Designing Internal Threads and Tapped Holes for CNC Machining

Threads are where precision parts quietly fail: a tapped hole strips during assembly, a thread gauge won't go, or a coating made a "perfect" thread impossible to bolt. Internal threads are also one of the last features cut, so a design error surfaces at the end of the process — exactly when it costs the most. Here is how we design, machine and inspect internal threads in CNC machining, and the choices that keep them trouble-free.

Start With the Thread Family

ISO metric (M) is the global default: the pitch in millimetres follows the diameter (M4×0.7, M6×1.0, M8×1.25…). Unified inch (UNC/UNF) persists in North American equipment and aviation (1/4-20, 1/4-28…). Pipe threads (NPT, Rp/BSPP) seal on tapered or parallel flanks for fluid lines. For new designs, metric coarse is the sensible default — strongest, easiest to tap, most forgiving of coating thickness. Fine pitches buy clamping security on thin walls and vibration resistance, at the cost of more fragile taps and tighter tolerance to misalignment.

The Minimum-Depth Rules That Actually Matter

Stripping happens at the first two or three engaged threads, not the last. That fact drives every rule below:

• Engagement in steel/aluminium: 1.0–1.5× diameter in steel, 2–2.5× in aluminium (its softer threads shear earlier). More depth adds cost and tap-breakage risk without adding strength.
• Blind-hole geometry: tapped depth should be full engagement plus 2–3 threads of incomplete lead-in; drill depth then adds another 0.5–1× diameter of chip clearance below the tap's taper. A drawing that says "M6×16 deep, drill 25 deep" tells us everything at a glance.
• Bottoming out: leave at least 2 pitches of unthreaded hole below the last full thread, or specify a form (roll) tap whose chips don't need a relief pocket.
• Through holes win: whenever the design allows, let the tap exit. Through-tapping is faster, cleaner and self-clearing — the single cheapest thread decision you can make.

Cutting vs Forming Taps — and Thread Milling

Three production routes reach the same thread:

Method	Best for	Watch-outs
Cut tapping	General work, most sizes	Chip evacuation in blind holes; breakage in hard or stringy alloys
Form (roll) tapping	Ductile materials: aluminium, brass, mild steel	Needs a larger pre-hole (≈ pitch × 0.55 of the cut-tap drill); no chips, stronger threads
Thread milling	Hardened stock, large bores, interrupted or off-centre threads, tight runout	CNC required; smaller risk of broken tools; one tool covers many pitches

Thread milling deserves a second look for anything above M6: the tool enters and exits on a helical path, so a snapped tap can't scrap the part, and it can hold genuine runout-to-datum control that tapping never will. On turning work, small brass and aluminium fittings usually roll-form — the cold-worked threads are measurably stronger than cut ones.

Pre-Hole Sizes: Why the Drawing Number Matters

Tap-drill charts assume 75% thread engagement, but the real decision is the balance between stripping torque (too little material) and tapping torque (too much). Practical numbers we machine to: 75% for diameters up to about M6, 65–70% for larger threads where tap torque becomes the failure mode, and 60–65% in tough alloys such as titanium or 316 stainless. If a threaded hole has ever "cracked taps for no reason", the pre-hole was the usual suspect.

Coatings and Plating Change Threads

Anodising, galvanising and plating build thickness on flanks. A 0.01 mm coating on both faces of an M4 thread eats a quarter of its flank clearance. The standard fixes, which we apply daily through our surface treatment services:

• Mask threads before anodising or powder coating.
• Specify plated threads pre-plated oversize (2B/3B equivalents) so the finished thread lands on gauge.
• For hard anodising on aluminium housings, design threaded inserts (Helicoil or press-in) instead of tapping before coating — see Anodizing vs Powder Coating for how film builds differ.

Inspection: How Threads Are Actually Verified

Production thread checks are functional, not dimensional: GO/NO-GO plug gauges prove the thread assembles and doesn't over-fit, per the philosophy in our quality control guide. Depth of thread is verified by gauge notch or CMM. If the drawing needs true position on threaded features, we tolerance the pilot hole and note the gauge-based verification — the approach recommended in our GD&T guide.

Frequently Asked Questions

How deep should a blind tapped hole be for an M6 screw, 20 mm long?

Thread about 24–25 mm (engagement plus lead-in), drill roughly 32 mm. The extra below-tap clearance is what keeps chips from packing and taps from bottoming.

Why won't my bolt go in after anodising?

The coating grew into the thread. Either mask the thread, specify oversize tapping before coating, or add a wire insert after coating — send us the finish spec early and we plan for it.

Can you repair a stripped thread in a machined part?

Often yes: Helicoil or Time-Sert inserts restore the original strength and usually exceed it. Designing the insert in from the start is cheaper than retrofitting one.

Which is stronger, rolled or cut threads?

Rolled — cold work strengthens the flank material by 10–30% and leaves a smoother surface. In ductile materials we roll-form wherever volume and geometry allow.

Related Reading

• GD&T Symbols Explained for CNC Machining Drawings
• A Practical Guide to CNC Machining Tolerances
• CNC Turning vs CNC Milling: Which Does Your Part Need?
• Brass vs Copper: Which Metal for Your CNC Parts?

Threaded features in your next part? Send the drawing to sales@nbrjmetal.com — we will confirm depths, pre-holes and coating strategy before quoting, so nothing surprises you at assembly.