§01 Anatomy of a thread callout
A complete thread callout on a drawing looks like one of these:
M6 × 1.0 - 6H ↓ 12
or, in unified (imperial) form:
1/4 - 20 UNC - 2B ↓ .500
Every element of the callout answers a specific question:
| Element | Meaning | Example (M6) |
|---|
| Designation | Standard family — M for ISO metric, UNC/UNF for Unified | M |
| Major diameter | Outer diameter of the thread (in mm or inches) | 6 mm |
| Pitch | Distance between adjacent thread peaks (mm), or threads-per-inch (TPI) | 1.0 mm |
| Tolerance class | Fit quality — 6H/6G for metric internal, 2B/3B for unified internal | 6H |
| Depth (↓) | Thread depth measured from the top face, NOT the drill depth | ↓ 12 |
§02 Metric vs unified — which to use
If your part is going into a machine assembled anywhere outside North America, use metric. Metric threads (M-series) are the global industrial default and every fastener in Europe, Asia, and most of South America is metric. Unified (UNC/UNF) is still dominant in US aerospace, US military, and US consumer products. Don't mix the two on one part — a drawing with both metric and unified threaded holes is a guaranteed source of assembly errors.
Practical rule: If the mating fastener is being bought in the US aerospace supply chain, use unified. For everything else, use metric. Never convert a unified thread to its closest metric equivalent in hopes of "standardizing" — the pitches are different, threads don't interchange even if diameters look similar.
§03 Tap drill reference
The tap drill is the drill diameter that creates the hole before tapping. It must be smaller than the thread's major diameter so that material remains for the tap to cut the thread form. Using the wrong tap drill is the #1 cause of broken taps.
Metric coarse (most common)
| Thread | Pitch | Tap drill Ø | Clearance drill Ø |
|---|
| M2 | 0.4 mm | 1.6 mm | 2.4 mm |
| M2.5 | 0.45 mm | 2.05 mm | 2.9 mm |
| M3 | 0.5 mm | 2.5 mm | 3.4 mm |
| M4 | 0.7 mm | 3.3 mm | 4.5 mm |
| M5 | 0.8 mm | 4.2 mm | 5.5 mm |
| M6 | 1.0 mm | 5.0 mm | 6.6 mm |
| M8 | 1.25 mm | 6.8 mm | 9.0 mm |
| M10 | 1.5 mm | 8.5 mm | 11.0 mm |
| M12 | 1.75 mm | 10.2 mm | 13.5 mm |
| M16 | 2.0 mm | 14.0 mm | 17.5 mm |
| M20 | 2.5 mm | 17.5 mm | 22.0 mm |
Unified coarse (UNC)
| Thread | Pitch (TPI) | Tap drill | Clearance drill |
|---|
| #4-40 | 40 | #43 (0.089") | #32 (0.116") |
| #6-32 | 32 | #36 (0.1065") | #27 (0.144") |
| #8-32 | 32 | #29 (0.136") | #18 (0.1695") |
| #10-24 | 24 | #25 (0.1495") | #9 (0.196") |
| #10-32 | 32 | #21 (0.159") | #9 (0.196") |
| 1/4-20 | 20 | #7 (0.201") | F (0.257") |
| 5/16-18 | 18 | F (0.257") | P (0.323") |
| 3/8-16 | 16 | 5/16" (0.3125") | W (0.386") |
| 1/2-13 | 13 | 27/64" (0.4219") | 33/64" (0.5156") |
§04 Three rules for thread depth
Rule 1 — Thread depth is not drill depth
If you write M6 ↓ 12, the drilled hole must go deeper than 12 mm — typically 3 mm deeper for manual tapping or 1.5×pitch for power tapping. The tap needs somewhere for chips to evacuate. A drill that stops exactly at thread depth creates a thread that's only usable for half its nominal depth because the bottom threads are partial.
Rule 2 — Thread depth ≤ 2× diameter
There's a myth that deeper threads are stronger. In fact, any thread engagement beyond 2× the diameter adds essentially zero pullout strength — by that depth, the fastener shank fails before the thread strips. Specifying M6 ↓ 30 just wastes cycle time and risks tap breakage from chip buildup.
Rule 3 — Minimum 1× diameter in soft metals, 1.5× in steel
For thread engagement in aluminum, brass, or plastic, use at least 1× diameter. In steel or titanium, use at least 1.5× diameter. Below these minimums the thread strips before the fastener yields.
Summary formula: For M6 in aluminum — drill depth = 15 mm, thread depth = 12 mm. The 3 mm difference is chip-evacuation space.
§05 The five most common thread callout mistakes
Specifying non-standard thread sizes (M5.5, 7/32-24)
Every non-standard thread requires a special tap (~$80-200) and the machine shop must stock it. For a prototype run, this adds significant cost and delay. Always pick from the standard sizes listed in the tables above. Non-standard sizes should only appear on parts that must mate with legacy hardware.
Forgetting the thread depth
A callout like M6 without depth leaves the machinist guessing. The default assumption is "through" for plates under 10 mm, or "1.5× diameter" for thicker parts — but this is a guess. Always specify depth, written with the downarrow: M6 ↓ 12 means "threaded 12 mm deep".
Mixing metric and unified on one part
A drawing with M6 threads on one face and 1/4-20 threads on another is an assembly disaster waiting to happen. Fasteners look similar but don't interchange. Unless you have a very specific reason (e.g., mating to a legacy US military assembly), pick one system for the whole part.
Specifying a tolerance class that isn't needed
6H is the default internal metric thread tolerance and works for 99% of applications. 6G is slightly looser (for plated parts). Only specify 4H or 5H for precision instrumentation, and only specify 7H for high-temperature service. Over-tight tolerance classes require special thread gauges during inspection — cost adder with no functional benefit.
Threading too close to an edge
Threads placed closer than 1.5× diameter from a part edge are likely to blow out the sidewall during tapping. For a blind M6 hole, keep the hole center at least 9 mm from any edge. If closer placement is required, specify a HeliCoil or threaded insert instead of a direct tap.
§06 Thread standards — ISO, ANSI, UTS, and when each applies
Machine threads come in several parallel standards that don't interchange. The world splits roughly into metric (ISO) and inch (UNS) systems, with regional variations:
| Standard | Region | Common applications |
|---|
| ISO 68-1 / ISO 724 / ISO 965 | Global (metric default) | Most international mechanical products |
| ANSI B1.1 (Unified Inch Screw Thread, UNC/UNF) | USA, Canada | Legacy US designs, aerospace, military |
| BSW / BSF (British Standard Whitworth / Fine) | UK (legacy) | Old British equipment, restoration work |
| JIS (Japanese Industrial Standards) | Japan | Japanese automotive, industrial equipment |
| DIN (Deutsches Institut für Normung) | Germany (largely aligned with ISO) | German machine tools, European heavy industry |
A metric M6×1.0 and a UNS 1/4-20 UNC are similar sizes but not interchangeable. Even a metric M6×1.0 and an M6×0.75 (fine pitch) aren't interchangeable — same diameter, different pitch, different threads. Specifying the wrong standard in an international supply chain is a common cause of rejected first articles.
§07 Pipe threads — a different animal
Pipe threads are designed to seal against leakage, not just transmit torque. They use tapered geometry that wedges tight as it's tightened. The major standards:
| Standard | Name | Type | Use case |
|---|
| NPT | National Pipe Tapered | Tapered (1:16) | USA plumbing, fuel, hydraulics |
| NPTF | National Pipe Tapered Fuel | Tapered, dry-seal | High-pressure, no sealant allowed |
| BSPT (G/R) | British Standard Pipe Tapered | Tapered (1:16) | UK, EU, Asia plumbing |
| BSPP (G) | British Standard Pipe Parallel | Parallel + O-ring | Hydraulic, pneumatic fittings |
| JIS B0203/B0202 | Japanese pipe standards | Tapered / Parallel | Japanese hydraulics |
The gotcha: NPT and BSPT are not interchangeable despite looking similar. Both are 1:16 taper, but they have different thread profiles (55° vs 60° angle) and different pitch. Forcing them together either leaks or strips the threads. For equipment that will be used internationally, either specify one standard consistently or use adapter fittings at the boundary.
§08 Anatomy of a proper thread callout
A complete thread callout on a drawing includes everything a machinist needs to produce the right thread without asking. Minimum information:
| Element | Example | What it specifies |
|---|
| Standard | M (metric) or - (inch) | Which thread system |
| Major diameter | 6, 8, 1/4, 3/8 | Nominal thread size |
| Pitch | ×1.0 (metric), -20 (inch TPI) | Coarseness — essential because multiple pitches exist per diameter |
| Tolerance class | 6H/6G (metric), 2B/3B (inch) | Fit quality between mating threads |
| Length (blind holes) | THRU, 15 deep, or DEPTH 15 | How deep the thread runs |
| Internal vs external | Implicit from hole vs shaft context, or noted | Which side of the mating pair |
| Class of fit | 6H (internal) / 6g (external) for metric; 2B / 2A for inch | Fit quality — 6H/6g is the default general-purpose pairing |
A proper internal metric thread callout looks like: M8×1.25 — 6H, DEPTH 20. This says: M8 (8mm nominal), 1.25mm pitch (coarse), 6H tolerance class (standard), 20mm thread depth in the hole. For an inch equivalent: 1/4-20 UNC-2B × 0.75 DP.
Callouts that cause rejection: M8 thread (no pitch specified), tapped 1/4-20 (no class, no depth), tap 6mm deep (no pitch, no class, no thread engagement spec). Each of these requires the shop to either guess or delay production to ask.
§09 Thread tolerance classes — what they mean
Thread fit determines how the mating parts assemble — loose, tight, or precision:
| Metric | Inch | Fit | Typical use |
|---|
| 6H internal + 6g external | 2B + 2A | General purpose, slight clearance | Default for 90% of assemblies |
| 6H internal + 6h external | 3B + 3A | Closer fit, less wobble | Precision alignment, safety-critical |
| 7H internal + 8g external | 1B + 1A | Loose fit, easy assembly | High-tolerance or dirty-thread applications |
| 6G internal + 6h external | 3B + 2A | Interference fit | Where looseness causes problems |
On most drawings, specifying 6H (internal) or 6g (external) is sufficient — it's the default understood by any competent machinist. Call out tighter classes (4H, 5H) only when the mechanical requirement justifies the cost, which is typically 50-100% more in inspection alone. Call out looser classes (7H, 8H) when you need easier assembly or tolerance for contamination.
§10 Thread-related cost traps
Threads are cheap individually but expensive cumulatively. Patterns that inflate cost:
01
Mixed metric + inch on the same part
A drawing with some M6 and some 1/4-20 threads forces the shop to swap tooling mid-cycle. Each tool change is 30-60 seconds. On a part with 20 threaded holes split between standards, you've added 10-20 minutes per part. Pick one system and stick with it.
02
Fine-pitch threads without justification
M8×1.0 (fine) requires a different tap than M8×1.25 (coarse). Fine-pitch threads are harder to tap — more tool breakage, slower cycle, sometimes require thread mills instead of taps. Use coarse pitch unless you have a real reason (vibration resistance, adjustment precision).
03
Threads in hard material without pre-drill allowance
Tapping 4140 at 32 HRC is possible but tool-expensive. Tapping the same feature before heat-treatment, then heat-treating, is often cheaper and more reliable. Alternatively, use a HeliCoil or other thread insert in the hardened part — the insert is replaceable, the hardened part is not.
04
Excessive thread depth
Most bolted joints only engage 1-1.5× diameter of thread. Specifying "tap through" on a 25mm-thick part wastes 15mm of tap travel on threads nobody uses. Specify the needed engagement depth and allow excess hole depth without threads.
05
Custom thread pitches or inch-metric hybrids
Anything outside standard ISO or UNS callouts requires custom tooling or thread milling. We've seen drawings with "M6×0.8" (non-standard pitch) that required special-order taps and 2 weeks additional lead time. Always use standard pitches unless a specific reason demands otherwise.
§11 Thread inserts as a cost strategy
For threads in aluminum, plastic, or any repeated-use hole, pressed-in inserts often cost less over the part's life than machined threads:
| Insert type | Best for | Cost | Strength vs machined thread |
|---|
| HeliCoil (wire coil) | Aluminum; medium strength; repair | $0.30-1.50 per hole | 110-130% of tapped aluminum |
| Keensert / solid insert | High strength in aluminum | $1.50-4.00 per hole | 200-300% of tapped aluminum |
| Press-in threaded insert (plastic) | Plastic parts | $0.50-2.00 per hole | 200-400% of tapped plastic |
| Rivnut (blind insert) | Sheet metal, one-side access | $0.20-0.80 per hole | Depends on sheet thickness |
Key decision factors:
- Frequent assembly/disassembly (maintenance access) → insert almost always
- One-time assembly → direct tap is cheaper
- High load per fastener → insert (especially in aluminum <6mm engagement)
- Plastic parts → insert almost always (threads in plastic strip easily)
§12 Threads on drawings — callout examples
Examples of properly-specified thread callouts, good and bad:
Bad: 3x M6 tapped — no pitch, no class, no depth. Requires clarification before quoting.
Better: 3x M6×1.0 - 6H, ↓ 12 — complete callout. Shop knows pitch (1.0mm coarse), fit class (6H default), and depth (12mm).
Best (with drill specification): 3x M6×1.0 - 6H ↓12 / Ø5.0 ↓15 — also specifies drill size (Ø5.0, standard for M6×1.0) and drill depth (15mm, allowing 3mm of unthreaded hole bottom for chip clearance). This eliminates any shop ambiguity about how to produce the feature.
Production-ready with inspection: 3x M6×1.0 - 6H ↓12 min · Go/No-Go verified — explicitly specifies inspection method. For regulated applications, include the specific gauge used: "GO gauge: standard 6H, NO-GO gauge: 7H per ISO 1502."
§13 Common thread-callout questions
Do I always need to specify tolerance class on threads?
No — if your drawing has a general note "All threads: 6H internal / 6g external per ISO 965-1" in the title block, you don't need to repeat the class on each callout. Only call out deviations (tighter or looser) from the default.
What's the difference between 2A/2B and 6g/6H?
2A/2B is the inch standard (ANSI B1.1); 6g/6H is the metric standard (ISO 965-1). The precision levels are comparable — both are "general purpose" default fits. Don't mix them on the same drawing.
Can I specify threads with standard deep-engagement callouts?
Yes — use "2D engagement" (2× diameter of thread engagement) as a general rule. For M6 that's 12mm of thread engagement. Some applications want 1.5D (for short bolted joints), others 3D (for high-vibration or high-load). Specify explicitly when deviating from 2D.
What about left-hand threads?
Rare but necessary for some counter-rotating shafts, bicycle pedals, propane fittings. Callout adds "LH" or "-LH": "M12×1.75 LH - 6H". Always clearly identify on drawing and add a note — left-hand threads are unusual enough that it's easy to cut right-hand by mistake.
Do I need tap depth on through holes?
No — through holes are obvious. For blind holes, always specify depth: "↓ 12" means thread to depth 12mm. Include separate drill depth if different from tap depth — chips need somewhere to go at the bottom.