CNC threading is the operation that most often decides whether an assembly line runs or stops. It looks trivial on a drawing — a leader line, an M4, a depth — yet one bad internal thread can scrap an audio chassis that has already been milled and anodized. This guide covers CNC threading from the process-selection side: tapping vs thread milling, internal thread machining in blind holes and hard alloys, and what to put on your drawing.
Key takeaways
- Tapping is the default for high-volume holes in free-cutting materials.
- Thread milling costs more per hole but removes the broken-tap risk.
- Blind hole tapping defects are caused by chips, not geometry.
- Thread class (6H/6g, 2B/2A) is a tolerance band, not a quality grade.
- Always dimension thread depth, not just hole depth.
What CNC threading covers
CNC threading produces a helical form on a part: internal threads in a pilot hole, external threads on a shaft, or rolled threads with no cutting. This guide focuses on internal thread machining, where the process choice is contested — external threads are usually single-pointed on a lathe, which our CNC turning service guide covers.
Tapping drives a multi-tooth tool along the hole axis; thread milling interpolates a cutter around the hole wall. Both meet the same standard; they differ in what happens when something goes wrong.
Tapping vs thread milling: the core decision
How tapping works
A tap is a form tool: its teeth match the finished profile, so the machine only has to feed it in straight, one revolution per pitch. Cutting taps make chips; forming taps displace material, giving a work-hardened thread but needing a larger pilot hole and ductile material.
The weakness is mechanical: the tool is loaded in torsion at the bottom of a hole, and if it binds, it shears. Removing a broken tap from hardened stainless can cost more than the part.
How thread milling works
A thread mill carries the profile ground along its flutes. The machine drills the pilot, then runs a helical pass — one turn around the hole while descending exactly one pitch. The cutter is smaller than the hole, so chips have somewhere to go and radial load drops.
So one cutter threads any diameter of the same pitch, depth is set by the program, and a broken cutter is easy to extract. The cost is cycle time: thread milling runs several times slower than tapping.
Tapping vs thread milling: side-by-side
| Factor | Tapping | Thread milling |
|---|---|---|
| Hole size | M1.6–M24, best under M12 | M3 upward, practical to M50 plus |
| Materials | Best in aluminum, brass, free-cutting steel | Stainless, titanium, hardened steel |
| Precision and class | Class built into the tap | Class set in the program; wear is compensated |
| Cost per hole | Lowest tool and cycle cost | Higher, one tool covers a whole pitch |
| Cycle time | Fastest — often seconds per hole | Slower, typically 3–5x tapping |
| Broken tool risk | Tap can shear in the hole; may scrap the part | Rarely breaks; extraction usually simple |
| Blind hole performance | Needs a bottoming tap plus chip clearance | Excellent — chips evacuate, depth set by code |
| Best fit | High volume, small holes, soft materials | Large holes, hard materials, high part value |
Read that as a risk decision, not a cost-per-hole decision: thread milling wins when the cost of one scrapped part exceeds the cycle penalty across the batch. Weighing this on a live part? Send the drawing and we will recommend a process per feature — start at our contact form.
Common thread standards and callouts
ISO metric threads
The metric profile is defined by ISO 68-1, with ISO 261 and ISO 262 covering the diameter-pitch combinations in general use. Tolerances come from ISO 965, where 6H and 6g live. A complete callout reads M8 x 1.25 – 6H: diameter, pitch, internal tolerance class. Omitting the pitch implies coarse — a common source of taps ordered wrong, so write it out.
Unified threads (UNC / UNF)
Unified is the North American standard under ASME B1.1: UNC is coarse, UNF is fine. Classes 2A/2B are the general-purpose fit; 3A/3B are tighter. A full callout reads 1/4-20 UNC-2B — size, threads per inch, series, class. Keep one system per drawing; mixing metric and Unified is an assembly-floor hazard.
Thread class and fit
Thread class is a tolerance band, not a badge of quality. 6H internal / 6g external is the standard metric pairing; 2B / 2A is the Unified equivalent. Tightening to 5H or 3B raises cost with no functional gain unless you are dealing with vibration, sealing or precision adjustment.
Practical rules for internal thread machining
Blind hole tapping and chip control
Blind hole tapping causes most CNC tapped-hole defects, and the mechanism is almost always chips: a cutting tap pushes swarf into a closed hole, it packs, torque spikes, and the tap breaks.
- Specify thread depth, then let the shop drill the pilot deeper — a pilot at full thread depth packs the bottom.
- Match the tap to the hole (spiral flute or bottoming), and use through-tool coolant in gummy materials such as 6061 and 304.
- For blind holes deeper than about 3x diameter, use a forming tap or thread milling.
Pilot hole size and wall thickness
Pilot diameter sets thread percentage. Around 75% engagement is standard; pushing to 100% roughly doubles tapping torque while adding almost no pull-out strength. Wall thickness matters too — a hole too close to an edge distorts during tapping, especially in thin-wall aluminum enclosures. Flag threaded bosses near edges; our DFM analysis guide covers that conversation.
What to put on the drawing: 6 items
A callout missing any of these generates a clarifying email, and each one costs a day:
- Thread designation with pitch — M6 x 1 or 1/4-20 UNC. Never leave pitch implied.
- Tolerance class — 6H, 6g, 2B, 2A. State it, or accept the shop default.
- Thread depth, not hole depth — minimum full-thread depth, dimensioned separately from drill depth.
- Hand and number of starts — right-hand single-start is the default; anything else must be explicit.
- Coating condition — whether the class applies before or after anodizing, plating or coating.
- Criticality — which holes are mating-critical, and whether a broken-tap repair is acceptable.
Material choice interacts with every item above; our CNC machining materials guide and aluminum CNC machining guide cover how alloy selection changes thread behavior.
Inspecting CNC tapped holes
Thread inspection is pass or fail, not measurement. The standard tool is a go/no-go thread gauge: the go end must thread in fully by hand, and the no-go end must not enter beyond about two turns — which is what thread class is really about.
A plug gauge says nothing about torque or pull-out strength, so high-value applications add a torque test. Hole position and pilot diameter are verified on a CMM — see our CNC inspection methods and CMM guide — and threads belong in the first article inspection report.
Conclusion
CNC threading is a process choice before it is a tooling choice. Tapping gives the lowest cost per hole and the fastest cycle, and is right for most small holes in aluminum and brass at volume. Thread milling trades cycle time for chip evacuation, blind-hole accuracy and near-total removal of the broken-tap failure mode.
The rest sits on the drawing: an implied pitch, a missing class, a depth that describes the drill instead of the thread. Six clear lines remove most of it.
At Ruijin Fenghui Precision Technology in Dongguan, we machine internal threads for audio equipment, drone, automotive, medical, robotics and 3C parts, with more than 23 years of experience and over 200 CNC machines under IATF 16949, ISO 9001 and ISO 13485. ±0.01mm is our standard working tolerance.
Send a STEP file and a 2D drawing and we will tell you which holes should be tapped, which should be thread milled, and what your callout is missing — quote within 24 hours, prototypes in 3 to 7 days. Start at our contact form.
New to the process? Our CNC machining guide covers the fundamentals, and the CNC machining tolerance guide shows where thread classes sit in your tolerance scheme.
CNC threading FAQ
What is the difference between tapping and thread milling?
Tapping drives a form tool into a pilot hole in one pass, with the thread profile built into the tap. Thread milling interpolates a cutter around the hole wall in a helical path, with the profile generated by the tool path. Tapping is faster and cheaper per hole; thread milling is safer on hard materials, blind holes and expensive parts.
When should I choose thread milling over tapping?
Choose thread milling for holes above roughly M12, for stainless, titanium or hardened alloys, for deep blind holes where chips would pack, for thin walls that deflect, or whenever the part is valuable enough that a broken tap would be expensive. The slower cycle time is usually cheaper than the scrap risk.
What thread class should I specify for CNC tapped holes?
Specify 6H for internal metric threads and 6g for external, or 2B and 2A for Unified UNC and UNF threads. That pairing covers the vast majority of assemblies and is what standard gauges are stocked for. Only tighten to 5H or 3B where vibration, sealing or precision adjustment genuinely requires it, since tighter classes need better tooling and slower inspection.
How are internal threads inspected on the shop floor?
Internal threads are checked with a go/no-go thread plug gauge. The go end must enter the full thread depth by hand, and the no-go end must not pass beyond about two turns. Position and pilot diameter are verified separately on a CMM, and thread features appear in the first article inspection report.