CNC screw processing service: how to choose the right shop

• 1
  Key takeaways
• 2
  Which turning route fits your part
• 3
  What a CNC screw processing service actually does
• 4
  Reading a tolerance callout on a turned part
• 5
  Materials that turn well and materials that fight back
• 6
  Volume, changeover, and what the price really reflects
• 7
  Finishing and secondary operations
• 8
  Step by step: how to vet a screw machining supplier

Screw machining means turning from bar stock on a machine where the bar feeds through a guide bushing and slides forward as the part is cut. The tool works within a few millimeters of the bushing, so a thin shaft stays supported instead of bending away from the cutter. That single detail is why the process holds tight roundness on long, slender parts that a standard lathe cannot touch.

The classic use case is a part under about Ø32 mm with features on both ends: a thread, a shoulder, a groove, a cross-hole. A sliding-head machine with a pick-off spindle can cut the front, part it off, then grip the back and finish the second face in the same cycle. No second op, no re-chucking error.

A CNC screw processing service is not the same as general CNC turning. General turning covers a wider size range and heavier cuts. Screw machining trades cut depth for speed and repeatability. If your part is Ø50 mm with a 6 mm depth of cut, you want a lathe, not a screw machine. If it is Ø6 mm and 80 mm long with a ±0.01 mm bore, screw machining is the only route that will hit it at volume.

A blanket tolerance on a title block tells you very little. The number that matters is the tightest feature on the drawing plus the datum it is measured from. A shop quoting ±0.005 mm on everything is either guessing or planning to sort parts after the fact. Both cost you money later.

Diameter tolerance and length tolerance behave differently on a screw machine. Diameter is set by the tool offset and holds well. Length accumulates from the bar stop position, thermal growth in the spindle, and how the part is cut off. A ±0.05 mm length is normal; ±0.01 mm length needs a different cutoff strategy and often a second op.

Ask which features need a CMM report and which are checked with a micrometer on the floor. A turned part with a 0.01 mm bore and a 0.2 mm thread relief does not need a full CMM layout on every piece. Targeting the report at the critical features keeps inspection cost proportional to risk.

Surface finish follows the same logic. Ra 0.8–1.6 μm comes off the tool on most aluminum and brass. Ra 0.2–0.8 μm usually needs a finishing pass, a different insert, or a secondary polish. Specify finish only where a mating surface or seal needs it.

Free-machining grades exist for a reason. 303 stainless, 12L14 steel, C36000 brass and 6061 aluminum cut clean, break chips, and hold tolerance with ordinary tooling. If the drawing allows a free-machining grade, take it. The per-part cost difference is real.

Some parts cannot use a free-machining grade. 316L and 17-4PH stainless are common in medical and marine work, and both work-harden if the tool rubs instead of cuts. The fix is a positive rake insert, a constant feed per revolution, and no dwelling in the cut. A shop that slows the spindle down to stop chatter on 316L is making the problem worse.

Titanium and Inconel turn at low surface speed with a lot of heat in the cutting zone. High-pressure coolant through the tool is close to mandatory above a 3× diameter depth. Tool life is short and predictable, so the quote should show a tool cost line, not bury it.

Plastics behave differently again. POM and PA turn cleanly but move with temperature. PEEK needs sharp tooling and a coolant strategy that does not shock the part. On thin-wall plastic parts, measure after the part reaches room temperature, not off the machine.

Screw machining earns its keep in the middle of the volume curve. A few hundred parts is enough to amortize the cam or program setup. Tens of thousands of parts run almost unattended. Between those points, the price per part falls steadily and then flattens.

Below about 50 parts, setup dominates. A shop with no minimum order quantity will still run the job, but the first part carries most of the cost. That is normal, not a red flag. What matters is whether the shop tells you the setup cost up front instead of hiding it in a per-part rate.

Changeover time is the hidden variable. A shop that quotes a five-day delivery and then takes three days to set up the bar feeder is not slower at cutting, it is slower at changeover. Ask how long the machine stops between jobs. On a well-organized floor, it is hours, not days.

Attrition matters on small parts. Below Ø3 mm, parts get lost in the chip conveyor, in the wash, in the deburr bowl. A quote that assumes zero loss will come back for a rework order. Plan for 2–5% attrition on very small parts and agree who covers it.

A turned part is rarely shipped as-cut. Deburring is the minimum, and on a screw machine part with cross-holes it is not optional. A burr left at the intersection of a drilled hole and a turned diameter will fail a functional check even if every dimension is in tolerance.

Plating and coating come next. Electroless nickel and zinc plating are common on steel and brass. Anodizing applies to aluminum, with hardcoat for wear surfaces and clear or colored for appearance. Each process adds a dimensional change: hardcoat anodize grows the part by roughly half the coating thickness per surface, which matters on a thread.

Laser marking is often specified on the same drawing. Minimum character height is 1.5 mm for a clean mark. Below that, the mark becomes a suggestion rather than a readable identifier. If traceability is the goal, give the marking its own flat area rather than putting it on a curved turned surface.

The pitfall is stacking operations across vendors. If the shop turns the part and a separate vendor plates it, the tolerance stack and the lead time both grow. A single shop that controls turning, deburr, and finish keeps one inspection record and one ship date.