CNC Turning

Turning is the fastest and cheapest way to make cylindrical parts — when the part is actually suited for it. The problem comes when someone sends a shaft with hex flats and cross-drilled holes to a conventional lathe shop, then wonders why the quote comes back with secondary operations tacked on. This page helps you pick the right lathe type up front, avoid the common design traps, and understand what actually drives cost on the shop floor.

CNC Turning vs CNC Milling — Which Process?

Start here. Turning and milling are fundamentally different: in turning, the part rotates and the tool is stationary; in milling, the tool rotates and the part is stationary. That geometric difference determines which process handles your part better — or whether you need both.

What Your Part Looks Like	Use This	Why	Cost Factor
Uniform or stepped cylinder — shafts, pins, bushings, nozzles	Turning only	The part spins, one tool cuts the OD, another bores the ID. Fast material removal, lowest cost per unit for cylindrical geometry.	1.0x (baseline)
Cylindrical body with axial features only — center holes, O-ring grooves, threads	Turning only	Drilling, grooving, and threading are all standard lathe operations. No need for a mill.	1.0x
Cylinder with flats, hex, slots, or cross-holes on the OD	Mill-turn or turning + secondary milling	Off-center and radial features require a rotating cutter. Mill-turn does it in one setup; two separate machines do it in two.	1.5–2.5x
Box, bracket, plate, housing — no rotational symmetry	Milling only	Turning can't produce non-cylindrical geometry. Milling is the correct process.	N/A (milling)
Long thin part (>10:1 L/D), tight concentricity, small diameter	Swiss-type turning	Guide bushing supports the stock right at the cut. No deflection, excellent concentricity, fast cycle time in volume.	2.0–3.0x (amortized at qty 100+)
Complex shaft with turned diameters, milled keyways, and drilled radial holes	Mill-turn center	Live tooling handles the milled and drilled features while the part is still chucked. One setup, tight positional tolerance between all features.	1.5–2.5x

The most common process mistake Sending a part that's fundamentally cylindrical to a milling machine because it has one or two off-center features. A mill-turn center handles the turning and the milling in a single setup for less total cost than turning on a lathe and then moving to a mill. But many buyers don't know to ask for mill-turn, so they end up paying for two setups on two machines.

Lathe Types Compared

"CNC lathe" is not one thing. The machine you need depends on part size, feature complexity, accuracy requirements, and batch quantity. The table below covers the three main types you'll encounter when sourcing turned parts.

Parameter	Conventional CNC Lathe	Mill-Turn Center	Swiss-Type Lathe
What it does	OD/ID turning, facing, drilling, threading, grooving — all rotational	All lathe ops + live tooling for milling, drilling off-center, cross-holes	High-precision turning of long thin parts with guide bushing support
Standard tolerance	±0.025 mm	±0.015 mm	±0.005 mm
Achievable tolerance	±0.01 mm	±0.005 mm	±0.002 mm
Surface finish (Ra)	0.8–3.2 μm	0.8–1.6 μm	0.4–0.8 μm
Max diameter	Up to 500–800mm (large chuck lathes)	Up to 300–500mm	Up to 32mm bar stock (some up to 42mm)
Max length	Up to 2000mm+ (between centers)	Up to 1000mm	Unlimited from bar (but usually <300mm finished)
L/D ratio	Up to 10:1 (tailstock), 4:1 (chuck only)	Up to 6:1	20:1 and beyond
Milling capability	None — requires secondary op	Full live tooling: end mills, drills, taps	Limited live tooling (back-working)
Sub-spindle	Optional (pickoff)	Standard on most	Standard
Setup time	30–60 min	60–120 min	120–240 min (guide bushing)
Hourly rate factor	1.0x	1.5–2.0x	1.8–2.5x
Ideal batch size	1–10,000+	10–5,000	100–1,000,000+

Why Swiss-type is expensive for low volume The guide bushing must be sized to the bar stock diameter, often to within 0.005mm. Setup involves careful alignment and test cuts to verify concentricity. For a run of 50 pcs, that setup time dominates the cost. At 1,000+ pcs, the fast cycle time (often under 30 seconds per part) more than compensates. Swiss-type is a production machine, not a prototyping machine.

When to Use Swiss-Type vs Conventional

This is the decision that gets mis-made most often in procurement. Swiss-type lathes are specialized, high-precision machines that excel at a specific range of parts. Outside that range, a conventional lathe does the same work for less money. Here's how to decide.

Decision Factor	Use Swiss-Type When	Use Conventional When
Part diameter	≤ 32mm bar stock (some machines up to 42mm). Swiss-type is built around the guide bushing — larger diameters defeat the purpose.	> 32mm. Conventional lathes handle up to 800mm chuck diameter. No contest above 50mm.
Length-to-diameter ratio	> 10:1, especially > 20:1. The guide bushing supports the stock at the cutting point, so a 5mm diameter part can be 200mm long without deflection.	≤ 10:1 with tailstock support, ≤ 4:1 chuck-only. Beyond that, the part deflects under cutting force and you lose roundness and concentricity.
Concentricity requirement	< 0.01mm between OD and ID. The guide bushing provides near-zero runout at the cut point. Swiss-type consistently achieves concentricity that conventional lathes struggle with.	≥ 0.01–0.025mm is acceptable. A well-set-up conventional lathe with a steady rest can hold 0.01mm on a good day, but not consistently across a batch.
Batch size	≥ 100 pcs. The long setup is amortized. At 1,000+ pcs, Swiss-type cycle times (often <30s) make it far cheaper per part than conventional.	< 100 pcs, or one-offs. Fast setup, flexible. No guide bushing alignment needed.
Feature complexity	Multiple OD steps, cross-drilled holes, back-side features (sub-spindle), milling — all in one cycle. Swiss-type machines with B-axis can do impressive secondary operations.	Straightforward turning: OD/ID profiles, threads, grooves, face. If the part needs milling, it goes to a second machine.
Surface finish	Ra 0.4–0.8 μm achievable directly from the machine, no grinding. The rigid setup and close tool proximity make fine finishes routine.	Ra 0.8–1.6 μm is typical. Ra 0.4 requires a dedicated finishing pass with slow feed and sharp inserts, adding cycle time.
Material type	Brass, aluminum, steel, stainless — all work well. Free-machining grades (303 stainless, 360 brass) are ideal for maximizing tool life in high-volume production.	Any machinable material. Conventional lathes are more forgiving of difficult materials (titanium, Inconel) because they use heavier, more rigid tools and deeper cuts.

Procurement tip When requesting quotes for small cylindrical parts (≤ 25mm diameter), always ask the shop if they have Swiss-type capability. If they don't, they'll quote it on a conventional lathe — which works fine for prototypes but gets expensive at volume. For production runs of small parts, a Swiss-type shop will typically be 30–50% cheaper per part despite the higher hourly rate, because cycle times are so much shorter.

Mill-Turn: When It Pays Off

Mill-turn centers are the most versatile machines in a turned-parts shop. They combine a lathe with live tooling — rotary cutters mounted in the turret that can mill, drill, and tap while the part is still chucked. The question is never "is mill-turn better?" (it almost always is). The question is "does the cost savings from one setup justify the higher machine rate?"

What Mill-Turn Enables in a Single Setup

Turned OD/ID profiles plus milled flats, hexes, and slots
Radial cross-holes drilled and tapped without removing the part from the chuck
Keyways milled into shafts with positional accuracy guaranteed by the machine, not the fixture
Angular holes and slots using the Y-axis or B-axis on multi-axis mill-turn machines
Back-side machining on the sub-spindle: the part is passed from main to sub spindle, flipped automatically, and the second end is machined — all without human handling

Cost Comparison: Two Setups vs One

Scenario	Conventional Lathe + Separate Mill	Mill-Turn (Single Setup)
Setup cost	2 setups: lathe setup ($50–80) + mill setup ($50–80) = $100–160	1 setup: $80–120
Handling / fixturing	Part must be unclamped, moved, re-chucked. Risk of datum shift between operations.	Part stays chucked. Sub-spindle picks off automatically. Zero datum shift.
Positional tolerance	Stack-up between lathe and mill datums. ±0.05–0.1mm typical between turned and milled features.	Machine guarantees position. ±0.01–0.02mm between all features.
Hourly rate	Lathe: $40–60/hr. Mill: $50–80/hr. Total depends on cycle times.	$70–120/hr. Higher per hour, but fewer total hours.
Lead time	Longer — two machines must be scheduled sequentially.	Shorter — one machine, one program, one operator.
Best for batch size	1–5 pcs where setup savings matter less than machine availability.	10+ pcs where setup amortization and cycle time savings compound.

When Mill-Turn Is Worth the Premium

Situation	Why Mill-Turn Wins
Shaft with keyway + threaded end + cross-drilled radial hole	All three operations in one setup. Conventional approach needs lathe + mill + drill press, minimum two setups.
Hydraulic manifold body with turned ports and milled mounting surfaces	Port threads are turned, mounting surfaces are milled, all datum-related. Eliminates tolerance stack-up between operations.
Part with features on both ends requiring tight coaxiality	Main spindle machines front end, sub-spindle picks off and machines back end. Concentricity between ends is guaranteed by the machine.
Production batch (100+ pcs) with turned + milled features	Single setup cycle time savings compound. At volume, mill-turn is almost always cheaper than lathe + mill.
Complex geometry that would need 3+ setups on conventional equipment	Each eliminated setup saves $50–100 in labor and fixturing, plus eliminates tolerance stack-up.

When mill-turn is NOT worth it Simple cylindrical parts with no off-center features. A conventional lathe at $40–60/hr will always beat a mill-turn at $80–120/hr for pure turning work. Don't pay for capability you don't need. Similarly, one-off prototypes of simple parts are usually cheaper on a conventional lathe because setup is faster and the shop has more machines available.

Turning Capabilities at a Glance

Parameter	Conventional Lathe	Mill-Turn	Swiss-Type
Typical tolerance	±0.025 mm	±0.015 mm	±0.005 mm
Best achievable	±0.01 mm	±0.005 mm	±0.002 mm
Surface finish (Ra)	0.8–3.2 μm	0.8–1.6 μm	0.4–0.8 μm
Max OD	500–800 mm	300–500 mm	32 mm (bar)
Max length	2000+ mm	1000 mm	Unlimited from bar
Min ID bore	1–2 mm	1–2 mm	0.5 mm
Thread types	Metric, UN, NPT, BSPT, custom	Same + milled threads	Metric, UN, custom
Thread accuracy	6H/6g (standard)	6H/6g	4H/4g achievable
Roundness	0.005–0.01 mm	0.003–0.005 mm	0.001–0.003 mm
Concentricity	0.01–0.025 mm	0.005–0.015 mm	0.002–0.005 mm

Common Materials for Turned Parts

Material	Turnability	Notes
Aluminum 6061-T6	Excellent	Fast cuts, good finish. Watch for built-up edge — use sharp inserts or DLC coating. Most common material for turned prototypes.
Aluminum 7075-T6	Very good	Stronger than 6061, slightly gummier. Good for structural shafts and bushings.
Mild Steel 1045	Good	Standard shaft material. Cuts well with uncoated or TiN-coated carbide. Produces continuous chips — chip breaker inserts recommended.
Stainless 304	Moderate	Work-hardens quickly. Keep depth of cut above 0.5mm to avoid work-hardened surface. TiAlN-coated inserts recommended.
Stainless 316	Moderate	Tougher than 304, same work-hardening issues. Slower feeds, frequent tool changes in production.
Stainless 303	Good	Free-machining grade with sulfur addition. The easiest stainless to turn. Preferred for Swiss-type production.
Brass 360	Excellent	Free-machining. Fast cycle times, excellent finish, long tool life. Standard for electrical connectors and fittings.
Titanium Ti-6Al-4V	Difficult	Low thermal conductivity means heat stays in the tool. Low cutting speeds (40–60 m/min), sharp inserts, flood coolant mandatory.
POM (Delrin)	Excellent	Plastic that machines like a dream. Fast feeds, no coolant needed, great finish. Common for bushings and wear parts.
PEEK	Good	High-performance plastic. Can be turned but generates abrasive dust. Carbide tools, compressed air cooling.
Nylon 6/6	Good	Absorbs moisture — dimensions change after machining if not stored properly. Account for 0.2–0.5% swelling in humid environments.

DFM for Turned Parts

These rules come from quoting and producing thousands of turned parts. Following them will not change what your part does — but it will reliably reduce cost, improve lead time, and eliminate the back-and-forth that delays RFQs.

DFM Rule	Guideline	Why It Matters
Avoid off-center features on conventional lathe parts	If your cylindrical part has flats, hex, or cross-holes, specify mill-turn from the start.	A conventional lathe cannot produce off-center features. The shop will quote a secondary milling operation, adding cost and lead time. Better to specify the right machine up front.
Avoid internal undercuts	Design IDs with straight walls. If an undercut is needed, use a standard groove width (2, 3, 4mm).	Internal undercuts require special relief-groove inserts or custom form tools. Standard groove widths use off-the-shelf inserts; non-standard widths require custom grinding ($150–400 per tool).
Limit thread depth	Blind hole threads: max 1.5–2x diameter. Through-hole: no practical limit.	The first 3–4 threads carry 80% of the load. Threads beyond 2x diameter add cycle time, increase tap breakage risk, and add zero functional strength. Use a thread relief ( undercut) at the bottom of blind holes.
Add thread entry chamfers	0.5–1.0mm x 45° chamfer at every thread start.	Without a chamfer, the threading tool has to start from a sharp edge, which causes burrs and can damage the first thread. Chamfers also help with assembly — bolts thread in smoothly.
Min wall thickness	1.0mm (aluminum), 1.5mm (steel), 2.0mm (stainless/titanium)	Thin walls deflect under the cutting pressure of the turning insert. The result: out-of-round bores, chatter marks, and scrapped parts. If thin walls are unavoidable, specify a mandrel or expanding arbor for the finishing pass.
Design for concentricity	Machine critical OD and ID in the same setup. If impossible, specify a turned datum diameter for the second operation to reference.	Every time you unclamp and re-chuck a part, you introduce runout. A 3-jaw chuck repeatability is typically 0.02–0.05mm. If you need 0.01mm concentricity between OD and ID, they must be cut in the same chucking — or use a 4-jaw with indication.
Use tailstock support for long parts	Any part with L/D > 4:1 needs tailstock or steady rest support.	Without support, the part deflects away from the tool. The turned diameter becomes tapered (larger at the chuck, smaller at the free end) and out-of-round. A tailstock or steady rest eliminates this.
Avoid very small step differences	Min 0.5mm diameter step between adjacent turned sections.	Steps smaller than 0.5mm are difficult to measure reliably with standard micrometers and bore gauges. They also create sharp corners that are hard to deburr. Increase the step or use a groove instead.
Parting-off width	Min parting width: 3mm. Narrow parts should be designed with a generous parting groove.	Narrow parting tools (under 3mm) are fragile and break frequently, especially in steel and stainless. A broken parting tool mid-cut scrubs the part. Wider parting tools are stronger and more reliable.
Specify standard thread sizes	Use metric (M) or UN standard sizes. Avoid custom pitches.	Standard thread inserts are stocked everywhere. Custom pitch inserts are special-order items with 2–4 week lead time and 3–5x the cost.
Account for anodize/plating thickness	For Type II anodize: subtract 10–25μm from critical diameters before anodizing.	Anodize adds material to all surfaces. A shaft that's 10.000mm before anodize will be ~10.020mm after. If it needs to press-fit into a 10.000mm bore, it won't go. Always specify post-finish dimensions or pre-finish dimensions clearly.

The undercut trap Designers often add internal undercuts (relief grooves) for O-rings or snap rings without realizing that the groove width determines the tool cost. A 2.0mm wide groove uses a standard insert that costs $15 and is in stock. A 2.5mm wide groove requires a custom-ground insert that costs $150 and takes two weeks to arrive. Always check standard groove insert widths (1.5, 2.0, 3.0, 4.0mm) before finalizing your design.

Concentricity procurement tip If your drawing calls out concentricity between OD and ID of 0.01mm, make sure both surfaces can be machined in the same setup. If the part geometry requires two setups (e.g., the ID is on the back side and can't be reached from the front), tell the shop you need sub-spindle capability or expect to pay for a custom fixture and indicator setup.

Cost Drivers for Turning

What makes one turned part cost $5 and another $500? Here are the main drivers, roughly in order of impact on the bottom line.

Cost Driver	Impact	How to Reduce It
Number of setups	High — each setup adds $40–100 in labor, fixturing, and datum re-establishment	Design for single-setup turning where possible. Use mill-turn for parts with both turned and milled features. Specify sub-spindle back-working instead of flipping manually.
Tight tolerances	High — ±0.005mm costs 3–5x more than ±0.025mm due to slower feeds, extra passes, and 100% inspection	Apply tight tolerance only to mating and datum surfaces. Leave non-critical dimensions at ±0.05mm or looser. Use GD&T to control what matters.
Surface finish requirements	Medium-High — Ra 0.4 requires a slow finishing pass with a sharp insert. Ra 0.2 may require grinding.	Ra 1.6 is the default for most turned surfaces and costs nothing extra. Only specify finer finish on sealing surfaces, bearing journals, or visible cosmetic areas.
Material cost	Medium — titanium is 5–8x the price of aluminum per kg; some grades of stainless are 3–4x mild steel	Use the cheapest material that meets your requirements. Consider that machining cost often exceeds material cost — a free-machining grade (303 stainless vs 316) can save more in cycle time than the material price difference.
Material machinability	Medium — titanium and Inconel cut 3–5x slower than aluminum, with more tool changes	Choose free-machining grades where possible (303 vs 304 stainless, 360 brass vs naval brass, 12L14 vs 1045 steel). The material premium is typically 10–20%, but cycle time savings are 30–50%.
Custom tooling	Medium — custom form tools, special grooving inserts, non-standard thread inserts	Design around standard insert sizes and widths. Standard groove widths: 1.5, 2.0, 3.0, 4.0mm. Standard thread: metric or UN. Standard drill sizes per chart.
Batch size	Variable — setup cost is fixed, so per-part cost drops significantly with quantity	At qty 1, setup can be 50–70% of the total cost. At qty 500, setup is under 5%. If you need ongoing parts, order a batch rather than piecemeal.
Inspection requirements	Low-Medium — CMM reports, material certs, first-article inspection	Only request CMM on critical dimensions. Full dimensional reports on every shipment add $15–40 per part. Ask for CMM on first article only, then switch to sampling.
Secondary operations	Low-Medium — grinding, honing, heat treatment, plating, deburring	Each secondary op means the part leaves the machine, goes to another process, comes back (or ships from another supplier). Logistics and handling add cost. Design so that turning alone achieves the required specs where possible.

Tolerance cost curve for turning Going from ±0.05mm to ±0.025mm adds roughly 15–25% to the part cost — achievable with standard inserts and a well-maintained lathe. Going from ±0.025mm to ±0.01mm adds 40–80% — now you're into finishing passes with sharp inserts and slower feeds. Going from ±0.01mm to ±0.005mm adds 100–200% — this is grinding territory on most lathes, and may require a cylindrical grinder as a secondary operation. Every tighter tolerance step costs exponentially more. Apply them surgically, not globally.

Common Mistakes

Mistake	Consequence	Fix
Specifying a cylindrical part with cross-holes as "lathe work only"	Shop quotes turning + secondary drilling on a mill. Two setups, two machines, tolerance stack-up between the turned OD and the cross-hole position.	Specify mill-turn from the start. The cross-hole is drilled in the same setup as the turning, with positional accuracy guaranteed by the machine.
Calling out concentricity tighter than the chuck can hold	Shop pushes back, requests deviation, or charges for custom fixturing with 4-jaw indication (adds $80–150 per setup).	Understand that 3-jaw chuck repeatability is 0.02–0.05mm. For tighter concentricity, specify "machine ID and OD in same setup" or accept the cost of precision fixturing.
Internal undercut with non-standard width	Custom-ground insert required. $150–400 tooling charge, 2–4 week lead time for the tool.	Use standard groove widths: 1.5, 2.0, 3.0, or 4.0mm. These use off-the-shelf inserts available same-day.
Blind hole threads deeper than 2x diameter	Long taps break. Cycle time increases. Bottom threads are incomplete and weak. The tap may not reach full depth on a lathe due to clearance.	Limit thread depth to 1.5x diameter. Add a thread relief (unthreaded counterbore) at the bottom so the tap has room to stop.
No thread entry chamfer	Burrs at thread start. First thread damaged. Assembly difficulty — bolts don't thread in smoothly.	Add 0.5–1.0mm x 45° chamfer at every thread entry. This is cheap to machine and saves assembly headaches.
Thin walls (<1mm aluminum, <1.5mm steel)	Part deflects during boring, producing out-of-round bores. Chatter marks visible on the surface. Parts may be scrapped.	Increase wall thickness. If thin walls are required, specify mandrel support for the finishing pass and expect higher cost.
Long parts (L/D > 4:1) without specifying tailstock	Part deflects, producing tapered and out-of-round diameters. The end furthest from the chuck will be undersized.	Always specify "tailstock support required" for parts with L/D > 4:1. Or design a center hole in the part end for a live center.
Specifying Ra 0.4 on all surfaces	Every surface gets a slow finishing pass. Cycle time doubles or triples. May require grinding as a secondary operation.	Ra 1.6 for non-critical surfaces. Ra 0.8 for bearing fits and mating surfaces. Ra 0.4 only for seals, dynamic pistons, or cosmetic visible areas.
Not accounting for plating/coating thickness on diameters	After anodize (Type II adds 10–25μm per surface), a shaft no longer fits its bore. A press-fit becomes a sloppy fit.	Specify post-coating dimensions on the drawing. Or clearly state "dimensions before anodize" and let the shop calculate the pre-finish sizes.
Using 316 stainless when 303 would work	316 cuts 30–40% slower than 303. More tool wear, shorter tool life, higher cost per part. The corrosion benefit is real — but only needed in specific environments.	Use 303 for non-corrosive environments. Use 316 only where corrosion resistance to chlorides or acids is required. The material price difference is small; the machining cost difference is large.
Requesting Swiss-type for a 50-piece order of 20mm shaft	Swiss-type setup time (2–4 hours) dominates the cost. Per-part price is 3–5x higher than conventional lathe for this quantity.	Use conventional lathe for prototyping and low volume (<100 pcs). Switch to Swiss-type when you move to production (500+ pcs).

← CNC Milling

Anodizing →