Every machinist has a tap drill chart taped to the wall. The chart says 3/8-16 UNC uses a 5/16 drill. But why? And when should you use something different? The answer is thread percentage. The standard drill size gives you approximately 75% thread engagement, which is the sweet spot where the thread is strong enough for any reasonable application but the tap is not fighting to cut a full-depth thread in a blind hole full of chips.
Understanding thread percentage gives you the ability to make smart compromises. Need to tap a deep hole in stainless? Drop to 65% thread and the tap will actually survive. Tapping cast aluminum and stripping threads? Go to 80% or use a thread-forming tap. This guide covers the math, the common sizes, and the practical decisions around chip evacuation, bottoming taps, and thread-forming alternatives.
Why 75% Thread Engagement Is the Standard
At 75% thread engagement, the internal thread carries about 90% of the load capacity of a full-depth thread. Going from 75% to 100% only gains about 10% more strength but roughly doubles the tapping torque and dramatically increases the risk of tap breakage.
The formula for drill size at a given thread percentage is: Drill diameter = Major diameter − (Thread percentage / 76.98 × Pitch). For 3/8-16 UNC at 75%: Drill = 0.375 − (75 / 76.98 × 0.0625) = 0.3141". That is very close to a 5/16" drill (0.3125"), which is why 5/16" is the standard tap drill for 3/8-16.
The reason 75% became the standard is economics. Tap life at 75% is roughly 3 to 5 times longer than at 85%. The bolt will break before the thread strips at 75% engagement, and replacing broken taps in blind holes costs far more than the marginal thread strength gained by cutting deeper.
50% engagement → ~75% of full thread strength
60% engagement → ~83% of full thread strength
75% engagement → ~90% of full thread strength
100% engagement → 100% but taps break constantly
The bolt always breaks before a 75% thread strips.
Drill & Tap Calculator
Two-in-one drill and tap calculator. Get drilling RPM and feed rates for any drill size, plus tap drill sizes with thread percentage for UNC, UNF, and Metric threads. Includes comprehensive thread data tables.
When to Drop to 60% or 65% Thread
Deep holes (depth greater than 1.5 times the tap diameter) in tough materials are where reduced thread percentage saves taps and money. Dropping to 65% thread reduces tapping torque by 20 to 30 percent and dramatically improves chip clearance in the flutes.
Exotic alloys like Inconel, Hastelloy, and titanium are another case for reduced thread percentage. These materials work-harden during cutting, and the additional volume removed at 75% vs 65% increases heat and tool wear disproportionately.
Through holes are more forgiving than blind holes because chips can exit through the bottom. For blind holes deeper than 1D in any material harder than HRC 25, consider reducing thread percentage or using a spiral-flute tap that lifts chips out.
A common rule of thumb: for blind holes deeper than 1.5D in steel or stainless, use a drill that gives 65% thread. For blind holes deeper than 2D, consider thread milling instead of tapping. Thread mills cannot break off in the hole.
Tap Types: Matching the Tap to the Hole
Straight-flute taps push chips ahead of them. They work in through holes and shallow blind holes. Spiral-point taps (gun taps) push chips forward through the hole. Excellent for through holes but cannot be used in blind holes. Spiral-flute taps have helical flutes that lift chips back out of the hole. They are the right choice for blind holes.
Bottoming taps have very short chamfers (1 to 2 threads) so they can cut threads close to the bottom of a blind hole. If the fastener needs to seat at the bottom, start with a taper or plug tap and finish with a bottoming tap.
Thread-forming taps (roll taps) do not cut material; they displace it. No chips means no chip packing, no broken taps, and threads that are actually stronger than cut threads because the grain flow follows the thread form. Ideal for aluminum, copper, and low-carbon steel.
Thread-forming taps require a slightly larger hole (60 to 65% thread) because the displaced material needs somewhere to go. A carbide thread-forming tap in 6061 aluminum can produce 10,000 to 50,000 holes before replacement.
Through hole → Spiral-point (gun) tap
Blind hole, shallow → Straight-flute tap
Blind hole, deep → Spiral-flute tap
Bottom of blind hole → Bottoming tap (second pass)
Aluminum or copper → Thread-forming (roll) tap
Drill & Tap Calculator
Two-in-one drill and tap calculator. Get drilling RPM and feed rates for any drill size, plus tap drill sizes with thread percentage for UNC, UNF, and Metric threads. Includes comprehensive thread data tables.
Chip Evacuation: The Real Reason Taps Break
Taps do not break because the material is too hard. Taps break because the flutes pack with chips, the torque spikes, and the tap twists apart. If you solve chip evacuation, you solve tap breakage.
In manual tapping, advance the tap one turn, then reverse half a turn to break the chip. On CNC, rigid tapping with peck cycles is more reliable than continuous tapping in deep or tough holes.
Tapping fluid matters more than most machinists realize. The right fluid reduces cutting forces by 15 to 25 percent. In steel, use sulfurized cutting oil. In aluminum, use a light tapping fluid. In stainless, use chlorinated or sulfur-chlorinated cutting oil. WD-40 is not tapping fluid.
Hole preparation also affects chip evacuation. A reamed hole has a smooth, round bore that lets the tap cut evenly. For critical tapped holes in tough materials, drilling slightly undersize and reaming to the final tap drill diameter is worth the extra operation.