Turning, Threading and Surface Finish
Surface speed and feed per revolution, depth of cut, constant surface speed, threading, nose radius and the finish you get.
Surface speed and feed for turning
The workpiece spins and the tool feeds along it, so the speed is the surface speed at the workpiece diameter and the feed is per revolution. The principles are the same as in milling (see Cutting Speed, Spindle Speed and Feed Rate); the speeds below are for single-point turning, where the cutting edge is continuously engaged and can run a little faster than a milling tooth.
| Material | HSS | Carbide (coated) |
|---|---|---|
| Aluminum | 80 to 150 m/min | 250 to 600 m/min |
| Brass | 60 to 100 m/min | 150 to 300 m/min |
| Plastics | 60 to 150 m/min | 150 to 300 m/min |
| Mild steel | 25 to 40 m/min | 150 to 250 m/min |
| Alloy steel (4140) | 20 to 35 m/min | 120 to 200 m/min |
| Stainless steel (304) | 15 to 25 m/min | 100 to 180 m/min |
| Gray cast iron | 20 to 35 m/min | 120 to 200 m/min |
| Titanium | 8 to 15 m/min | 40 to 90 m/min |
n = 1 000 Vc ÷ (π D) Vf = n f
As the diameter reduces, the same surface speed needs a higher RPM; check the maximum spindle speed and the chuck’s limit for large or unbalanced work.
Depth of cut, roughing and finishing
| Pass | Depth of cut ap | Feed f | Note |
|---|---|---|---|
| Roughing | 1 to 5 mm | 0.25 to 0.5 mm/rev | Largest depth the machine and workpiece allow |
| Semi-finishing | 0.5 to 1 mm | 0.15 to 0.25 | Leave 0.2 to 0.5 mm |
| Finishing | 0.1 to 0.5 mm | 0.05 to 0.15 | Set by the finish and tolerance |
| Parting off | the blade width (2 to 4 mm) | 0.03 to 0.1 | Slower speed (about 60 %), coolant, rigid setup |
- Feed is limited by the nose radius: for roughing keep f below about half the nose radius (0.4 mm/rev for an 0.8 mm radius); above it the finish and the chip control suffer.
- Depth is limited by power and rigidity, not by the tool: a deeper cut costs less tool life than a faster one (see Tool Life, Wear and Cutting Economics).
- Depth at least 2 to 3 times the nose radius keeps the chip thick enough to break; a depth below the nose radius rubs and gives a long stringy chip.
- Support long work with a tailstock or steady rest; a slender part bends away from the tool (L ÷ D over about 5 needs support).
Worked example: roughing a Ø60 bar to Ø54, 150 mm long
- Depth of cut: (60 − 54) ÷ 2 = 3 mm. Surface speed 180 m/min: n = 955 rpm. Feed 0.30 mm/rev: Vf = 286 mm/min. One pass takes 150 ÷ 286 = 0.52 min (31 s).
- The removal rate is 180 × 3 × 0.30 = 162 cm³/min.
- As the bar turns down the RPM should rise with the diameter; a control with constant surface speed does this on each pass.
Constant surface speed and spindle limits
On a facing cut the diameter goes to zero at the center, so a fixed RPM gives a surface speed that falls to zero, while constant surface speed (G96 on most controls) raises the RPM towards infinity. Every control needs a spindle speed limit (G50 or G92 with an S value) for this reason.
Worked example: facing a Ø100 mm disc at 150 m/min
- At the edge the speed is n = 1 000 × 150 ÷ (π × 100) = 477 rpm; at a diameter of 10 mm it would need 4 775 rpm; at 1 mm 47 746 rpm.
- With a limit of 3 000 rpm the spindle stops speeding up at a diameter of 16 mm; below it the surface speed falls (at 10 mm it is only 94 m/min).
- Check the chuck and the workpiece: a high speed on an unbalanced part or a large chuck is dangerous (see Machine and Hand Tool Safety).
Nose radius and surface finish
The tip of a turning tool is rounded (the nose radius r), and the feed leaves a series of scallops on the surface. The theoretical arithmetic mean roughness is Ra = f² ÷ (32 r), with f the feed per revolution.
| Nose radius | f = 0.05 | f = 0.10 | f = 0.15 | f = 0.20 | f = 0.30 |
|---|---|---|---|---|---|
| r = 0.4 mm | 0.20 µm | 0.78 µm | 1.76 µm | 3.13 µm | 7.03 µm |
| r = 0.8 mm | 0.10 µm | 0.39 µm | 0.88 µm | 1.56 µm | 3.52 µm |
| r = 1.2 mm | 0.07 µm | 0.26 µm | 0.59 µm | 1.04 µm | 2.34 µm |
Worked example: Ra 1.6 µm
- With r = 0.8 mm and f = 0.10 mm/rev the theoretical finish is 0.10² ÷ (32 × 0.8) × 1 000 = 0.39 µm.
- To reach Ra 1.6 µm the feed must be at most √(32 × r × Ra ÷ 1 000) = 0.20 mm/rev with the 0.8 mm radius, or only 0.14 mm/rev with a 0.4 mm radius: a bigger nose radius allows a faster feed for the same finish.
- Real surfaces are rougher than the theory (about 70 % rougher in this example: 0.66 µm) because of built-up edge, vibration and wear: leave a margin, and cut finishing passes at a higher speed to avoid the built-up edge.
- A large nose radius also raises the radial force and the chatter risk on slender work: use a smaller radius there.
Turning power
Worked example: power for the roughing cut
- At f = 0.30 mm/rev the chip thickness is about f sin κ = 0.30 mm, so for mild steel kc = 1 800 × 0.30−0.25 = 2 434 N/mm².
- Pc = Q kc ÷ 60 000 = 162 × 2 434 ÷ 60 000 = 6.6 kW; the motor must supply 8.2 kW at 80 % efficiency (see Cutting Force, Power and Torque).
- The tangential force on the tool is Pc ÷ Vc = 6 573 W ÷ 3 m/s = 2 191 N: a small lathe may not deliver it.
- On a lathe with less power, reduce the depth first.
Threading
A thread is cut by a single-point tool that follows the thread helix: the feed per revolution equals the pitch, so the carriage is synchronized to the spindle. It takes several passes of decreasing depth, because the tool cuts on a growing length of edge.
external thread depth ≈ 0.6134 P internal thread depth ≈ 0.5413 P pass k of N: depthk = h × √(k ÷ N)
Worked example: an M20 × 2.5 external thread
- Thread depth h = 0.6134 × 2.5 = 1.53 mm (1.35 mm for the internal thread). In 8 passes the cumulative depths follow h √(k ÷ 8) as below.
| Pass | Cut this pass | Total depth |
|---|---|---|
| 1 | 0.54 mm | 0.54 mm |
| 2 | 0.22 mm | 0.77 mm |
| 3 | 0.17 mm | 0.94 mm |
| 4 | 0.15 mm | 1.08 mm |
| 5 | 0.13 mm | 1.21 mm |
| 6 | 0.12 mm | 1.33 mm |
| 7 | 0.11 mm | 1.43 mm |
| 8 | 0.10 mm | 1.53 mm |
- Threading speed is lower than turning: 30 m/min with carbide gives 477 rpm on the Ø20 mm bar, a feed rate of 1 194 mm/min and 1.5 s per 30 mm pass: 12 s for 8 passes.
- Infeed at 29° along the flank (compound infeed) so that the chip forms on one flank and curls away; finish with one or two spring passes at no depth.
- Use a coolant on steel, a sharp insert and keep the RPM below what the machine can synchronize (a coarse pitch needs a lower RPM so that the carriage can keep up).
Facing, parting off and grooving
Worked example: parting off a Ø40 bar
- Parting is slow because the blade is thin and deep in the cut: use about 60 % of the turning speed (90 m/min, 716 rpm on Ø40) and a feed of 0.06 mm/rev.
- The blade must cut a radius of 20 mm: 20 ÷ (716 × 0.06) = 28 s at a fixed RPM; with constant surface speed the RPM rises as the diameter falls, which shortens it.
- Keep the blade on center and square, the overhang short, and lubricate well; withdraw to clear chips on deep parting.
- Facing: the tool cuts towards the center; the surface speed falls to zero there, so use constant surface speed and a light finishing pass.
- Grooving: feed slowly (0.03 to 0.1 mm/rev), use a narrow tool with coolant and dwell at the bottom for a clean groove.
- Chip control: a groove or a chip breaker on the insert makes short chips at the right feed and depth; a long stringy chip means the depth or the feed is too low.
Troubleshooting
| Symptom | Likely cause | Try |
|---|---|---|
| Long stringy chips | Feed or depth too low for the chip breaker | Raise the feed or the depth; change the insert geometry |
| Poor finish with wavy marks | Chatter, a long overhang, a nose radius too large | Shorten the overhang, a smaller radius, change the speed, support the work |
| Finish too coarse | Feed too high for the nose radius | Lower the feed or use a larger radius (Ra = f² ÷ 32 r) |
| Taper on a long bar | The work bends away from the tool | Support with a tailstock or steady; light finishing passes |
| Thread is torn or the wrong pitch | Spindle and carriage not synchronized, wrong gearbox or G-code | Check the pitch, the lead and the threading cycle; lower the speed |
| Insert wears in minutes | Speed too high or no coolant | Lower the speed 20 %; use coolant; check the grade |
| Parting blade breaks | Not on center, too high a feed, chips packing | Center the blade, lower the feed, lubricate, withdraw to clear |
Related
- Speeds and Feeds: the overview of this guide.
- Speeds and Feeds by Material: speeds and chip loads by material.
- Drilling, Reaming, Tapping and Boring: boring and drilling on the lathe.
- Lathe Turning Calculator and Turning: Lathes and Operations and Designing for Turning.
FAQ
What feed should I use when turning?
Roughing 0.25 to 0.5 mm/rev, finishing 0.05 to 0.15 mm/rev, limited to about half the nose radius when roughing.
How do I get a better finish when turning?
Lower the feed, use a larger nose radius (Ra = f² ÷ 32 r), increase the speed to avoid built-up edge, and reduce vibration with a shorter overhang or support.
What is constant surface speed?
The control raises the RPM as the diameter decreases to keep the surface speed constant (G96); a spindle limit (G50) stops it racing near the center.
How many passes does a thread need?
About 6 to 10 for a 2.5 mm pitch, with decreasing depths following depth × √(k ÷ N), plus one or two spring passes.
References
- Oberg, E., et al., Machinery’s Handbook (turning speeds and feeds, thread forms and thread-cutting).
- Sandvik Coromant, Turning Handbook and Metal Cutting Technology (nose radius, feed and finish; threading).
- ISO 68-1 and ISO 261 (ISO metric screw thread basic profile); ISO 4287 (surface texture: Ra).
Last reviewed: October 2026. Speeds, feeds and finishes are typical: your machine, tool and material set the real values.