Every unified inch and ISO metric thread, with the drill that cuts it and the hole that clears it.
Tap drills, clearance drills, minor diameters, and thread percentages — computed, not transcribed, so you can dial the thread percentage to your material instead of picking between somebody else’s 75% and 50% columns. Set a sheet thickness and the chart also tells you the thing most charts leave out: whether that thread will actually hold.
Tap drill, clearance drill, and minor diameter for every thread in both series. The standard column is the traditional shop pick — the value stamped on the chart in every tool room. The live column recomputes for whatever thread percentage you dial in, and always tells you the percentage that drill actually achieves, so nothing hides behind a rounding convention.
Thread percentage is how much of the theoretical full thread actually gets cut. It is the one number that decides whether your tap survives the hole. Going from 75% to 100% buys you a few percent of pull-out strength and roughly doubles the tapping torque — which is why nobody taps to 100% on purpose.
The largest tap drill on any chart. Roughly 90% of the strength of a 75% thread at a fraction of the torque. Reach for it in hardened steel, in blind holes deeper than 2× diameter, and any time you have already snapped one tap.
304 and 316 work-harden as the tap cuts, so the last thread is always the hardest. Backing off to 60–65% keeps the torque down and the tap in one piece. This is our default on stainless.
A1008 and A36 cut cleanly but are strong enough that full-depth threads load the tap hard. 70% is the sweet spot for carbon steel sheet and plate.
The classic chart default, and the right call in soft metals where torque was never the constraint. 5052, 6061, and brass all tap happily at 75%. Above 80% you are fighting the tool for almost nothing.
A tap drill chart tells you what to drill. It does not tell you whether the thread will hold — and in flat sheet, that is the question that actually decides the design.
Tap a 1/4-20 into 0.060″ sheet and you get 1.2 full threads. It will feel tight going together and tear straight out the first time somebody torques it. There is no drill size that fixes that.
Two gates have to clear before a tapped hole in sheet is worth having:
1. At least two full threads. thickness ÷ pitch ≥ 2. Below two threads the thread strips under any real assembly torque. Three or more is a thread you can trust.
2. Thickness of at least half the major diameter. The pitch gate alone is misleading at large diameters — 0.090″ sheet clears two threads of 5/16-24 on paper, but that joint tears out through the sheet long before the thread strips.
Set a sheet thickness in the chart above and every row gets checked against both. Where a thread does not clear them, self-clinching hardware is the answer — a PEM stud or nut moves the load into a flange that is far bigger than the hole, and works down to about 0.040″.
A tap drill chart assumes somebody is holding a drill. On a laser-cut part the tap hole gets cut by the laser first — and the laser has a minimum hole size that scales with material thickness. Which means the two requirements pull in opposite directions.
In the quote app: flag the hole and pick the thread — #8-32, M4×0.7 — and the tap drill diameter is applied for you. If you would rather model it, model the tap drill diameter and note the thread, or model the clearance hole and call out the thread. Any of the three works; see tapping for the file requirements.
The limit you cannot design around: our recommended minimum laser-cut hole is 1 × material thickness, and the absolute floor is 0.5 × thickness. Below the recommended floor the bore tapers and the edge roughens; below the absolute floor the laser cannot make the hole at all and it becomes a drilled secondary operation.
So the two rules squeeze from opposite sides. The thread needs the sheet thick — at least half the screw diameter, and two full threads of pitch. The laser needs the tap hole large relative to the sheet. Since a tap drill is always smaller than its screw, thick material runs out of laser first: a 1/4-20 tap hole is 0.201″, so in 1/4″ plate that hole is below the recommended floor and we drill it instead of cutting it.
The band chart below is that squeeze, computed for every size we tap. Nothing here blocks a part — a drilled tap hole is a normal secondary operation, it just costs a little setup and lead time. It is worth knowing before you pick a gauge.
You have a drill in your hand, or a diameter on a print with no thread callout. Pick the drill and see every thread it is a sensible tap drill for, with the thread percentage each one lands at.
Shows every thread landing between 50% and 90% engagement. Outside that band the drill is either too tight to tap or too loose to hold.
The questions that come up most often on tapped holes, thread percentage, and what actually holds in sheet metal.
#7 drill — 0.201″ — which lands at about 75% thread. That is the standard chart value for 1/4-20 UNC. Tapping stainless or a deep blind hole? Open it to 13/64″ (0.2031″) for roughly 70%, or use the slider in the chart above to pick your own percentage and see the real drill.5.0 mm for M6×1, the standard coarse pitch. Metric has a rule of thumb that actually works: tap drill = major diameter − pitch. So 6 − 1 = 5. It lands at 77% thread, which is why the rule survived. For M6×0.75 fine pitch the drill is 5.25 mm. The same rule gives M3 → 2.5, M4 → 3.3, M5 → 4.2, M8 → 6.8, M10 → 8.5.thickness ÷ pitch ≥ 2) and thickness of at least half the major diameter. Three full threads is a thread you can trust. Below those limits, use self-clinching hardware — a PEM stud or nut spreads the load into a flange much larger than the hole and works down to about 0.040″.0.060″. In the inch series only #4-40 clears both gates — 2.4 full threads — and even that is marginal, being under three. #6-32, #8-32 and #10-32 all land at 1.9 threads and fail the two-thread minimum outright, which surprises people because those are the sizes they reach for. Metric fares better on the finer pitches: M2, M2.5 and M3 all hold. For anything larger than about a #4 in 16 gauge, use self-clinching hardware. Set 0.060″ in the chart above and it marks every row for you. Converting gauges? See the sheet metal gauge chart.1 × material thickness with an absolute floor of 0.5 × thickness. A tap drill is always smaller than its screw, so thick material runs out of laser first — a 1/4-20 tap hole is 0.201″, which is under the recommended floor in 1/4″ plate, so we drill it as a secondary operation instead. That is routine, not a problem; it just adds a little setup. The band chart above works it out for every size we tap.drill = major − 1.299 × pitch × (% / 100) and snapped to a real drill size, then shown with the percentage that drill actually achieves. Minor diameters use major − 1.22687 × pitch. Both were checked against the published inch chart across all 53 thread rows — every minor diameter and every 75% tap drill matches. Metric standard tap drills use the D − pitch rule and match the published metric chart on all 26 rows. Clearance holes are tabulated: ISO 273 for metric, standard drill-chart practice for inch.