Tap Drill Size and Percent of Thread, Explained

By Bradley Taylor · August 2026

The chart on the shop wall says a 1/4-20 tap gets a #7 drill. That number is not wrong. It is one answer to a question most people never think to ask, which is how much thread the hole actually needs. Once you understand what the chart is assuming, you know when to follow it and when to drill bigger on purpose.

What percent of thread means

A tapped hole never has a complete thread form. The drill sets the minor diameter of the hole, and the tap cuts the thread profile into whatever material is left between that hole and the major diameter. The bigger the drill, the less material the tap engages, and the shallower the finished thread. Percent of thread is just a way of saying how much of the full theoretical thread height you kept.

For inch cut taps the standard formula is simple. Drill size equals major diameter minus 0.01299 times percent of thread, divided by threads per inch. Run it for 1/4-20 at 75 percent and you get 0.250 minus 0.0487, which is 0.2013. The closest standard drill is #7 at 0.201. So the familiar chart number is really a 75 percent thread number. The chart never tells you that. It just hands you the answer and lets you believe tapping is supposed to feel like that.

What more thread actually buys you

The reason this matters is that the two things you care about do not scale together. Thread strength climbs quickly as you go from a shallow thread up toward the middle percentages, then the curve flattens out. Somewhere past 75 percent you are adding very little strength. Tapping torque does the opposite. It keeps climbing, and it climbs steepest right where the strength curve has already gone flat. Published testing on this goes back to the 1940s and the conclusion has not moved. Past roughly three quarters engagement you are buying almost no strength and paying for it with real torque.

There is a second thing the strength argument leans on. In most joints with a normal amount of thread engagement, say a hole depth around the fastener diameter or more in decent material, the bolt breaks before the threads strip. When the bolt is the fuse anyway, chasing a fuller thread in the hole gains you nothing you can measure at the joint.

The honest default

In production work, on a machine, the industry standard recommendations are a perfectly good place to live. We use them at work. Rigid tapping in a CNC with the right speed, a good tap, and coolant where it belongs will run a 70 or 75 percent hole all day without complaint. The point of understanding percent of thread is not to argue with every chart in the building. It is to know which lever to pull when the situation changes.

When to drill bigger

Hand tapping is the clearest case. All the torque is coming from your wrist through a tap wrench, your alignment is only as good as your eye, and the tap has no sympathy for either problem. The larger the starting hole, the easier the job gets. You give up some full thread to get that ease, and most of the time that trade is worth taking. Backing off toward 60 or 65 percent makes the tap start easier, cut easier, and clear chips easier, and in a hole with normal engagement the joint will never know the difference.

Small taps are the other case. Below about a #10 there is not much torque margin between cutting and snapping, and everyone who has broken a #4-40 off in a finished part knows exactly what that costs. A slightly larger hole is the cheapest tap insurance there is.

Tough materials stack on top of both. Work hardening stainless, tool steels, anything gummy that loads up the flutes. The harder the material fights, the more a fuller thread costs you and the less it gives back.

When fuller thread earns its keep

There are honest exceptions. Thin material where you only get two or three turns of engagement. Short blind holes where the print will not let you drill deep. Soft materials like plastics and some aluminum where threads can strip before the fastener fails. In those cases the threads really are the weak link, and holding a higher percent of thread is doing real work. That is also where you check the print twice, because a callout that tight usually exists for a reason.

Roll form taps play by different rules

Everything above is for cut taps. A roll form tap does not cut material out of the hole, it squeezes the thread up out of the hole wall. The displaced material has to go somewhere, so the starting hole is quite a bit larger than a cut tap hole at the same percent of thread. Use the form tap drill size, not the chart on the wall. The tap drill calculator handles both types and shows you the nearest standard drills with the actual percent of thread each one gives.

The ten second version

Follow the standard recommendation when you are set up to tap under power in normal material. Drill toward 60 or 65 percent when you are hand tapping, running small taps, or fighting tough material, and accept that you are trading a little thread for a lot of ease. Save the high percentages for short engagement and soft materials where thread depth genuinely matters. And when the drill index does not have the exact size, check what percent the nearest drill actually gives before you grab it. The calculator does that math for you.

As always, this is general practice, not a spec. Prints, customer requirements, and the governing standard win every argument.