Screw processing: the key of modern manufacturing
Screw processing turns bar stock into threaded and turned parts at high cycle rates, with the same program repeating part after part. This page explains the mechanism, the machines behind it, the tolerance and finish range it can hold, and the geometries where it stops making sense. Written for design engineers and buyers who need to pick a process, not a slogan.
What screw processing actually does
Screw processing is turning performed on a machine built around bar stock instead of a chucked blank. The bar feeds through a guide bushing, and the tool cuts close to that bushing so the workpiece stays supported right at the point of contact. That single detail drives most of the geometry limits you will hit later.
The name comes from the original job: screws, pins, and small threaded fasteners, run in large batches on cam-driven screw machines. CNC versions replaced the cams with servo axes and a program. The motion is the same, the setup is not. A job that took hours of cam changes now takes minutes of offset entry.
Two families dominate. Sliding-head machines pull the bar through a bushing while the tools stay close to the support point. Fixed-head machines with a chuck or collet hold the blank and move the tool on a turret. A mill-turn center adds live tooling and a B axis, so cross-holes, flats, and slots come off in the same cycle.
For our shop, 16 mill-turn centers and 12 four-axis mills carry most screw-type work, with 16 simultaneous 5-axis centers handling the parts that need angled features. Bar capacity is the practical limit: below Ø1 mm the stock buckles or whips, and above roughly Ø65 mm the guide bushing advantage fades and a chucked lathe is usually the better call.
- 1Bar-fed, not blank-fedStock enters through a guide bushing or collet, so the tool always cuts near a support point.
- 2Program repeats, not the operatorOnce offsets are set, cycle-to-cycle variation comes from tool wear and thermal drift, not from hand feeding.
- 3One cycle, several featuresLive tooling and sub-spindles let you cut threads, cross-holes, and a back-side chamfer without a second op.
Sliding-head vs fixed-head: which machine runs your part
Sliding-head machines win on long, slender parts. Because the guide bushing sits millimeters from the tool, a Ø3 mm shaft with an 8:1 length-to-diameter ratio stays straight. On a chucked lathe the same part deflects under cutting force and you chase taper all afternoon.
Fixed-head machines win on short, stiff parts with large diameter changes. If your part is Ø40 mm with a Ø20 mm shoulder, the stock does not need full-length support, and a turret lathe gets there with simpler tooling and easier chip evacuation.
Swiss-type is often used as a synonym for sliding-head, though the two are not identical. The distinction matters less than the support principle: if the cutting zone is close to a bushing, you get slender-part capability; if it is not, you need the part to support itself.
Tool count drives cycle time more than spindle speed on small parts. A part with six features and four tools available runs in one pass. The same part with eight features may need a second op, and that second op costs more than the machining itself in fixture time and handling.
- 1Pick sliding-head whenL/D is above 4:1, the diameter is under Ø32 mm, and features are mostly axial or on the OD.
- 2Pick fixed-head whenThe part is short and stiff, or the diameter step is large relative to the bar.
- 3Pick mill-turn whenCross-holes, flats, or slots would otherwise need a second operation on a mill.
What tolerance and finish screw processing can hold
On a well-set sliding-head machine, turning holds ±0.005 mm (±0.0002 in) on diameters in a stable run. That number assumes a sharp tool, a rigid bushing, and a material that does not work-harden at the cut. Push past it and you are measuring the machine's thermal drift, not the part.
Threads are where screw processing shows its value. Because the thread is cut in the same cycle as the shank, concentricity between thread and shank stays tight, which matters for any part that threads into a bore and also pilots on its OD. Rolling threads instead of cutting them adds fatigue strength but needs a larger blank.
Surface finish follows tool nose radius and feed. Ra 0.8–1.6 μm is the normal band for turned features at production feeds. Ra 0.2–0.8 μm is reachable with a wiper insert, a slower feed, or a finish pass, but it costs cycle time. As-machined Ra 1.6–3.2 μm is fine for most internal parts.
Watch the material. Stainless 303 cuts cleanly and holds tolerance; 304 and 316L work-harden at the cut and will push a light finishing pass into chatter if the feed is too low. Titanium TC4 and Inconel need lower surface speeds and more tool changes, which shows up in both cycle time and cost.
- 1±0.005 mmPractical floor on turned diameters in a stable production run, not a one-off.
- 2Ra 0.8–1.6 μmStandard turned finish at normal feeds with a sharp insert.
- 3Thread concentricityCut in the same cycle as the shank, so runout stays tight without a second op.
Tooling, setup, and where the cost hides
Cycle time is visible. Setup and tooling are where the money actually goes on small runs. Changing from one bar diameter to another means a different guide bushing, a different collet, and a fresh set of offsets. On a 200-piece order that changeover can equal the machining time.
Thread tools are single-purpose. A M4 × 0.7 thread tool does not cut a 10-32 UNF thread. If your part family mixes metric and imperial threads, budget for more tools and more setup, or standardize the thread on the drawing.
Bar remnants are real cost. A 3 m bar leaves an end piece too short to grip, and that scrap is priced into the order. On expensive stock like titanium or beryllium copper, nesting parts to reduce remnant loss matters more than shaving a second off the cycle.
Deburring is the quiet step. Turned parts leave a burr at every thread exit and every cross-hole intersection. On a high-volume run, a tumbling or brushing step is normal. If your drawing calls for a burr-free edge on a cross-hole, say so, because it changes the process plan.
- 1Bar change costNew bushing, new collet, new offsets. Amortize it across the order before quoting.
- 2Thread toolingOne tool per thread form. Mixed metric and imperial means more tools.
- 3DeburringThread exits and cross-hole breaks need a defined edge condition on the drawing.
Material behavior on a screw machine
Free-machining grades exist for a reason. 303 stainless, 12L14, and C36000 brass cut fast, break chips cleanly, and hold tolerance without drama. If your part is a bushing, spacer, or pin and the drawing allows a free-machining grade, take it. The cycle time difference against 304 is often 30% or more.
Aluminum is the easy case. 6061, 2024, 6082, and 7075 all turn well at high spindle speed. 7075 holds a better finish on thin walls; 6061 is more forgiving on deep cuts. The one trap is thread galling on anodized aluminum, so specify a thread class that leaves clearance.
Titanium and Inconel are the hard cases. Both generate heat at the cut, both work-harden, and both wear tools. Cycle times run several times longer than the same part in steel. Screw processing still works, but the economics only hold when the geometry genuinely needs turning.
Plastics behave differently again. POM and PA cut cleanly but hold chips and generate static. PEEK needs sharp tools and a coolant strategy or it smears. Carbon fibre is abrasive and will destroy a carbide insert quickly, so it usually belongs on a different process route.
- 1Free-machining grades303, 12L14, C36000. Take them when the drawing allows.
- 2AluminumHigh speed, good finish. Watch thread galling after anodizing.
- 3Titanium and InconelWork-hardening and tool wear push cycle time up sharply.
Process fit by part geometry
Use this when the drawing is done and you are choosing a route
| Part condition | Screw processing fit | Why | Watch out for |
|---|---|---|---|
| L/D above 4:1, under Ø32 mm | Strong fit | Guide bushing supports the cut zone | Bar whip at high spindle speed |
| Short stubby part, large step | Weak fit | Support comes from the part itself | Turret lathe is simpler |
| Thread plus cross-hole | Strong fit | Live tooling cuts both in one cycle | Tool count limits feature number |
| Deep axial hole past 5× D | Conditional | Peck cycle adds time | Chip packing in 304 and 316L |
| Hardened steel above 45 HRC | Weak fit | Tool wear dominates cost | Grinding may be cheaper |
| Thin-wall tube under 0.5 mm | Conditional | Bushing supports, but clamping marks | Ovality after release |
| One-off prototype | Workable | No minimum order quantity here | Setup amortized over one part |
The short answer
If your part is slender, under Ø32 mm, and needs a thread plus a few turned features, screw processing is the right route. If it is short and stiff with a large diameter step, or harder than 45 HRC, a chucked lathe or grinding will cost less and hold tolerance more easily.
Questions engineers ask next
What is the smallest diameter screw processing can run?
Below Ø1 mm the bar starts to buckle and whip, and the guide bushing cannot stabilize it reliably. Between Ø1 mm and Ø3 mm the process works, but spindle speed and bar support have to be tuned per material.
If your part is smaller than that, ask about the feature directly. Sometimes the geometry can be redrawn to keep the critical diameter above the practical floor.
Can screw processing cut a thread and a cross-hole in one cycle?
Yes, if the machine has live tooling and enough stations. The thread is cut on the main spindle and the cross-hole is drilled with a driven tool, either on the main spindle or after a sub-spindle transfer.
The limit is tool count, not capability. A part with more features than available stations needs a second operation, which adds handling and fixture cost.
How does screw processing compare to a chucked lathe on cost?
For small, slender parts in volume, screw processing is usually cheaper per piece because bar feeding runs unattended and cycle times are short. For short, stiff parts or very small quantities, a chucked lathe avoids the bushing and collet changeover.
The crossover sits around a few hundred pieces for simple parts, and much lower when the part needs live tooling that a turret lathe does not have.
Which materials are hardest to run on a screw machine?
Inconel and titanium TC4 are the hardest in our experience. Both work-harden, both hold heat at the cut, and both wear inserts quickly. Cycle times can run several times longer than the same part in 303 stainless.
Carbon fibre and other abrasive composites are also difficult, mainly because tool life drops fast. Those parts often move to a different process route.
Do you inspect every screw-processed part?
We run raw material checks, in-process monitoring, and a final inspection before shipment. Reports are available on request.
For tight-tolerance features we measure against the drawing at the machine and confirm at final inspection, so the tolerance you see on the report is the one the part was accepted against.
What bar size does your equipment handle?
Our mill-turn and multi-axis capacity covers a range of bar and blank sizes. The practical upper bound for screw-type work is around Ø65 mm, above which a chucked lathe is usually the better route.
Tell us the part diameter and length and we will confirm the machine and the tooling before quoting. We quote and return a DFM analysis within 12 hours.
Send the drawing, get a process answer
We quote and return a free DFM analysis within 12 hours, covering the machine route, tooling, and the features that will drive cost. No minimum order quantity, from one prototype to 10,000+ part runs.
12-hour quote100% inspectionNo minimum orderNDA on request
More process notes
We publish setup notes, tooling trials and inspection data from the factory floor.
