CNC Turning
Also: turning, CNC lathe, lathe work, live tooling, mill-turn, turned parts, CNC lathe machining, bar-fed turning
CNC turning makes shafts, bushings, pins and fittings by spinning bar stock against a fixed cutting tool; live tooling adds cross holes and flats in the same setup.
5,131 CNC machining companies in the Noramark directory
CNC machining shops by state
A chuck or collet grips the bar and spins it at up to several thousand rpm while single-point tools on a turret move along the axis (Z) and across it (X) to cut diameters, faces, grooves, tapers, threads and bores. A bar feeder lets the lathe cut a part, part it off and pull the next length without an operator. Live (driven) tools on the turret with a C-axis spindle add cross-drilled holes, flats, keyways and bolt circles; a sub-spindle takes the part off to finish the back side, so a complete part drops off in one cycle.
Turning is the fastest and cheapest way to make anything round, because it is a continuous cut in a rigid setup. Diameters hold ±0.025 mm (±0.001") routinely and ±0.013 mm (±0.0005") with care; finishes of 0.8 µm Ra (32 µin) come straight off the tool. Threads, ODs and bores cut in one chucking are concentric within 0.013 mm (0.0005"), which is why a turned part with a critical bore is finished in one setup wherever possible.
The part has to be mostly rotationally symmetric, and off-axis features are limited to what live tools can reach. Long slender work deflects: above a length of four or five diameters it needs a tailstock, and above ten it belongs on a Swiss machine. Very high volumes of simple parts move to multi-spindle screw machines, and parts with more milling than turning are cheaper on a mill-turn center or a mill.
At a glance
| Typical tolerances | Standard ±0.05 mm (±0.002") on diameters and ±0.13 mm (±0.005") on lengths; ±0.013 mm (±0.0005") on diameters with care, and ±0.005 mm (±0.0002") after grinding. Concentricity and runout of 0.013 mm (0.0005") between features cut in one chucking; about 0.05 mm (0.002") between main-spindle and sub-spindle features unless the shop qualifies the pickoff. |
|---|---|
| Size limits | Bar-fed lathes take bar to 50-80 mm (2-3") diameter and cut parts up to about 300 mm (12") long from bar. Chucked work goes to 400-600 mm (16-24") diameter and 1,000-2,000 mm (40-80") between centers on common machines, with larger lathes at fewer shops. Parts under about 3 mm (1/8") diameter belong on a Swiss machine. |
| Surface finish | As-turned 0.8-1.6 µm Ra (32-63 µin) on diameters and faces; 0.4 µm Ra (16 µin) with a finishing insert, a fine feed and a rigid setup in steel, brass or aluminum; 0.1-0.2 µm Ra (4-8 µin) after grinding, honing or polishing. Feed marks run around the part, which suits seals. A parted-off end carries a small nub unless it is faced on the sub-spindle. |
| Lead time | Prototypes in 3-7 business days; bar-fed production in 2-4 weeks, longer when a special bar size or a mill cert has to be ordered. Grinding, plating or heat treatment adds about a week per operation. |
Typical of U.S. job shops; confirm with the shop for your part.
Materials
Free-machining steels (12L14, 1215) and C360 brass turn fastest, followed by 1018, 1045, 6061 and 7075; 4140 turns well annealed or pre-hardened to 28-32 HRC. Among stainless grades 303 and 416 cut freely, 304 and 316 work-harden and want a positive rake and steady feed, and 17-4 PH is turned in condition A or H1150 then aged. Titanium and Inconel turn at a fraction of the speed with rigid setups and flood coolant. Delrin, nylon and PEEK turn cleanly; PTFE and UHMW deflect and need sharp tools and light cuts.
What drives the cost
- Cycle time: stock removed, length, number of tools, and the cutting speed the material allows
- Material: brass and 12L14 cut at two to three times the speed of 304 and ten times the speed of titanium
- Live-tool and sub-spindle work, which turns a ten-second part into a minute of cycle
- Tolerances below ±0.025 mm (±0.001") and finishes below 0.8 µm Ra
- Quantity: bar-fed setups amortize quickly, so unit price falls steeply from 10 to 500 pieces
- Long, thin or thin-walled geometry that must be cut slowly to avoid chatter and deflection
- Secondary operations: grinding, thread rolling, plating, passivation, heat treatment
When to use it
- Shafts, pins, bushings, spacers, fittings, nozzles and standoffs: anything round
- Quantities from one to tens of thousands, bar-fed at the higher end
- Diameters and concentricity held to ±0.013 mm (±0.0005") without grinding
- Threads, grooves, tapers and bores that must be concentric with the OD
- Turned parts with a few cross holes, flats or keyways, done in one cycle on a live-tool lathe
When not to
- Prismatic parts with no axis of symmetry: mill them
- Slender parts under about 20 mm (3/4") diameter with length more than ten times the diameter: Swiss machining supports the bar at the cut
- Volumes above 50,000 of a simple shape, where a multi-spindle screw machine or cold heading is cheaper
- Very large, heavy or unbalanced parts that cannot be gripped and spun safely
Design tips
- Design from a standard bar size: the smallest stock diameter that covers the largest feature saves material and roughing time.
- Put a chamfer or radius on every edge and end; sharp edges become burrs and add deburring cost.
- Keep unsupported length under about four diameters; longer parts need a tailstock center, so put a center hole on the drawing.
- Specify threads by class (6g/6H or 2A/2B) and give a relief groove or thread runout so the tool can exit.
- Expect a radius at the bottom of a bore or shoulder; a tool cannot cut a sharp inside corner.
- Tolerance diameters tighter than lengths; a lathe holds a diameter to ±0.013 mm far more easily than a shoulder position.
- Say which features must be concentric to which, with a runout tolerance to a datum, rather than tightening every diameter.
Tools and guides
Frequently asked questions
- What is the difference between CNC turning and CNC milling?
- In turning the part spins and the tool is fixed; in milling the tool spins and the part is fixed. Turning is for round parts and holds diameters and concentricity best; milling is for prismatic parts. A mill-turn center does both in one setup.
- What tolerances can a CNC lathe hold?
- ±0.025 mm (±0.001") on diameters is routine and ±0.013 mm (±0.0005") is achievable with care and gauging. Tighter than that, or finishes below 0.4 µm Ra, means grinding after turning. Lengths and shoulder positions hold about ±0.05-0.13 mm (±0.002-0.005").
- What is live tooling on a lathe?
- Powered rotary tools mounted on the turret, used with a C-axis that indexes and holds the spindle. They drill cross holes, mill flats and keyways and tap off-center holes while the part is still in the chuck, which avoids a second operation on a mill and keeps everything concentric to the turned features.
- How big a part can be CNC turned?
- Bar-fed work runs to 50-80 mm (2-3") diameter. Chucked parts go to 400-600 mm (16-24") diameter and up to 2 m (80") long on common machines, and larger lathes exist at heavy-industry shops. Parts under 3 mm (1/8") diameter are Swiss work.
- CNC turning or Swiss machining?
- Swiss machining wins for parts under 32 mm (1-1/4") diameter that are long, slender or need ±0.005 mm (±0.0002"), in quantities of hundreds and up. Conventional CNC turning wins for larger diameters, short parts and small quantities, because it sets up in a fraction of the time.
