Tap Drill Size Calculator
Find the tap drill for any metric or unified thread at a target percent of thread, with the nearest stocked drill and minimum thread depth by material.
70 to 75 percent is the usual target. Above 80 the tapping torque climbs steeply for very little strength.
Use 2x diameter in soft tempers, or specify a threaded insert.
Tap drill
Thread engagement
The tap drill for a thread follows from the percent of thread you want, not from a single correct number. This calculator solves the standard relation for metric and unified threads, snaps the result to the nearest stocked number, letter, fractional or metric drill, reports the engagement each one actually produces, and gives a minimum thread depth for your material.
How to read the result
Percent of thread describes how much of the theoretical sharp-V thread form is actually cut. It is not a measure of strength in any direct sense: going from 75 percent to 100 percent adds only a few percent of stripping strength while roughly doubling tapping torque, which is why production shops work nearer 65 to 75 percent and tap breakage falls away.
The familiar shop rule for metric threads, drill diameter equals major diameter minus pitch, is a convenient approximation rather than a 75 percent rule. For M6 x 1 it gives a 5 mm drill, which actually leaves about 92 percent of thread. That is fine in free-machining steel and punishing in stainless. The calculator shows the real figure so the choice is deliberate.
Thread depth matters at least as much as hole size. A fastener tightened into too few threads strips the part rather than the bolt, and the softer the material the deeper the engagement has to run before the joint reaches the fastener's own strength.
Frequently asked questions
- What percent of thread should I aim for?
- Around 70 to 75 percent for general work. Below about 60 percent the thread loses meaningful strength; above 80 percent tapping torque climbs steeply for very little gain, and tap breakage becomes the dominant risk in tough or gummy materials. In stainless and titanium, working nearer 60 to 65 percent is common and sensible.
- What is the tap drill for M6 x 1.0?
- 5.2 mm (0.205 in) gives 75 percent of thread by the standard formula. The 5.0 mm drill most shops reach for gives about 92 percent, which taps harder and gains very little strength. Both are legitimate; 5.0 mm is the safer choice only if the thread will see repeated disassembly in a soft material.
- How deep should a tapped hole be?
- Start at one times the major diameter for steel and stainless, 1.5 times for cast iron, bronze and aluminum, 2 times for magnesium and zinc, and 2.5 times for plastics. Add a couple of pitches of unthreaded relief at the bottom of a blind hole so the tap is not bottoming as it cuts.
- Should I use a threaded insert instead?
- In aluminum, magnesium or plastic that gets disassembled more than a few times, yes. Heat-set inserts in plastic and helical or keyed inserts in light alloys move the wear to a steel thread and survive repeated service. For a joint assembled once, a correctly sized tapped hole at adequate depth is usually enough.
Other calculators
Ready to check a real design? Upload your files. We measure your model against per-process, per-material rules and send a DFM review before you commit to a quote.