ThreadLab — Tap Drill, Thread & Measurement Suite

Use an 8.5 mm drill bit for an M10 x 1.5 tap. That is the standard coarse-thread tap drill, giving about 77% thread engagement. The quick shop rule for metric threads is: tap drill = major diameter minus pitch (10 - 1.5 = 8.5 mm). For tougher materials like stainless steel, open the hole slightly to 8.6-8.7 mm to reduce tap breakage risk.

Use a #7 drill bit (0.201 inch) for a 1/4-20 UNC tap. That is the standard tap drill and produces about 75% thread engagement, the default used in Machinery's Handbook tap drill tables. If you are tapping steel or stainless and want an easier cut, a 7/32 inch (0.2188 inch) drill gives roughly 50% thread, which is still plenty strong for most non-critical joints.

For a cutting tap at the standard 75% thread engagement: metric, drill (mm) = major diameter (mm) - pitch (mm), e.g. M8 x 1.25 needs 6.8 mm. Inch threads: drill (inch) = major diameter - 75 / (76.98 x TPI), e.g. 3/8-16 needs 0.375 - 75/(76.98 x 16) = 0.314 inch, so use a 5/16 inch (0.3125 inch) drill. For a custom thread percentage, replace 75 with your target percent in the same formula. This calculator does the math for you in the Tap Drill Finder tab.

Thread percentage is how much of the full V-thread depth your drilled hole leaves for the tap to cut: % = (major diameter - drill diameter) x 76.98 / pitch. A 75% thread is the shop standard - strong enough for nearly all joints while keeping tapping torque manageable. The practical working range is 65-85%. Use 75-85% for aluminum, brass, and plastics; drop to 65-70% for stainless steel and titanium, where full-depth threads greatly increase tap breakage risk with little strength gain.

For metric pitch: use a caliper to measure across 10 thread crests and divide by 10, or lay a steel rule against the thread and count crests over 10 mm. For TPI: count the crests in exactly one inch. A thread pitch gauge is faster and more accurate than either method. Enter your measurements into the Thread Identifier tab - it converts pitch to TPI automatically (TPI = 25.4 / pitch in mm) and matches against standard metric, UNC, UNF, and NPT threads.

Measure two things: the outside diameter with a caliper, and the pitch (metric) or threads per inch (a pitch gauge is best). Then match the pair against standard tables - many different threads share a diameter but almost none share both diameter and pitch. The Thread Identifier tab does this automatically and ranks the closest matches across metric coarse/fine, UNC, UNF, and NPT. Tip: pipe threads (NPT) are tapered 1:16, so measure the OD at the large end.

The three-wire method is the standard way to measure the pitch diameter of an external thread accurately: you rest two wires in adjacent thread grooves on one side, one wire on the opposite side, and measure over them with a micrometer. The Machinery's Handbook formulas for 60-degree threads are: best wire W = 0.57735 x pitch, measurement over wires M = E - 0.866025 x P + 3W, and pitch diameter E = M + 0.866025 x P - 3W. The calculator tab solves it in both directions and computes the wire constant C = 3W - 0.866025 x P, so E = M - C.

Use the best-size wire: W = 0.57735 x pitch (for 60-degree UN and metric threads). It contacts the thread flanks exactly at the pitch line, where the measurement is least affected by small angle errors. For 20 TPI that is 0.0289 inch; for M10 x 1.5 it is 0.866 mm. If you only have a standard wire set, pick the closest size - the calculator shows the nearest standard wire and recomputes the wire constant for the actual wire you use.

Use a 23/32 inch (0.7188 inch, 18.26 mm) drill for 1/2-14 NPT. NPT tap drills from the standard chart: 1/8-27 uses R (0.339 inch), 1/4-18 uses 7/16 inch, 3/8-18 uses 37/64 inch, 3/4-14 uses 59/64 inch, and 1-11.5 uses 1-5/32 inch. Remember NPT threads are tapered 1:16 (3/4 inch per foot), so drill the hole straight and let the tapered tap form the taper - do not try to pre-taper the hole.

NPT (National Pipe Taper) threads taper at 1:16, so the male and female threads wedge together to form a pressure-tight seal - that is why they are used for plumbing, pneumatics, and hydraulics. NPS (National Pipe Straight) threads do not taper; they seal with a gasket or O-ring instead. You cannot reliably seal an NPT male thread in an NPS female port without sealant, and mixing them is a common cause of leaks.

A clearance hole is the unthreaded hole a bolt passes through - it must be slightly larger than the bolt's major diameter. Close fit is the tightest practical clearance (e.g. 0.257 inch / F drill for a 1/4 inch bolt) for precision assemblies where parts must not shift. Free fit is looser (0.266 inch / H drill for 1/4 inch) for general assembly, painted parts, or slightly misaligned holes. Metric follows ISO 273 with fine, medium, and coarse series - e.g. M10 uses 10.5, 11, or 12 mm.

Per ISO 273: for M8, drill 8.4 mm (fine), 9 mm (medium, the common choice), or 10 mm (coarse). For M10, drill 10.5 mm (fine), 11 mm (medium), or 12 mm (coarse). Medium (normal) series suits general machine assembly; use fine for dowel-like precision fits and coarse for structural steel or castings. The Clearance tab lists all three series for M3 through M24 plus inch close/free fits.

The rule of thumb from Machinery's Handbook practice: minimum full-thread engagement of 1 x bolt diameter in steel, 1.5 x diameter in cast iron or brass, and 2 x diameter in aluminum or magnesium. Deeper than that adds little strength because the first few engaged threads carry most of the load. The Thread Depth tab computes the minimum engagement for your thread size and material, plus the drill depth needed to achieve it.

Drill depth = desired full-thread depth + tap chamfer allowance + drill point allowance. The chamfer (the tapered lead of the tap that does not cut full threads) needs about 7-10 threads for a taper tap, 3-5 for a plug tap, and 1-2 for a bottoming tap. Add roughly 0.3 x drill diameter for the 118-degree drill point. Example: an M10 x 1.5 hole with 15 mm of full thread using a plug tap needs 15 + 4 x 1.5 + 0.3 x 8.5 = 23.6 mm drill depth.

The Charts tab contains full printable tap drill tables for metric coarse/fine and UNC/UNF threads, plus the clearance drill chart - use your browser's print function (or save as PDF) for a shop copy. A calculator beats a chart when you need a non-standard thread percentage, an unknown-thread identification, or three-wire measurement math; the chart is best taped to the wall for the twenty sizes you use every day.

All formulas are the standard published ones: tap drill and thread percentage per the cutting-tap formula (drill = D - Hp x P / 76.98), three-wire measurement per Machinery's Handbook (M = E - 0.866025 x P + 3W), NPT dimensions per ASME B1.20.1-based charts, and metric clearance holes per ISO 273. Treat results as planning references - verify critical or pressure-retaining threads with proper thread gauges. Everything runs 100% in your browser; no input is sent anywhere. Machine safely: wear eye protection, never wear gloves near rotating tools, and secure your workpiece before cutting.