CNC Screw Processing Guide: How Threaded Parts Are Actually Made
This guide explains what happens when a screw, stud, or threaded insert is cut on a CNC machine. It covers thread forms, single-point vs thread milling, cutting parameters, and the defects that show up in inspection. For design engineers and buyers who need to judge whether a thread can hold its class, not just whether it fits.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
What CNC screw processing actually cuts
A screw is a cylinder with a helix wrapped around it. CNC screw processing removes material along that helix in a controlled pass, so the flank angle, pitch, and root radius all come from the tool path rather than from a die. That is why the same machine can cut M3 × 0.5 in 316L in the morning and a 7/16-20 UNF stud in 4140 in the afternoon.
The cut is not one operation. On a mill-turn center the blank is turned to the major diameter, the thread is cut, and the part is parted off in one setup. If the part needs a hex head or a slot, that comes before or after on the same spindle. Every time the part is re-chucked, runout adds up and the thread starts to tilt.
The controlling dimension is the pitch diameter, not the outside diameter. Pitch diameter sits between the crest and the root, and it decides whether the thread assembles with the right clearance and the right flank contact. A screw that measures 5.97 mm on the outside and 5.38 mm on the pitch will pass a go gauge and fail a no-go gauge.
For most parts that we run, the achievable tolerance is ±0.005 mm on the turned features and a thread class held within the limits of the standard. The tolerance is not the hard part. Holding it across 10,000 pieces without the tool wearing past the limit is the hard part.
- 1Turning firstMajor diameter and any shoulder or undercut are cut before the thread.
- 2Thread secondSingle-point, thread milling, or a die head, depending on size and volume.
- 3Inspect lastPitch diameter, flank angle, and lead are checked, not just the OD.
Pick the thread form before the tool path
The thread form decides the shape of the cut. A 60° V-profile from ISO 68-1 or ASME B1.1 is the default for fasteners. A trapezoidal form such as Tr 20 × 4 moves load over a wider flank and is used on lead screws where the thread has to push something for years, not just clamp it.
Buttons and rolled threads are a different animal. A rolled thread is formed by displacing material, not removing it. The grain flows along the flank, the root is stronger, and the blank diameter is smaller than the finished major diameter. You cannot roll a thread on a part that is already finished to size, and you cannot roll a thread into a thin wall without the wall bulging.
Cut threads are the safer choice when the thread runs close to a shoulder, when the material is brittle, or when the part is a one-off. Rolled threads win on fatigue life and on cycle time once the volume justifies a die head. For a batch of 50 aluminum standoffs, cutting is cheaper. For 50,000 steel studs, rolling usually wins.
There is a third option that gets overlooked: thread milling. A single-point tool follows a helical path around the bore or boss. It cuts a full thread with one tool, handles a shoulder better than a tap, and produces a chip that clears easily. On a 5-axis machine with a Ø400 mm rotary table, a milling cutter can reach a thread that a tap cannot.
- 1V-profile 60°Standard fasteners, ISO and UN series.
- 2TrapezoidalLead screws and power transmission.
- 3RolledHigh volume, high fatigue, forged grain flow.
- 4MilledShoulders, large diameters, hard materials.
Speeds, feeds, and the numbers that matter
Threading parameters depend on pitch, material, and whether the tool is a single-point insert or a mill. For aluminum, a single-point tool runs at 150–250 m/min surface speed with a feed equal to the pitch per revolution. For 316L stainless, drop to 60–90 m/min and take two or three passes instead of one. The feed per revolution must equal the pitch exactly, or the thread lead drifts.
Depth of cut is set by the thread height. For an M8 × 1.25 thread, the radial infeed is roughly 0.81 mm total, split across passes. A common mistake is to take the whole depth in one pass on a small diameter. The tool deflects, the pitch diameter comes out oversize, and the go gauge still enters because the major diameter was cut correctly.
Coolant matters more than most people expect. In 304 and 316L, the thread root is where work hardening starts. If the tool rubs instead of cuts, the next pass cuts into a harder surface. High-pressure coolant directed at the flank, plus a sharp insert, keeps the cut in the shearing regime. Flood coolant on a deep blind hole is often not enough.
Rigidity sets the floor on what is possible. A thread cut on a Ø3 mm shank sticking 30 mm out of a collet will chatter no matter what the speed is. Support the part close to the thread, use a smaller nose radius, and accept a slower cycle. We would rather run a part at 70% of the theoretical speed than scrap a batch at full speed.
- 1Feed = pitchAny mismatch shows up as lead error along the length.
- 2Split the depthTwo or three passes for stainless, one or two for aluminum.
- 3Coolant at the flankPrevents work hardening at the root in 300-series steel.
- 4Rigidity firstShort overhang beats any parameter change on small threads.
Geometry that decides whether the thread can be cut
A thread needs room to start and room to end. On an external thread, a runout groove or an undercut lets the tool exit without leaving a partial thread. Without it, the last two threads taper and the nut binds. On an internal thread, a relief at the bottom of a blind hole does the same job for the tap or the mill.
Wall thickness is the next limit. A rolled thread on a thin-wall tube will swell the bore. As a rule, keep the wall at least 0.6 × the thread pitch for rolled threads and 0.4 × the pitch for cut threads. A M10 × 1.5 thread rolled into a 1 mm wall will ovalize the part before the thread is complete.
Thread depth beyond 2 × the diameter adds little holding strength and a lot of risk. The load is carried by the first few engaged threads. Going from 12 mm to 20 mm of engagement on an M6 thread does not double the pull-out force, but it does double the chance of a broken tap. Design for 1.5 × D to 2 × D and stop there.
Chamfer the entry. A 90° chamfer at the start of the hole or the end of the stud guides the mating part and removes the burr that would otherwise sit on the first thread. On parts that get plated, the chamfer also keeps the coating from bridging the crest. We add a chamfer by default unless the drawing says otherwise.
- 1Runout grooveLets the tool exit clean on external threads.
- 2Wall rule0.6 × pitch minimum for rolled threads.
- 3Engagement1.5 × D to 2 × D carries the load; more adds risk.
- 4Chamfer90° entry protects the first thread and the coating.
Defects that pass the eye and fail the gauge
Cross-threading is the most reported field failure and the least likely to come from the machine. It usually starts with a damaged first thread, a burr, or a chamfer that is too small. The fix is at the entry, not in the thread itself. A 0.2 mm burr on the lead thread is enough to start the mating screw at an angle.
Pitch diameter drift is the classic manufacturing defect. The major diameter is cut to size, the thread looks right, and the go gauge enters. The no-go gauge then enters too, because the pitch diameter is oversize by 0.02–0.04 mm. This comes from tool wear, from a single heavy pass, or from thermal growth on a long run. In-process gauging catches it before the batch is finished.
Lead error is harder to see. The thread is the right size but the helix advances at the wrong rate, so a nut runs tight at one end and loose at the other. It comes from feed mismatch, from spindle synchronization on a worn machine, or from a part that moved in the chuck. A lead gauge or a thread analyzer finds it. A caliper never will.
At GreatLight we check pitch diameter, major diameter, and thread class, and we run 100% inspection before shipment. Raw material certificates, in-process checks, and final reports are available on request. For a thread that has to hold a class across a full run, the gauge is the only honest answer.
- 1Cross-threadEntry damage or burr, not a thread size problem.
- 2Pitch driftOversize pitch diameter; caught by no-go gauge.
- 3Lead errorFeed or synchronization issue; needs a lead gauge.
- 4Inspection100% before shipment; reports on request.
Which threading method fits which part
Sizes are typical working ranges, not hard limits.
| Method | Typical size range | Best for | Watch out for |
|---|---|---|---|
| Single-point turning | M2 to M60 and larger | One-offs, tight pitch diameter control | Cycle time on small threads; tool deflection |
| Thread milling | M4 upward, any pitch | Shoulders, blind holes, hard materials | Needs a helical path; slower than tapping |
| Tapping | M1.6 to M20 | Through holes and shallow blind holes | Tap breakage; chip packing in blind holes |
| Thread rolling | M3 to M24, high volume | Fatigue-critical studs and screws | Blank diameter must be sized for rolling |
| Die head | M3 to M16, high volume | External threads on bar stock | Limited to external threads; setup per size |
When to cut, when to roll
Cut the thread when the part is a prototype, has a shoulder or a blind hole, or runs under a few hundred pieces. Roll the thread when the part is a fatigue-critical fastener and the volume is high enough to justify a die head. If the thread sits next to a shoulder or the material is titanium or Inconel, mill it instead of tapping.
Questions engineers ask about threaded parts
Can you hold a 4H thread class on a small aluminum part?
Yes, but the part has to be rigid enough to cut without deflection. On small aluminum threads we take lighter passes and gauge the pitch diameter during the run. A 4H class is a tighter pitch diameter band than 6H, so tool wear has to be watched more closely.
If the part is a thin wall or has a long overhang, we will usually recommend 6H and a controlled minor diameter instead. That gives the same assembly result without the scrap risk.
Why does my stainless thread gall during assembly?
Gall is a material problem, not a size problem. 304 and 316L can cold-weld to a mating stainless screw under load. The thread surfaces are too similar and the oxide layer breaks down.
Two fixes work. Use a different alloy on one side, such as a 316 screw into a 303 nut, or specify a dry-film lubricant on the thread. A slightly looser class also helps.
What surface finish should I specify on a thread?
For most fasteners, Ra 1.6–3.2 μm on the flanks is fine and keeps the cost down. A smoother finish is only needed when the thread has to seal, as in a pipe thread or a hydraulic fitting.
We can reach Ra 0.8–1.6 μm on the flanks when the drawing calls for it. Going below Ra 0.8 μm on a thread rarely helps and adds cycle time.
Do you cut left-hand threads and non-standard pitches?
Yes. Left-hand threads, UNEF, UNF, BSP, and metric fine pitches are all cut from the drawing. There is no tooling cost for a left-hand thread on a single-point operation.
For a rolled thread, a non-standard pitch needs a die head or roll set, so it only makes sense at volume.
How do you check a thread on a part that cannot go on a gauge?
We use thread milling with a single-point tool and measure the pitch diameter with a thread micrometer or a three-wire setup. For internal threads, we use a thread analyzer when the geometry allows.
On very small or very deep threads, we cut a sample and section it. The cross-section shows the flank angle and the root radius directly.
What is the smallest thread you can produce?
M1.6 is practical on a rigid setup in brass or aluminum. Below that, tap breakage and gauge availability become the limit, not the machine.
If you need a very small thread, tell us the material and the engagement length. We will say whether it is a cutting job or whether a different fastening method is the better call.
Send us the thread, not a description of it
Upload the drawing and we will return a quote with DFM notes on the thread within 12 hours. No minimum order quantity, from one prototype to a 10,000-part run.
12-hour quoteNo MOQ±0.005 mm100% inspection
More CNC screw processing notes
We publish setup notes, tooling trials and inspection data from the factory floor.
