Thread callouts are one of the most misread features on CNC drawings — partly because there are two major standards (metric and unified), partly because the callout itself packs four separate pieces of information into one line. This page explains the anatomy of each callout, gives you a tap-drill lookup table, and shows the three thread-depth rules that keep tool breakage out of your quote.
A complete thread callout on a drawing looks like one of these:
or, in unified (imperial) form:
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 |
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.
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.
| 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 |
| 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") |
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.
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.
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.
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.
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".
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.
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.
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.
Every quote includes a DFM review by a mechanical engineer. Non-standard thread sizes, over-tight tolerances, and edge-proximity issues all get flagged before the part goes to the floor.