Category
Send your part number — quotes typically within hours.
WhatsAppMon–Sat · 9:00–18:00 GMT+8
Why Hooguu Tools
- 📦250,000+ SKUs in stock
- 🏷️50+ brands, all genuine OEM
- ✈️Worldwide via DHL/FedEx
- ↩️30-day money-back
Tapped holes are among the highest-risk operations on a CNC machining center, and most tap failures trace back to one parameter: the pilot hole diameter. A hole that is 0.05–0.10 mm too small can double tapping torque; a hole that is too large strips the thread class and scrapes out of tolerance on the go gauge. This reference consolidates the tap drill charts that production shops use daily — ISO metric coarse and fine, UNC/UNF inch threads, NPT and BSPP pipe threads — together with the engagement formulas behind them, roll-form tap pilot holes, tapping speeds and a diagnosis table for the most common thread problems.
Why 75 Percent Thread Engagement Is the Shop Standard
Thread engagement describes how much of the theoretical full thread profile the tap actually cuts, and it is controlled entirely by the pilot hole diameter. The smaller the hole, the more material the tap must remove, and tapping torque rises almost linearly with engagement while thread strength flattens out well before 100 percent. Testing on medium-carbon steel consistently shows that a 75 percent engagement thread carries roughly 90 percent of the load capacity of a theoretical 100 percent thread, while requiring far less torque and generating far less heat in the tap.
That is why virtually every tap manufacturer, including OSG and YG-1, publishes chart values based on the 75 percent convention. Use 65 percent engagement for materials that tap hard — austenitic stainless steels, titanium, Inconel — and for deep blind holes where chip packing is the dominant failure mode. Values above 85 percent are rarely justified outside thin nut applications and galling-prone fits.
The engagement-controlled tap drill diameter follows this formula (any consistent unit):
Tap drill = D − 1.299 × (% engagement / 100) × P
where D is the major diameter and P is the thread pitch. For metric threads the practical shortcuts are 75%: TD ≈ D − 0.97 × P and 65%: TD ≈ D − 0.84 × P.
| Engagement | Relative thread strength | Relative tapping torque | Typical use |
|---|---|---|---|
| 60% | ~78% | ~55 | Titanium, deep blind holes > 3×D |
| 65% | ~84% | ~65 | Stainless, Inconel, gummy low-carbon steel |
| 70% | ~88% | ~80 | General purpose on tough materials |
| 75% | ~92% | 100 | Industry standard, all materials |
| 85% | ~97% | ~130 | Short, high-load fits only |
| 100% | 100% | >200 | Theoretical profile, not practical |
Torque and strength values are relative to the 75% baseline; exact figures vary with material and tap geometry.
ISO Metric Coarse Thread Tap Drill Chart (75% Engagement)
Values below follow the formula above and match the chart data published by OSG, YG-1 and other major tap makers. Where the computed value falls between standard drill sizes, choose the nearest available drill and verify the thread class with a go/no-go gauge on the first article.
| Thread | Pitch (mm) | 75% drill (mm) | 65% drill (mm) | Minor dia. limit ≈ (mm) |
|---|---|---|---|---|
| M3 × 0.5 | 0.5 | 2.5 | 2.6 | 2.46 |
| M4 × 0.7 | 0.7 | 3.3 | 3.4 | 3.24 |
| M5 × 0.8 | 0.8 | 4.2 | 4.3 | 4.13 |
| M6 × 1.0 | 1.0 | 5.0 | 5.2 | 4.92 |
| M8 × 1.25 | 1.25 | 6.8 | 7.0 | 6.65 |
| M10 × 1.5 | 1.5 | 8.5 | 8.7 | 8.31 |
| M12 × 1.75 | 1.75 | 10.2 | 10.5 | 10.03 |
| M14 × 2.0 | 2.0 | 12.0 | 12.3 | 11.84 |
| M16 × 2.0 | 2.0 | 14.0 | 14.3 | 13.84 |
| M20 × 2.5 | 2.5 | 17.5 | 17.9 | 17.29 |
| M24 × 3.0 | 3.0 | 21.0 | 21.5 | 20.75 |
ISO Metric Fine Pitch Examples
Fine pitches are common on machine elements, hydraulic fittings and adjusting screws. The same formula applies; the drill simply moves closer to the major diameter as pitch decreases.
| Thread | Pitch (mm) | 75% drill (mm) |
|---|---|---|
| M6 × 0.75 | 0.75 | 5.25 |
| M8 × 1.0 | 1.0 | 7.0 |
| M10 × 1.25 | 1.25 | 8.8 |
| M12 × 1.5 | 1.5 | 10.5 |
| M12 × 1.25 | 1.25 | 10.8 |
| M16 × 1.5 | 1.5 | 14.5 |
| M20 × 2.0 | 2.0 | 18.0 |
Note on thread class: a standard twist drill leaves the pilot hole slightly oversize with a tolerance of roughly +0.05/+0.15 mm depending on diameter and drill condition. For drawing-specified 6H class in tough alloys — or for threads that will be gauged 100 percent — ream the pilot hole to the 75% value minus one pitch-diameter tolerance band, or use a dedicated tap-and-ream workflow on the machining center.
Inch Threads: UNC and UNF Tap Drill Sizes
For unified threads the same 1.299 formula governs; the chart below gives the conventional number, letter or fractional drill with its metric equivalent for shop-floor conversion.
| Thread | 75% drill (US) | Metric ≈ | Thread | 75% drill (US) | Metric ≈ |
|---|---|---|---|---|---|
| #6-32 UNC | #36 | 2.7 mm | 3/8-16 UNC | 5/16″ | 7.9 mm |
| #8-32 UNC | #29 | 3.5 mm | 3/8-24 UNF | Q | 8.4 mm |
| #10-24 UNC | #25 | 3.8 mm | 1/2-13 UNC | 27/64″ | 10.7 mm |
| #10-32 UNF | #21 | 4.0 mm | 1/2-20 UNF | 29/64″ | 11.5 mm |
| 1/4-20 UNC | #7 | 5.1 mm | 5/8-11 UNC | 17/32″ | 13.5 mm |
| 1/4-28 UNF | #3 | 5.4 mm | 3/4-10 UNC | 21/32″ | 16.7 mm |
| 5/16-18 UNC | F | 6.5 mm | — | — | — |
Pipe Threads: NPT and BSPP (G) Tap Drills
Pipe threads behave differently from parallel fastener threads because the fit is controlled by depth, not by pitch diameter alone. NPT (tapered, 1:16) seals on thread interference: tap depth directly sets the L1 gauge position, so drill depth must leave room for the taper to develop over 3–5 effective turns. BSPP/G threads are parallel and rely on a face or O-ring seal, so they tap like ordinary threads and depth is set by the drawing.
| Size | TPI | Type | 75% tap drill | Metric ≈ |
|---|---|---|---|---|
| 1/8″ | 27 | NPT | 21/64″ | 8.3 mm |
| 1/4″ | 18 | NPT | 7/16″ | 11.1 mm |
| 3/8″ | 18 | NPT | 9/16″ | 14.3 mm |
| 1/2″ | 14 | NPT | 45/64″ | 17.9 mm |
| 3/4″ | 14 | NPT | 57/64″ | 22.6 mm |
| 1″ | 11½ | NPT | 1-5/32″ | 29.4 mm |
| G 1/8 | 28 | BSPP | — | 8.8 mm |
| G 1/4 | 19 | BSPP | — | 11.8 mm |
| G 3/8 | 19 | BSPP | — | 15.25 mm |
| G 1/2 | 14 | BSPP | — | 19.0 mm |
| G 3/4 | 14 | BSPP | — | 24.5 mm |
| G 1 | 11 | BSPP | — | 30.75 mm |
- NPT depth control: tap until the L1 (ring) gauge face is flush to within one turn of the reference plane; adjust Z depth in quarter-turn increments after the first article.
- BSPP depth control: tap to the specified effective thread depth plus 1–2 pitches of allowance; the seal is made at the face, not in the threads.
- Chips: pipe taps are large-diameter, coarse-pitch taps — prefer spiral-point or spiral-flute geometry with through-tool coolant when the spindle allows.
Roll (Form) Tapping: Larger Pilot Holes, Zero Chips
Form taps displace material into the thread profile instead of cutting it. The result is a chipless process — a major advantage in blind holes — with a work-hardened, slightly stronger thread and no risk of chips packed at the hole bottom. The trade-offs: form tapping requires ductile material (steel, aluminum, copper, stainless in some grades; never cast iron or brittle alloys), rigid setups, generous lubrication, and a larger pilot hole than a cut tap of the same size.
A practical starting rule for metric form taps is TD ≈ D − 0.5 × P; chart values below are typical mid-range figures. Because the thread is formed rather than cut, a drill tolerance of ±0.05 mm visibly changes forming torque — hold the pilot hole tightly and always validate against the tap manufacturer’s chart for the exact material and class of fit.
| Thread | Cut tap drill (mm) | Form tap drill (mm) | Delta |
|---|---|---|---|
| M4 × 0.7 | 3.3 | 3.7 | +0.4 |
| M5 × 0.8 | 4.2 | 4.65 | +0.45 |
| M6 × 1.0 | 5.0 | 5.55 | +0.55 |
| M8 × 1.25 | 6.8 | 7.4 | +0.6 |
| M10 × 1.5 | 8.5 | 9.3 | +0.8 |
| M12 × 1.75 | 10.2 | 11.25 | +1.05 |
- Lubrication: use EP cutting oil or a high-concentration emulsion; dry form tapping is not viable in steel.
- Speed: run form taps 30–50% faster than the equivalent cut tap in the same material.
- Blind-hole depth: form tapping needs far less overrun — useful thread depth + ~2 × P versus +4 × P for cut taps (see below).
Tap Chamfer Types and Geometry Selection
The chamfer at the front of a tap determines how many incomplete threads it leaves and which hole type it suits. Selecting the wrong chamfer is one of the most common causes of rough threads and broken taps in production.
| Chamfer type | Chamfered threads | Best suited to | Notes |
|---|---|---|---|
| Taper (starter) | 7–10 | Through holes, hand tapping | Lowest torque, cuts gradually |
| Plug | 3–5 | Through holes, general CNC work | The default choice on machining centers |
| Semi-bottoming | 2–2.5 | Shallow blind holes | Higher torque than plug |
| Bottoming | 1–2 | Blind holes tapped close to the bottom | Highest torque; pre-tap with a plug tap on deep threads |
Flute geometry follows the same logic as drilling: spiral-point (gun) taps push chips forward and suit through holes; spiral-flute taps pull chips up and out of blind holes; straight-flute taps handle short-chipping materials such as cast iron and brass; and form taps suit ductile materials in blind or through holes. Modern ranges such as the OSG EXOTAP series and YG-1’s spiral-point and spiral-flute lines cover these variants with TiN, TiCN and TiAlN coatings; TiAlN or nACo-type coatings are preferred for stainless and titanium where galling and built-up edge dominate.
Tapping Speeds and CNC Setup
Tapping speeds are modest compared with drilling because torque, not heat, limits the process. Start at the low end of each band until the first articles gauge correctly, then move up.
| Workpiece material | Cut tap Vc (m/min), HSS | Form tap Vc (m/min) |
|---|---|---|
| Low-carbon steel (<200 HB) | 12–18 | 18–28 |
| Alloy steel, 42CrMo4 (200–300 HB) | 8–12 | 12–18 |
| Stainless 304/316 | 3–6 | 5–8 |
| Titanium Ti-6Al-4V | 3–5 | not recommended |
| Gray cast iron | 8–14 | not applicable |
| Aluminum alloys | 30–60 | 45–90 |
| Brass / bronze | 25–45 | not applicable |
Rigid (synchronous) tapping is the default on any modern CNC: the spindle and Z axis are electronically geared, feed is set exactly to pitch (F = P in mm/rev), and the tap never has to pull itself into the hole. Floating holders are only needed on older controls. Two setup rules matter most:
- Runout: hold tool-side runout below 0.05 mm for class 6H threads; excess runout oversizes the pitch diameter and is the most common hidden cause of loose go gauges.
- Class of fit: where the control allows it, a small radial offset of the tap centerline (X-shift compensation, typically 0.02–0.05 mm) tunes the pitch diameter without changing the tap.
Worked Example: M10 × 1.5, 6H, Through Hole in S355 Plate, 20 mm Thick
- Pilot hole: 8.5 mm solid carbide drill, Vc = 80 m/min → n = 3000 rpm, f = 0.15 mm/rev, vf = 450 mm/min, coolant-through emulsion.
- Tapping: HSS-E TiAlN spiral-point plug tap, Vc = 12 m/min → n = 1000 × 12 / (π × 10) ≈ 382 rpm, rigid G84, F = 1.5 mm/rev → vf = 573 mm/min.
- Lubrication: flood emulsion 8–10% concentration, or MQL with tapping oil for small batches.
- Check: go gauge full-depth entry, no-go gauge stops within two turns.
Blind Hole Depth and Chip Management
Every blind tapped hole needs overrun below the last usable thread: the tap chamfer cuts incomplete threads at the bottom, and chips need somewhere to go. Undersized overrun is the classic cause of bottoming-out tap breakage.
| Process | Hole type | Drill depth rule |
|---|---|---|
| Cut tap | Blind | Useful thread + 4 × P (minimum) |
| Cut tap | Through | Useful thread; break through the far face |
| Form tap | Blind | Useful thread + 2 × P |
| NPT tap | Blind or through | Tap to L1 gauge reference; depth sets the fit |
- Prefer spiral-flute or form taps for blind holes; never peck a tap in and out — the reverse stroke work-hardens the crests and snaps the tap.
- Blow out or flush chips before gauging; chips left in the hole seize the go gauge and scratch the flanks.
- For thread depths beyond 2.5–3 × D in stainless, drop engagement to 65% and step up to a coated tap with a slightly larger pilot hole.
Common Tapping Problems: Cause and Fix
| Problem | Likely cause | Corrective action |
|---|---|---|
| Tap breaks at hole bottom | Drill depth overrun too small; chips packed | Add depth per the table; switch to spiral flute or form tap |
| Excessive torque | Pilot hole undersized; engagement above 75% | Recheck chart value; use 65% column for tough materials |
| Go gauge loose / oversize thread | Tool runout > 0.05 mm; worn tap; drill oversize | Check runout, replace tap, verify drill diameter |
| Torn, rough flanks | Wrong chamfer type; dull tap; insufficient lubricant | Use plug chamfer for through holes; fresh coated tap; raise oil concentration |
| Chatter marks on threads | Overhang too long; holder not rigid | Shorten tool overhang; use synchronous tapping with a rigid holder |
| NPT gauge leaks / fits loose | Insufficient tap depth | Deepen by quarter-turn steps until L1 gauge is within one turn |
| Form tap seizes in steel | No EP lubrication; hole too small; material too hard | EP oil mandatory; verify form-tap drill size; abandon form tapping above ~30 HRC |
Quick Selection Checklist
- Confirm the exact thread callout — M10 × 1.5, 3/8-16, G 1/4 and NPT 1/4 are easy to confuse on drawings.
- Choose engagement: 75% standard, 65% for stainless, titanium, Inconel and deep blind holes.
- Match tap type to the hole: spiral point for through, spiral flute or form for blind, straight flute for cast iron and brass.
- Match chamfer to depth: plug for most CNC work, bottoming only where the drawing leaves no room.
- Calculate drill depth: useful thread + 4 × P (cut) or + 2 × P (form).
- Set rigid synchronous tapping with F exactly equal to pitch; verify runout < 0.05 mm.
- Lubricate generously — EP oil for form tapping, 8–10% emulsion or MQL for cutting taps.
- Gauge the first article with go/no-go gauges before releasing the program to production.
Getting the pilot hole right is the cheapest form of tap insurance available. Keep this chart at the machine, derive non-listed sizes with the 1.299 formula, and let the engagement tables — not habit — decide when to open the hole up for a hard material or a deep blind thread.
Written by wg
Need Help?
Can't find a part number, need bulk pricing, or want a custom quote?
Currency
Show prices in your local currency.
Shop by Brand
View all 50+ brands →CNC Knowledge Hub
- Tap Drill Sizes and Thread Data Reference: ISO Metric, UNC/UNF and Pip… Nov 21, 2026
- MQL vs Flood vs High-Pressure Coolant: Cutting Fluid Selection Guide f… Nov 20, 2026
- Sumitomo AC800P CVD Turning Grades Explained: AC8025P, AC810P, AC820P… Nov 20, 2026
- Magnesium Alloy Machining Tool Selection Guide: DLC Coatings, Cutting… Nov 19, 2026