Surface finish calculator: Ra from feed
What finish a finishing pass leaves at your feed and insert nose radius — or which feed to use for the Ra you need.
Quick answer
Theoretical Ra ≈ 0.0321 × f² / r, Rz = f² / (8r) (f = feed per rev, r = nose radius). Example: 0.006 IPR with a 1/32″ radius → Ra ≈ 37 µin; 0.15 mm/rev with r 0.8 mm → Ra ≈ 0.90 µm. A real cut is a bit rougher than theory.
- Surface finish Ra (theoretical)
- —
- —
- Feed per minute (G94)
- —
- Peak-to-valley Rz (theoretical)
- —
- Min. finishing depth of cut (≈ ⅔ r)
- —
This is the theoretical minimum from the tool geometry. Real surfaces are rougher: chatter, built-up edge, insert wear, machine rigidity. Wiper inserts give roughly twice as good a finish at the same feed.
Feed per revolution for a target Ra
Theoretical values, mm/rev. Leave some margin for the finishing pass.
| Radius r, mm | Ra 6.3 | Ra 3.2 | Ra 1.6 | Ra 0.8 | Ra 0.4 |
|---|---|---|---|---|---|
| 0.2 | 0.20 | 0.14 | 0.10 | 0.07 | 0.05 |
| 0.4 | 0.28 | 0.20 | 0.14 | 0.10 | 0.07 |
| 0.8 | 0.40 | 0.28 | 0.20 | 0.14 | 0.10 |
| 1.2 | 0.49 | 0.35 | 0.24 | 0.17 | 0.12 |
| 1.6 | 0.56 | 0.40 | 0.28 | 0.20 | 0.14 |
Recommended depth of cut (per side)
⚠ These numbers are approximate, not rules. Cutting data is chosen from the insert maker's recommendations and the rigidity of your particular machine, so yours may differ noticeably. Start conservatively and adjust by the result.
A guide for carbide on a small lathe. Depth is per side (radial); the diameter shrinks by twice as much. Finishing values assume a 0.4 mm (1/64″) nose radius. A common insert-maker rule: finishing depth at least ⅔ of the nose radius (from 0.5 mm with r 0.8), or the insert rubs instead of cutting.
| Material | Roughing ap, mm | Finishing ap, mm | Finishing feed, mm/rev |
|---|---|---|---|
| Mild / medium carbon steel | 1–2.50.039–0.098″ | 0.2–0.50.008–0.020″ | 0.08–0.150.003–0.006″ |
| Stainless steel | 0.5–20.020–0.079″ | 0.2–0.40.008–0.016″ | 0.08–0.150.003–0.006″ |
| Cast iron | 1–30.039–0.118″ | 0.2–0.50.008–0.020″ | 0.1–0.20.004–0.008″ |
| Aluminum | 1–40.039–0.157″ | 0.2–0.50.008–0.020″ | 0.05–0.150.002–0.006″ |
| Brass, bronze | 1–30.039–0.118″ | 0.2–0.50.008–0.020″ | 0.08–0.150.003–0.006″ |
| Plastics (nylon, acetal) | 1–40.039–0.157″ | 0.3–10.012–0.039″ | 0.1–0.20.004–0.008″ |
Who needs it and why
A drawing calls out a surface finish — Ra 125 µin or Ra 63 µin. What gets you there is mostly the finishing feed and the insert nose radius. The calculator shows which feed gives the Ra you need and how much stock to leave for the finishing pass.
- Setting up a finishing pass — which feed to use for the Ra on the drawing and how to write it per minute.
- Choosing an insert — how the finish changes with a 1/64″ radius instead of 1/32″.
- When the finish is worse than expected — compare with the theoretical value: if the real one is much worse, the cause is chatter, wear or built-up edge, not the feed.
- Planning — how much stock to leave for the finishing pass in different materials.
The formulas
A tool with nose radius r leaves an arc on the part every revolution, shifted by the feed f. Between the arcs there are cusps of height Rz = f² / (8 · r), and the average roughness is Ra ≈ 0.0321 · f² / r (about Rz / 4). Feed is squared: halve the feed and the roughness drops four times; double the radius and it halves.
To turn feed per revolution and RPM into feed per minute for the program, use the RPM and cutting speed calculator. The online generator and the Turn G-code app take a separate feed for the finishing pass.