Tap Drill Size Calculator
Tap drill sizes for UNC, UNF and metric threads — with the form tap hole, the torque cost, and why 75% thread is a convention rather than a target.
75% is a convention, not a target
Every tap drill chart is built around 75% thread engagement, so most people tap 75% threads without ever deciding to. It is the most expensive habit in the subject: 75% costs roughly twice the tapping torque of a 60% thread, for almost no strength you will ever use.
The reason it buys so little is the failure mode. In a steel joint with about one diameter of engagement, the bolt breaks in tension before the threads strip. The threads are already stronger than the fastener at 55 or 60%, so the extra material a 75% thread leaves in the hole is never loaded anywhere near its capacity. Meanwhile the torque to cut it climbs steeply, because the tap is removing more material and rubbing over more flank area at once. A broken tap in a nearly finished part costs vastly more than the difference is worth — which is why production shops routinely run 55 to 65%, and why 75% survives mostly as the number on the wall.
- A form tap needs a bigger hole. It displaces material instead of cutting it, so the thread crest is pushed up out of the hole wall and the hole has to start larger — roughly half the deduction. Using a cutting tap's drill with a form tap will snap it, and that is one of the commonest ways a new form tap dies on its first hole.
- The answer to a weak joint is length, not percentage. Percentage sets how deep each thread is; length sets how many of them share the load. One diameter of engagement in steel, about two in aluminium, two and a half in plastics — and in soft materials it is the material around the thread that fails, not the thread form.
- Small taps break in torsion long before the thread strips. Below about an eighth of an inch or M4, the tap itself is the weak point regardless of what any strength calculation says. Lower percentage and generous lubrication buy far more than arithmetic does.
- Stainless is the material that punishes 75%. It work-hardens and galls, so tapping torque is already high before percentage enters the picture. Cast iron is the opposite: free-machining and low in torque, so a full thread is genuinely cheap and 75% is a real choice there rather than an inherited default.
- The achievable percentage jumps. Drill sizes are a discrete set, so asking for 70% may hand you 73%. No tap drill chart figure is exact, including the ones here.
- A real hole is not the calculated hole. A twist drill wanders, cuts oversize and leaves lobes, so the actual percentage usually lands a few points below the calculation. Reaming or boring before tapping is what closes that gap when it matters.
How to use
- Pick the thread and the material you are tapping into.
- Set the thread engagement, or take one of the presets.
- Read the cutting tap drill, and the larger hole a form tap needs.
- Check the engagement depth — length moves the failure point, percentage barely does.
Frequently asked questions
Why is 75% thread engagement a bad default?
Because it is a convention rather than a decision. Every tap drill chart is built around 75%, so people tap 75% threads without ever choosing to, and it costs roughly twice the tapping torque of a 60% thread. In a steel joint with about one diameter of engagement the bolt breaks in tension before the threads strip, so the threads are already stronger than the fastener at 55 or 60% and the extra material is never loaded near its capacity. A broken tap in a nearly finished part costs vastly more than the difference is worth.
So what should I use instead?
Production shops routinely run 55 to 65%, and that is the range worth defaulting to. Stainless and tool steels sit at the low end because they work-harden and gall, so tapping torque is already high before percentage enters the picture. Cast iron and brass sit at the high end because they are free-machining and a full thread is genuinely cheap there. The only place 75% is a real choice rather than an inherited default is a material that taps easily.
Why does a form tap need a different hole?
A form or roll tap displaces material rather than cutting it, so the thread crest is pushed up out of the hole wall and the hole has to start larger — roughly half the deduction of a cutting tap. Using a cutting tap drill with a form tap is one of the commonest ways a new form tap dies on its first hole, because it has nowhere to put the material it is trying to move. In exchange you get no chips, a stronger grain-flow thread and much longer tap life.
How deep should the hole be threaded?
About one fastener diameter in steel, one and a half in cast iron and brass, two in aluminium and two and a half in plastics. Engagement length is the number that actually moves the failure point: percentage sets how deep each thread is, but length sets how many threads share the load. If a joint is stripping, adding length fixes it and adding percentage almost never does — especially in soft materials, where it is the material around the thread that gives way rather than the thread form.
Where does the 0.0130 in the tap drill formula come from?
From the geometry of a 60 degree thread. The theoretical single thread height is 0.6495 divided by threads per inch, and the minor diameter sits two of those below the major diameter, so a full 100% thread deducts 1.299 divided by TPI. Divide by 100 and you get the 0.0130 per percent that every shop chart uses. The metric equivalent is pitch times percentage divided by 76.98, and the two agree with each other once you convert.
Why does the calculator not hit the percentage I asked for?
Because drill sizes are a discrete set. Asking for 70% on a given thread may hand you 73%, since the nearest stocked drill is wherever it happens to be. This is worth knowing before treating any tap drill chart figure as exact — the standard 1/4-20 tap drill is a number 7, which actually gives 75.4% rather than a round 75%. Every chart in every shop is rounded the same way.
Will my hole really be the size the drill says?
Usually not quite. A twist drill wanders as it enters, cuts slightly oversize because of runout, and leaves a hole with lobes rather than a true circle, so the real thread percentage typically lands a few points below the calculation. That works in your favour if you were aiming at 75% and against you if you were already at 55%. Reaming or boring before tapping is what closes the gap when the number genuinely matters.
Why do small taps break so easily?
Because torsional strength falls with the cube of diameter while cutting torque falls much more slowly. Below about an eighth of an inch or M4 the tap itself is the weak point regardless of what any thread strength calculation says, so it breaks in torsion long before the thread would ever strip. At those sizes a lower thread percentage, a sharp tap and generous lubrication buy far more reliability than arithmetic does.
🔒 This tool runs entirely in your browser. Nothing you enter is uploaded, logged, or stored.