Machining Formulas Cheat Sheet: Turning, Milling, Drilling, Boring
Turning, milling, drilling and boring calculations actually share one core set of formulas; only the way each process converts feed differs slightly. This page collects the most-used formulas — cutting speed, spindle speed, feed, material removal rate, machining time and surface roughness — into a one-page cheat sheet, with links to the detailed calculation guide for each process.
1. Start with Three Shared Quantities: Cutting Speed vc, Spindle Speed n, Feed f
Whatever the process, the starting point is cutting speed vc and spindle speed n, converted between each other through diameter D. The third quantity, feed f, is where the processes diverge (next section).
| What to find | Formula | Unit |
|---|---|---|
| Cutting speed vc | vc = π × D × n ÷ 1000 | m/min |
| Spindle speed n | n = vc × 1000 ÷ (π × D) | rpm (rev/min) |
Which diameter is D?
In turning, D = the workpiece diameter being machined; in milling, drilling and boring, D = the tool diameter. The same tool at a different diameter gives a different vc. Ball-nose and bull-nose cutters are the exception: milling uses the effective diameter at the depth of cut (Dcap), not the nominal tool diameter — see Effective Diameter and Ball-Nose Speed.
The three shared quantities and the common symbols are listed below; always make the units consistent before substituting.
| Symbol | Name | Common unit |
|---|---|---|
| vc | Cutting speed | m/min |
| n | Spindle speed | rpm |
| D | Diameter (workpiece or tool) | mm |
| fn | Feed per revolution | mm/rev |
| fz | Feed per tooth | mm/tooth |
| z | Number of teeth (edges) | — |
| vf | Feed rate | mm/min |
| ap | Depth of cut | mm |
| rε | Corner (nose) radius | mm |
2. How Each of the Four Processes Calculates Feed
Once the shared quantities are set, the difference is in feed rate vf. Turning, drilling and single-edge boring use feed per revolution; milling uses feed per tooth times the number of edges — the step most often confused.
| Process | Feed rate formula | Note |
|---|---|---|
| Turning | vf = fn × n | fn is feed per revolution (mm/rev) |
| Drilling | vf = fn × n | Same as turning, by feed per revolution |
| Milling | vf = fz × z × n | fz feed per tooth (mm/tooth), z number of teeth |
| Boring | Single-edge vf = fn × n; multi-edge vf = fn × edges × n | Multi-edge boring uses feed per edge times the number of edges |
The table gives the industry-standard conversion formulas; the actual fn and fz values depend on material, tool and cutting conditions — look them up in the tool manufacturer's catalogue or a calculation tool rather than substituting from memory.
For detailed substitution and worked examples per process, see Turning Machining Formula Handbook, End mill Cutting Conditions Guide, Drilling Formula Handbook and Drilling Parameters Setting Guide.
3. Other Common Formulas: Removal Rate, Machining Time, Surface Roughness, Power
With speed and feed settled, the following set covers productivity and quality. Convert all units to a consistent basis before substituting.
| Item | Formula | Notes |
|---|---|---|
| Material removal rate MRR (turning) | Q = ap × fn × vc | ap (mm), fn (mm/rev), vc (m/min); result is about cm³/min. Milling and drilling forms are in the next section |
| Machining time Tc | Tc = L ÷ vf | L is feed travel (mm), vf is feed rate (mm/min); compute vf first |
| Theoretical roughness h (turning, peak-to-valley) | h ≈ fn² ÷ (8 × rε) × 1000 (μm) | fn feed per rev, rε corner radius (mm); h is the peak-to-valley height, not Ra; affected in practice by built-up edge, vibration and wear |
h is not the Ra on the drawing: at fn 0.2 and rε 0.8, h is about 6.25 μm, while Ra ≈ fn² × 50 ÷ rε (μm, per Seco technical data) gives about 2.5 μm. Matching h against a drawing Ra pushes the feed lower than needed. For actual Ra ranges by process, see Surface Roughness by Process Chart.
4. Net Power, Torque and Removal Rate
Use this set to check whether the machine has enough power and the spindle enough torque. The power formulas share one structure across the four processes; what changes is which quantity goes in and the divisor.
| Process | Net power Pc (kW) | Removal rate Q (cm³/min) |
|---|---|---|
| Turning | Pc = vc × ap × fn × kc ÷ (60 × 10³) | Q = vc × ap × fn |
| Milling | Pc = ae × ap × vf × kc ÷ (60 × 106) | Q = ap × ae × vf ÷ 1000 |
| Drilling | Pc = vc × DC × fn × kc ÷ (240 × 10³) | Q = vc × DC × fn ÷ 4 |
| Boring | Pc = vc × ap × fn × kc ÷ (60 × 10³) × (1 − ap ÷ DC) | Q = vc × DC × fn ÷ 4 |
Torque: Mc = Pc × 30 × 10³ ÷ (π × n) (N·m). ae is the radial width of cut (mm) and DC the drill or bore diameter (mm); kc is the specific cutting force (N/mm²), which varies with material and chip thickness — take its value from the tool maker’s catalogue.
The milling divisor is 1000 times the turning one (60 × 106 vs 60 × 10³) because the milling formula uses feed rate vf (mm/min) while the turning formula uses cutting speed vc (m/min). Plug the turning divisor into a milling calculation and the result is off by 1000, so the power check is wrong from the start.
5. How to Use It, in One Line
The formulas are only the shared skeleton: find n from diameter and vc, calculate vf by process, then feed those into MRR, Tc and Ra. Always look up the real vc, fn and fz in the tool manufacturer's catalogue or a calculation tool — never from memory.
Detailed calculation guides per process
Turning: Turning Machining Formula Handbook; milling: End mill Cutting Conditions Guide; drilling: Drilling Formula Handbook and Drilling Parameters Setting Guide.
Worked once: turning a φ50 workpiece at 700 rpm → vc = π × 50 × 700 ÷ 1000 ≈ 110 m/min. A 100 mm long workpiece at 1000 rpm and fn 0.2 mm/rev → vf = 0.2 × 1000 = 200 mm/min, Tc = 100 ÷ 200 = 0.5 min (30 seconds).
6. Frequently Asked Questions (FAQ)
Q: Why is the feed formula different for turning and milling?
Turning (and drilling) is single-edge continuous cutting, calculated by feed per revolution: vf = fn × n. Milling is multi-edge rotary cutting, so multiply by the number of teeth: vf = fz × z × n. Treating milling like turning without the tooth count makes the feed far too low.
Q: If I only know the cutting speed vc, how do I set the spindle speed?
Use n = vc × 1000 ÷ (π × D). In turning D is the workpiece diameter being machined; in milling, drilling and boring it is the tool diameter. A different diameter gives a different spindle speed for the same vc.
Q: Where do I find the values for vc, fn and fz?
Look them up by material, tool grade and cutting conditions in the tool manufacturer's catalogue or a calculation tool — not from memory. The recommended ranges and substitution methods for each process are in the corresponding calculation guides.
Q: Can this sheet give me the machining time directly?
Yes. Find n from vc, then vf by process, and finally Tc = L ÷ vf (L is feed travel). That gives the cutting time for one operation, not yet including air moves, tool changes and other auxiliary time.
For the full reading guides on this topic, see Surface Finish: A Complete Reading Guide and Machining Calculation Reading Guide.
Published: 2026-07-27 | Last updated: 2026-10-17
