CNC Towers Six Basic Knowledge: How a Lathe Cuts Round Metal Parts
A working explanation of the six basic knowledge points behind CNC towers for design engineers and buyers who need to judge whether a round part belongs on a lathe. The page covers chip formation, tool geometry, workholding, tolerance limits, and the boundary between turning and milling. Read it and you can tell, before you request a quote, whether a part is a turning job or a milling job.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Basic knowledge one: what happens at the tool tip
On a lathe, the workpiece turns and a single-point tool feeds along the axis. The tool does not scrape material away. It shears a layer of metal ahead of the tool tip, and that layer leaves as a chip. Everything else in turning follows from this one fact.
Chip thickness depends on feed per revolution, not on spindle speed alone. Feed 0.1 mm/rev in aluminium 6061 gives a thin chip that carries heat away well. Drop to 0.02 mm/rev and the tool rubs instead of cutting, which work-hardens stainless 316 and shortens insert life.
Cutting speed sets tool temperature. Aluminium runs at 300–600 m/min with carbide, mild steel 1018 at 150–250 m/min, stainless 304 at 100–180 m/min, and titanium TC4 at 40–80 m/min. Push past these windows and the insert edge breaks down in minutes.
Depth of cut controls how much material comes off per pass. Roughing takes 2–4 mm per side on rigid setups. Finishing takes 0.1–0.5 mm per side to hold ±0.005 mm and Ra 0.8–1.6 μm without chatter.
- 1RoughingHeavy depth of cut, moderate feed, loose tolerance
- 2FinishingLight depth of cut, fine feed, tight tolerance
Basic knowledge two: tool geometry and insert choice
Insert shape decides how much of the tool can enter a feature. A 80° diamond (C shape) is strong and handles interrupted cuts. A 55° or 35° diamond reaches into corners and undercuts but flexes more, so it suits light finishing passes only.
Rake angle changes cutting force. Positive rake cuts free and suits aluminium and plastics. Negative rake is stronger and suits steel 4140 and cast iron, though it pushes the part away from the tool and demands a rigid setup.
Nose radius trades finish against vibration. A 0.8 mm radius leaves a better finish at a given feed than a 0.4 mm radius, but it also pushes harder on slender shafts. On a Ø10 mm shaft, use 0.2–0.4 mm radius or the part deflects and the diameter tapers.
Coating matters more than substrate for tool life. TiAlN suits steel and stainless at high temperature. Uncoated polished inserts suit aluminium, because coatings build up on the edge and smear the surface.
- 1AluminiumPolished uncoated insert, positive rake, high speed
- 2Stainless 304TiAlN coated, sharp edge, moderate speed
- 3Titanium TC4Sharp uncoated or AlTiN, low speed, flood coolant
Basic knowledge three: workholding sets the real limit
A three-jaw chuck is fast but repeats to about 0.05 mm. A collet repeats to 0.01–0.02 mm and grips the full circumference, which matters on thin-wall parts. For ±0.005 mm work, we often turn between centers or use a soft jaw bored in place.
Part stick-out is the most common cause of taper and chatter. A safe rule is stick-out no more than 3× the diameter for unsupported turning. A Ø20 mm bar should not project more than 60 mm without a tailstock or steady rest.
Thin-wall tubes deflect under chuck pressure. A Ø50 mm tube with a 1.5 mm wall will ovalize if clamped at full force. We bore soft jaws to the finished diameter and clamp on a thick section, or use an expanding mandrel from the inside.
For parts up to 4,000 mm long, we turn on machines with travels of 4,000 × 400 × 150 mm. Long shafts get a steady rest and a low depth of cut, typically 0.5–1.5 mm per side, to keep straightness inside 0.02 mm over the length.
Basic knowledge four: where tolerance and finish come from
Diameter tolerance on a lathe comes from three sources: thermal growth, tool wear, and machine positioning. Thermal growth on a Ø100 mm aluminium part can reach 0.01 mm after an hour of cutting if coolant flow is uneven.
Tool wear shifts the diameter steadily. An operator compensates by measuring every 10–20 parts and offsetting the tool. On a 500-part run of stainless 316, expect two or three offsets even with a coated insert.
Surface finish follows feed and nose radius. The theoretical peak-to-valley height is roughly feed squared divided by eight times the nose radius. Feed 0.1 mm/rev with a 0.8 mm radius gives about Ra 0.4 μm in theory; in practice we see Ra 0.8–1.6 μm on steel.
Achievable finish depends on material. Aluminium 6061 reaches Ra 0.2–0.8 μm with a polished insert. Stainless 316 often stops at Ra 0.8–1.6 μm because the material tears. Titanium TC4 usually lands at Ra 1.6–3.2 μm without a secondary operation.
Basic knowledge five: when turning stops and milling starts
Turning creates surfaces of revolution. A part with a single axis of symmetry, like a shaft, bushing, or flange, is pure turning work. Add a cross-hole or a milled flat and the part needs a second operation.
A mill-turn center cuts round and prismatic features in one setup. We run 16 mill-turn centers, which removes the re-clamping error that appears when a part moves from lathe to mill. For a part with a Ø0.02 mm coaxial bore and an off-axis slot, mill-turn holds the relationship in one fixturing.
Not every part belongs on a lathe. A rectangular housing with pockets on four faces is faster on a 3-axis or 5-axis mill. Turning it would mean a custom fixture and still leave the corners uncut.
The rule we use: if more than 70% of the removed volume is reachable by a tool feeding along one axis, turning is the cheaper route. Below that, milling or mill-turn wins on cycle time.
- 1Pure turningShafts, pins, bushings, flanges, threaded studs
- 2Mill-turnCoaxial bores plus cross-holes or flats
- 3MillingPrismatic parts, pockets, thin ribs
Basic knowledge six: matching material to the cut
Free-machining grades cut cleaner. Aluminium 6061 and 2024, stainless 303, and brass C36000 break chips well and hold finish. Stainless 304 and 316 gummy at low speed and work-harden if the tool rubs, so they need a sharp edge and a feed that never drops to zero.
High-strength alloys need lower speed and more rigidity. Steel 4140 and 4340 run at 120–200 m/min with coated carbide. Inconel runs at 25–50 m/min and often needs ceramic or whisker-reinforced inserts.
Plastics behave differently. POM and PA cut cleanly at high speed with sharp positive-rake tools. PEEK needs slower speed and a coolant wash to stop heat buildup. Carbon fibre and other composites wear the edge fast; polycrystalline diamond inserts last longer but cost more.
Titanium TC4 is the hardest common material to turn. It conducts heat poorly, so the edge sees most of the temperature. Use low speed, high feed, flood coolant, and never let the tool dwell. A dwell of half a second is enough to work-harden the surface.
Turning versus milling: how to route a part
Use the dominant geometry, not the drawing title, to pick the process.
| Part feature | Best process | Why | Typical tolerance |
|---|---|---|---|
| Shaft with steps and threads | Turning | All surfaces share one axis | ±0.005 mm |
| Bushing with a cross-hole | Mill-turn | One setup keeps coaxiality | ±0.01 mm |
| Flange with bolt circle | Turning then milling | Face and bore first, holes second | ±0.02 mm |
| Rectangular housing | 3-axis or 5-axis mill | Pockets sit on several faces | ±0.01 mm |
| Thin-wall tube, Ø50 × 1.5 mm | Turning with soft jaws | Chuck pressure must be spread | ±0.02 mm |
| Impeller with curved blades | 5-axis mill | No axis of revolution | ±0.01 mm |
| Long shaft, 1,500 mm | Turning with steady rest | Deflection control dominates | ±0.02 mm |
The one rule worth remembering
If the part is round and most material comes off along one axis, choose turning for cycle time and finish. If it is prismatic or carries features on several faces, choose milling or mill-turn. Mixing the two on a part that does not need it adds setups and tolerance stack-up.
Common questions about turning
Can you hold ±0.005 mm on a turned diameter?
Yes, on a rigid setup with a collet or soft jaws, a sharp finishing insert, and light depth of cut. We verify with in-process measurement and offset the tool as it wears.
It is not a default. Long shafts, thin walls, and gummy stainless push the practical limit to ±0.01 mm or wider.
Why does my turned part come out tapered?
Usually tool deflection or part deflection. Stick-out beyond 3× the diameter, a worn insert, or too heavy a finishing pass all bend the system.
Reduce depth of cut to 0.1–0.3 mm, add a tailstock or steady rest, and check that the tool is on center. A tool below center rubs; above center digs in.
What surface finish can turning reach without grinding?
Aluminium 6061 reaches Ra 0.2–0.8 μm with a polished insert. Steel and stainless typically land at Ra 0.8–1.6 μm. Titanium TC4 usually stops near Ra 1.6–3.2 μm.
Finer than that needs a secondary operation such as grinding, honing, or polishing. Turning alone has a practical floor set by feed and nose radius.
Is turning cheaper than milling for a round part?
Almost always, because a single-point tool removes volume continuously and the part needs one setup. A milling operation on the same round part means interpolating a circle, which is slower and leaves a scallop pattern.
The gap widens on long parts. A 500 mm shaft takes minutes on a lathe and much longer on a mill.
How do you hold a thin-wall tube without ovalizing it?
Bore soft jaws to the finished outside diameter and clamp on a thick section. If the whole part is thin, use an expanding mandrel and cut from the outside in.
Light depth of cut and a sharp insert reduce radial force. High chuck pressure is the main cause of ovality, not the cutting itself.
What part size can you turn?
We run machines with travels up to 4,000 × 400 × 150 mm and a Ø400 mm rotary table. That covers most shafts, bushings, and flanges.
For parts beyond that envelope, we would split the part or route it to a different process.
Send a drawing and get a routing answer
Upload your part and our engineers will tell you whether it belongs on a lathe, a mill, or a mill-turn center, with a quotation and DFM notes.
12-hour quote100% inspectionNDA on request
More machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
