Turning: Lathes and Operations
Lathe anatomy, facing, turning, boring, grooving, threading and parting, inserts, speeds and surface finish.
The lathe
On a lathe the workpiece spins and a stationary tool removes material as it moves along (Z) or across (X) the rotating part. This makes round shapes: shafts, pins, bushings, spacers, threaded parts and anything with a diameter. A CNC lathe moves the tool under program control, so it can follow a profile of steps, tapers and curves.
- Headstock and spindle hold and turn the work. The spindle bore limits the bar diameter that can pass through.
- Chuck (three-jaw, four-jaw, collet) grips the work; see Holding the work below.
- Carriage, cross-slide and tool post carry the tool: Z moves along the bed, X across it. A turret holds several tools.
- Tailstock supports the free end of long work with a center, or holds drills and reamers.
- Axes: X (usually a diameter) and Z (along the spindle axis). Some machines have C (spindle positioning), live tooling and a Y axis for milling features on a turned part.
Turning operations
| Operation | What it does | Tool |
|---|---|---|
| Facing | Cuts the end flat and sets the length; usually the first cut | General turning tool, feeding in X to the center |
| Turning | Reduces the diameter along the length: steps, tapers and curves | General turning tool, feeding in Z |
| Boring | Enlarges a drilled hole accurately | Boring bar, feeding in Z |
| Grooving | Cuts a channel (O-ring seat, circlip groove, thread relief) | Narrow grooving insert, feeding in X |
| Threading | Cuts a helical thread | 60° threading insert, feed equals the pitch |
| Parting off | Cuts the finished part from the bar | Thin parting blade, feeding in X to the center |
| Drilling, reaming, tapping | Holes on the centerline | Drill in the tailstock or turret |
| Knurling | Presses a grip pattern on the surface | Knurling wheels (pressed, not cut) |
Speed, feed and cutting data
On a lathe the feed is per revolution of the work, not per tooth. The cutting speed is set at the diameter being cut.
n = 1 000 × Vc ÷ (π × D) Vf = n × f MRR = Vc × f × ap (cm³/min with Vc in m/min, f and ap in mm) Pc = ap × f × Vc × kc ÷ 60 000 (kW)
Here D is the diameter of the work at the cut, f is the feed per revolution (mm/rev), ap the depth of cut per side, and kc the specific cutting force (N/mm²).
Worked example: turning a 40 mm bar, ap = 2 mm, f = 0.2 mm/rev
| Aluminum (Vc 250 m/min, kc 700) | Mild steel (Vc 120 m/min, kc 1 800) | |
|---|---|---|
| Spindle speed | 1 989 rpm | 955 rpm |
| Feed rate | 398 mm/min | 191 mm/min |
| Material removal | 100 cm³/min | 48 cm³/min |
| Cutting power | 1.17 kW | 1.44 kW |
A hobby lathe with a 0.75 kW motor cannot take this cut in steel; use a lighter cut such as ap = 0.5–1 mm, or a slower speed.
Constant surface speed and constant rpm
The cutting speed falls as the tool nears the center (the diameter gets small). Many controls offer constant surface speed (G96), which raises the spindle speed as the diameter decreases to keep Vc steady, and constant rpm (G97), which holds the speed fixed. Always set a spindle speed limit (G50 on Fanuc-type controls; G92 on some) so that facing toward the center does not spin the chuck dangerously fast.
| Diameter | rpm for 200 m/min |
|---|---|
| 40 mm | 1 592 rpm |
| 20 mm | 3 183 rpm |
| 10 mm | 6 366 rpm |
| 5 mm | 12 732 rpm |
- Start values by material are in Speeds & Feeds and Machining Metals. Insert makers publish a speed and feed range for every grade.
- Depth of cut should be larger than the nose radius, and no more than about two-thirds of the insert’s cutting edge. A very light cut, below the nose radius, rubs instead of cutting.
- Feed for roughing: 0.15–0.4 mm/rev. For finishing: 0.05–0.15 mm/rev, depending on the nose radius and the finish needed.
Inserts and tool holders
Most CNC turning uses indexable inserts: small carbide plates clamped in a holder. When an edge wears, the insert is turned to a fresh edge, or replaced, with no resetting of the tool. The insert’s shape sets the nose angle (strength against access).
Reading an insert code (ISO 1832)
| Position | Example: CNMG 120408 | Meaning |
|---|---|---|
| 1 | C | Shape: 80° rhombic |
| 2 | N | Clearance angle: 0° (negative insert; used with a negative-rake holder) |
| 3 | M | Tolerance class |
| 4 | G | Hole and chip-breaker type |
| 5 | 12 | Size: inscribed circle 12.7 mm (cutting edge length about 12 mm) |
| 6 | 04 | Thickness 4.76 mm |
| 7 | 08 | Nose radius 0.8 mm |
- Negative inserts (N) are stronger and have twice the edges, because both faces are used; positive inserts (with clearance, for example CCMT) cut with less force and suit light cuts, thin parts and small lathes.
- Grades (the carbide and coating) are matched to the material: P for steel, M for stainless, K for cast iron, N for non-ferrous, S for heat-resistant alloys and titanium, H for hard materials.
- Chip-breakers curl and snap the chip into short pieces. Use the breaker for the depth and feed range, or you get long, dangerous strings.
- Holders and boring bars. Choose the holder for the insert, the approach angle, and the size of your turret. A steel boring bar can reach about 4 × its diameter; carbide bars about 6–7 ×; beyond that use damped bars.
- Small lathes often use brazed carbide tools or HSS tool bits, which can be ground to any shape and cost little.
Surface finish and nose radius
The tool nose is round, so it leaves tiny ridges between passes, a ridge height set by the feed and the nose radius. The theoretical peak-to-valley height is h = f² ÷ (8 × r) and the average roughness Ra = f² ÷ (32 × r), where f is the feed per revolution and r the nose radius, all in mm.
Worked example: finishing with a 0.8 mm nose radius
- At f = 0.1 mm/rev: Ra = 0.1² ÷ (32 × 0.8) = 0.000 mm = 0.39 µm, a fine finish.
- At f = 0.3 mm/rev: Ra = 0.09 ÷ 25.6 = 3.5 µm, suitable for roughing or a coarse finish.
- As a rule, keep the feed below about half the nose radius for roughing (0.40 mm/rev for r = 0.8) and a quarter for finishing, so that the tip is not overloaded.
- A larger nose radius gives a better finish for a given feed, but pushes the tool away more and can cause vibration on a long, thin part.
Threading
A thread is cut by feeding the tool along Z exactly one pitch per revolution of the spindle, over several passes, each deeper than the last. The controller synchronizes the feed to the spindle encoder.
Worked example: an external M10 × 1.5 thread
- Thread depth (ISO metric, external): h = 0.6134 × P = 0.6134 × 1.5 = 0.92 mm per side. The minor diameter is about 10 − 1.2269 × 1.5 = 8.16 mm.
- Cut it in about 6–8 passes, shrinking the depth of each (for example 0.30, 0.20, 0.15, 0.12, 0.10, 0.05 mm), then spring passes with no extra infeed.
- Feed = pitch = 1.5 mm per revolution; at 600 rpm the tool moves 900 mm/min. Run the spindle slowly (200–800 rpm) so the control keeps up.
- Start the thread 2–3 pitches before it begins and leave a thread relief groove at the end, so the tool can run out.
- Thread cycles: G76 (Fanuc-type) or a G33 line-by-line threading. Check the dialect and the infeed method.
- Insert: a threading insert has a 60° profile (ISO metric, Unified) matched to the pitch range; a full-profile insert cuts the crest too.
- Check with go/no-go gauges or thread wires; see Fits in Practice for thread classes.
- Coarse threads are easier to cut and less sensitive to damage; fine threads give more adjustment.
Grooving and parting off
- Grooving uses an insert as wide as the groove, which feeds straight in. Widen the groove with more passes, and use a slow feed (0.05–0.1 mm/rev); deeper grooves need more clearance and chip flow.
- Parting off uses a thin blade. The deeper it goes, the more it deflects, so keep the blade short (stick-out just past the radius), the tool exactly on center, perpendicular, and the feed constant. Reduce the feed near the center, where the blade can grab and the part can fall.
- Blade width is about 0.1 × the diameter for general parting (3 mm for 30 mm bar); the parted face usually leaves a small nub that is removed by facing.
- Support the part as it is parted off so that it does not fall into the machine or bend the blade at the end.
Boring and drilling
- Drill first (center drill, then drill) in the tailstock or turret, then bore to size. A drill follows its start and can wander, so leave stock for the boring bar.
- Boring bars are long and thin, so they deflect and vibrate. Keep the bar as short and as large as the hole allows, use a positive insert and a small nose radius, and cut light.
- Chip evacuation inside a hole is hard: use through-coolant bars, air or short chips.
- Reamers finish holes to size and tolerance, with 0.1–0.2 mm of stock.
Holding the work
| Method | Use | Typical run-out | Notes |
|---|---|---|---|
| Three-jaw chuck | Round and hexagonal stock | 0.02–0.05 mm | Self-centering; quick; jaws wear and the grip is not repeatable after turning around |
| Four-jaw chuck | Square, odd or off-center work | adjustable to 0.01 mm | Each jaw is set separately; slower but very accurate |
| Collet (5C, ER) | Small bar and finished parts | 0.005–0.01 mm | Best accuracy and grip on a small diameter |
| Soft jaws | Finished parts, thin walls, repeat jobs | bored in place | Machined to the part, so the grip is even and repeatable |
| Between centers | Long shafts, to finish in one set-up | very low | A drive dog turns the work; allows turning the whole length |
| Steady rest, follow rest | Long, slender work | — | Supports the middle or follows the tool to prevent bending |
| Faceplate, fixtures | Odd-shaped parts | — | Clamp the part to a plate bolted to the spindle; balance it |
- Grip enough. Hold at least one diameter of the work in the chuck, and do not let a long part overhang more than about 3 × its diameter without support (tailstock).
- Thin walls distort in a chuck; use soft jaws, or machine the part in a bore pad or on an expanding mandrel. See Workholding and Fixturing.
- Safety. Remove the chuck key before the machine starts, keep the guard closed, and never wear loose clothing or gloves near a rotating part. See Troubleshooting, Accuracy and Safety.
Set-up: tool height, offsets and nose compensation
- Tool height. The cutting edge should be on the spindle centerline, within about ±0.1 mm. A tool that is too low rubs and leaves a “pip” in the center when facing; too high, and the clearance is lost.
- Tool offsets. Touch the tool to a known surface (the face and a turned diameter) and store the X and Z values, so that the controller knows where the tool tip is. Wear offsets adjust the size after measuring.
- Nose radius compensation (G41 left, G42 right on a lathe) corrects the path so that tapers and arcs come out right, because the cutting point moves around the nose. Enter the tool’s nose radius and orientation (tool tip number).
- Work zero. Set Z0 on the finished face of the part and X0 on the centerline; see G-code and Programming for a worked lathe program.
- Test cut a small diameter, measure it, and correct the X offset before the finishing pass.
Related
- CNC Machining: the overview of this guide.
- Designing for Turning: drawing parts that turn well.
- G-code and Programming: lathe G-code, including a worked program.
- Workholding and Fixturing: chucks, collets and soft jaws.
- Speeds & Feeds.
FAQ
Why does the part have a pip in the center after facing?
The tool tip is above or below the centerline. Reset the tool height so that the edge is on center; a slight rise at the center of a faced end is a sign that it is not.
What is constant surface speed?
A mode (G96) in which the control changes the spindle speed as the diameter changes to keep the cutting speed constant. It gives a more even finish on a face or taper. Always set a spindle speed limit with it.
How do I choose an insert?
Choose the shape for the access you need (80° or 55° for general, 35° for profiling, round or square for heavy roughing), the grade for the material, the nose radius for the finish and strength (0.4 mm for finishing, 0.8 mm for general), and a chip-breaker for the depth and feed.
Can I turn a part longer than its diameter times three?
Yes, with support. Up to about eight diameters can be held with a tailstock center, and beyond that a steady or follow rest is needed. The deflection chart on the Designing for Turning page shows why.
Why does the thread not fit?
Common causes are a wrong pitch or the wrong feed, cutting at too high a speed for the control, a worn insert, or a thread that is too deep or too shallow. Check the pitch with a gauge, and test the fit with a mating nut before the last pass.
References
- Oberg, E. et al., Machinery’s Handbook, 31st ed., Industrial Press: turning, threading, cutting speeds and feeds.
- Sandvik Coromant, Turning Handbook, and Kennametal, Turning Tools Application Guide.
- ISO 1832, Indexable inserts for cutting tools: designation; ISO 68-1 (ISO general-purpose metric screw threads: basic profile).
- Kalpakjian, S. and Schmid, S., Manufacturing Engineering and Technology, Pearson.
- Smid, P., CNC Programming Handbook, Industrial Press (lathe G-code).
Last reviewed: October 2026. Cutting data are starting points: machines, tools and materials differ, so test on scrap and follow the tool maker’s data.