Threads & Holes Design Guide
Metric vs UN threads, thread classes, blind hole depth, engagement and tap drills
Threads are among the most-specified and most-often-failed features in machined parts. The designer chooses a thread standard (ISO metric or ASME unified), a tolerance class, a minimum engagement length and — for blind holes — a drill-point depth. Each choice affects machinability, assembly strength and quoting cost.
1. Thread standards
ISO metric threads (ISO 965-1) are designated M6 × 1.0 — nominal diameter and pitch; unified threads (ASME B1.1) use #/UNC/UNF, e.g. 1/4-20 UNC. Metric coarse is the default for new designs; UNF/fine pitches hold better under vibration but need sharper taps.
Tolerance classes: 6H is the standard internal (tapped hole) class, 6g for external (screw); 5H/4h for precision fits, 7H/8g for loose fits with coatings. Class designations appear on the drawing as M6×1.0-6H.
2. Engagement and strength
Minimum thread engagement is 1.5× the nominal diameter in aluminum and softer materials, 1.0× in steel; longer engagement does not add strength because the bolt usually fails first. Shear-out and stripping are prevented by correct engagement plus proper tap drill size (about 75% thread depth standard).
Formed threads (thread milling, rolling) can strengthen fatigue life vs cut threads; for production, thread rolling is preferred where vibration or dynamic load matters.
3. Blind holes
A blind tapped hole must accommodate the tap drill point: total drilled depth = thread length + 3–4 pitches + drill-point allowance (~0.3× drill diameter). Under-specifying depth is the most common thread error — the tap bottoms out, breaks, or the part is scrapped.
Prefer through-holes where the design allows: they are cheaper, vent no trapped air, and tolerate misalignment better. For sealed assemblies use pipe threads (NPT/BSP, ASME B1.20.1 / ISO 228) and call the class explicitly.
4. Specification on drawings
Specify: thread standard + size + pitch + class + depth + location tolerance (true position at MMC is standard practice). Example: “M5 × 0.8 – 6H, depth 12 mm min, true position ⌀0.1(M) A B C.”
The platform recommends standard sizes (M1.6–M24 metric, #2–1″ unified) and flags non-standard threads for manual review — custom pitches and left-hand threads require special taps and raise cost.
Quick reference
| Thread | Standard | Class (hole) | Engagement | Blind depth rule |
|---|---|---|---|---|
| M6 × 1.0 | ISO 965-1 | 6H | 9 mm (1.5×d, aluminum) | thread length + 3–4 pitches + drill point |
| 1/4-20 UNC | ASME B1.1 | 2B | ~10 mm (1.5×d) | same rule; add tap drill allowance |
| M3 × 0.5 | ISO 965-1 | 6H | 4.5–6 mm | min tap drill depth ≈ thread + 2 mm + point |
| NPT 1/8-27 | ASME B1.20.1 | NPT | pipe standard | taper hole per standard |
Sources & references
- ISO 965-1 — ISO general purpose metric screw threads
- ASME B1.1 — Unified Inch Screw Threads
- ASME B1.20.1 — Pipe Threads
- Xometry Learning Center — Threads Guide (public engineering reference)