz into the chipbreaker window, page 06), and chipping at the corner is often a feed or interruption problem rather than a speed one. When a cut is wrong, do not lower both numbers by instinct — name which symptom you see, and move the lever that controls it. That is also why the formulas keep them separate: vc gives you n, fz gives you vf, and each is chosen for a different reason.

Why the programmed feed rate is not the chip thickness

A new operator often sets vf directly ("feed 600 mm/min") and treats that as how aggressively the cut bites, but the chip thickness the edge actually feels is set by fz — the advance per tooth — not by the travel speed alone. vf = n·zc·fz means the same 600 mm/min can be produced two ways: a 4-flute tool at 3800 RPM with fz = 0.04, or an 8-flute tool at 1900 RPM with fz = 0.08. Those two cuts feed the table at identical speed, but the second tool takes twice the chip per edge, which doubles the load per tooth and changes whether the chipbreaker breaks it (page 06) and whether the corner survives. This is why the course chooses fz first and derives vf, rather than picking vf and hoping each edge is loaded sanely. It also exposes a common miscalculation: running a high-flute tool at a feed rate tuned for a low-flute tool silently halves the chip per tooth, which starves the edge into rubbing and built-up edge even though the table moves at a healthy pace. Pick fz for the edge, multiply by teeth and RPM, and let vf be the result — never the starting number.

Why the catalog speed is a starting point, not a target

The vc you read in a tool catalog is the surface speed the grade is rated for under ideal conditions — a known material, a fresh edge, adequate rigidity, and appropriate coolant. On your machine the real constraints may be tighter: a lighter-duty spindle, a long overhang, an interrupted cut, or a less-than-perfect setup. That is why the course treats the catalog vc as a starting point rather than a fixed dial: set it, run a short trial, and read the result. If the edge shows crater wear quickly, you are running hot — lower vc; if it welds a built-up edge, you may be too low (page 25). The number is not wrong because the catalog said 120 and you ran 120 and the edge failed; the assumption behind the catalog number may not match your setup. This is also why every vc on this page is tagged a classroom assumption: the arithmetic that converts vc to RPM is exact, but choosing vc itself is an engineering judgement anchored to the catalog and adjusted by the trial log.

Why you round RPM down, not up, after the calculation

When the locked n comes out to 3819.72 and the controller only takes integers, the direction of rounding is a small but real decision. Rounding up to 3820 changes the surface speed by a fraction of a percent, which is harmless; but the habit worth keeping is to round toward the safer value when the edge is near a limit. On a brand-new grade in a difficult material, landing on 3800 rather than 3820 keeps you just inside the catalog window on the first trial, and you can always step up once wear confirms the edge is comfortable. The exact 3819.72 belongs in the calculation and the cost math, while the programmed 3800 is what the spindle actually turns — the page's worked example deliberately shows both. This also keeps the locked numbers consistent: every later page that multiplies 3800×4×0.04 to get 600-series feed uses the rounded, programmable RPM, not the theoretical one, so the arithmetic traces cleanly from catalog to controller.

When a beginner mixes the units, the error is rarely obvious on the readout: a feed set in inches where millimetres are expected either barely cuts or overloads the edge. Building the habit of writing the unit next to every number on the worksheet is what prevents that class of mistake, and it also makes the worksheet readable by the next shift without guesswork.

Finally, never read a speed number off a sticker and assume it applies to every diameter; the spindle speed that is safe on a small mill may be a different condition on a large cutter at the same surface speed. Always recompute on the actual diameter in the holder.

Common Mistakes

• Forgetting the ×1000. Using vc in m/min directly with D in mm gives a result 1000× too small. Fix: always include 1000 in n = 1000·vc/(πD).
• Confusing feed per tooth with feed per revolution. Multiplying vf by zc for a turning operation (only one edge engaged) double-counts. Fix: milling uses zc; turning uses feed per revolution with zc = 1.
• Trusting the theoretical Ra as a guarantee. 0.781 µm is the geometric floor, not the shop result. Fix: measure the real surface and treat wear and vibration separately.
• Ignoring drill point height. Programming a 20 mm deep hole with a flat-bottom assumption wastes the last 3 mm. Fix: for a Ø10 drill at 118°, add 3.004 mm when planning through-hole depth.

Worked unit check. The locked baseline uses vc = 120 m/min on a Ø10 mm tool. Convert the diameter to metres for the formula: 10 mm = 0.010 m, so n = 1000·vc/(π·D) = 1000×120/(3.1416×10) ≈ 3819.7 RPM, rounded to 3800 on the machine. Then feed: vf = n·zc·fz = 3800×4×0.04 = 608 mm/min. The place people slip is the ×1000: dropping it gives 3.8 instead of 3800, and mixing mm/min with inch/min multiplies the motion by 25.4. Carry the unit with every number — m/min, RPM, mm/min, mm/tooth — rather than only the value, and the arithmetic stays honest.

When you inherit a program written in inches, do not convert one number at a time. Recompute the whole chain — speed, spindle RPM, feed per tooth and feed rate — because mixing mm/min with inch/min feeds is a common crash or poor-surface cause. Keep the units block visible at the top of the setup sheet and cross-check the first part against a hand calculation before running the batch.

One useful habit on the shop floor is to sanity-check every computed feed against what the machine is actually doing: if vf implies the tool is covering more length per minute than the table move suggests, a unit or zc error has slipped in. Write units next to every number on the setup sheet and keep a worked example at the front so the next operator repeats the same convention rather than guessing.

Finally, remember that the catalog speed is a starting point tied to a stated tool life and a stated material, not a fixed recipe. On your first cut, run near that starting speed, watch the chip and the edge, and adjust — the number on the page is the beginning of the conversation with the machine, not the end of it.

Keep a small table of your own starting speeds and feeds for the three materials you run most often, and update it each time a trial changes the setting. Over a few months that table becomes a personal baseline that beats any single catalog number, because it is already tuned to your machines and tooling.

Practice