Tap Drill Size Calculator

Tap drill size for metric and UNC/UNF threads at any thread percentage, the nearest metric, fractional, number or letter drill, and form tap hole sizes.

The interactive tool loads here when JavaScript runs.

About this tool

What is the Tap Drill Size Calculator?

A tap drill chart gives one answer per thread, usually for 75% thread engagement. That is fine until the chart drill is missing from the rack, the job is in stainless or titanium and you want less engagement, or you are using a form tap that needs a bigger hole. This calculator works out the theoretical drill for any percent of thread, finds the nearest standard drill and tells you the engagement that drill really gives.

Pick a metric coarse or fine thread (M1.6 to M36), a UNC or UNF size from #0 to 1-1/2 inch, or enter any major diameter and pitch. Choose cutting or form (roll) tap, set the percent of thread, and choose metric drills, fractional, number and letter drills, or every drill at once. A table lists the drills either side of the target with their thread percentages, with the usable band shown in green.

For M6 x 1 at 75% the theoretical drill is 5.03 mm and a 5.0 mm drill gives 77%. For 1/4-20 UNC the answer is a #7 drill (0.201 in) at 75.4%, the same as every shop chart.

  • Metric coarse and fine threads from M1.6 to M36 and UNC/UNF from #0 to 1-1/2 inch, plus custom threads
  • Cutting and form tap formulas with any percent of thread
  • Nearest metric, fractional, number or letter drill and the real thread percentage it gives
  • Options table either side of the target, a full chart for the chosen series and a drill check field
  • Formula panel, copy and share link; runs entirely in your browser
Read the guide: Tap Drill Sizes and Percent of Thread: Choosing the Right Hole

How to use the Tap Drill Size Calculator

  1. Choose metric, UNC/UNF or a custom thread, then pick the size. For a custom thread enter the major diameter and pitch in millimetres.
  2. Select cutting tap or form tap. The percent of thread resets to 75% or 65%; change it to suit the material and the job.
  3. Leave the drill series on Auto to match the thread system, or choose metric, inch or all drills to see what else is close.
  4. Read the recommended drill and the thread percentage it gives, then scan the options table for an alternative in the green band.
  5. Type a drill you already have in the check field to see what thread percentage it would leave.

Worked examples

M6 x 1 coarse, cutting tap

Input

M6 x 1, cutting tap, 75% thread, metric drills

Output

Theoretical 5.026 mm; 5.0 mm drill gives 77.0%

The common rule "major minus pitch" gives the same 5.0 mm. A 5.1 mm drill would drop the thread to 69%, still fine in most steels.

1/4-20 UNC, cutting and forming

Input

1/4-20, cutting tap 75%; then form tap 65%

Output

Cut: #7 (0.201 in) at 75.4%. Form: #1 (0.228 in) at 64.7%

The form tap needs a hole 0.027 in larger. Using a #7 hole with a form tap would very likely break the tap.

1/2-13 UNC with inch drills

Input

1/2-13, 75% thread, inch drills

Output

Theoretical 0.4251 in; 27/64 in drill gives 78.2%

With all drills selected the calculator picks a 10.8 mm metric drill at 0.4252 in, which lands almost exactly on 75%.

M12 x 1.75 and the chart value

Input

M12 x 1.75, cutting tap, 75%

Output

Theoretical 10.295 mm; 10.3 mm gives 74.8%; the chart 10.2 mm gives 79.2%

Many charts list 10.2 mm, which is D − P rounded down. Both are acceptable; 10.3 mm is easier on the tap.

Background and insight

The percent-of-thread convention measures how much of the basic thread depth the tapped hole leaves for the screw to bear on. For 60° unified and ISO metric threads the basic double height used for this purpose is 1.299 × pitch, so the cutting tap drill formula is drill = D − 0.01299 × %thread × P, with P in millimetres or as 1/TPI in inches. Machinery's Handbook gives this form and the inverse, %thread = (D − drill) / (0.01299 × P).

Tap makers commonly point out that a 75% thread is only a few percent weaker than a full thread in steel, because the bolt or the external thread usually fails first, yet a 100% thread takes roughly three times the torque to tap. That is why charts settle on 75% for general work, 60 to 65% for tough or work-hardening alloys, and higher only for thin sections where every bit of engagement counts.

Form taps do not cut; they push material into the thread shape, so the hole must be larger. Tap makers and Machinery's Handbook give drill = D − 0.0068 × %thread × P for forming, with 60 to 70% thread typical. A 1/4-20 form tap at 65% calls for 0.2279 in, which is a #1 drill. Always check the tap maker's chart, since some coatings and alloys move the ideal hole by a few hundredths of a millimetre.

Common use cases

  • Drilling and tapping on the shop floor

    Find the tap drill when the chart drill is missing and see what the closest drill on the rack will give you.

  • Hard or gummy materials

    Drop to 60 to 65% thread in stainless, titanium or Inconel to cut tapping torque and tap breakage.

  • Form tapping

    Get the larger pilot hole a thread-forming tap needs in aluminium, copper and mild steel.

  • CAD and drawings

    Pick a hole size for a tapped hole callout and record the thread engagement it produces.

Tips and limitations

  • Drills cut slightly oversize, often by 0.02 to 0.05 mm in steel, so the real thread percentage is a little lower than the table shows.
  • Blind holes need extra depth for the tap chamfer: about 3 to 5 pitches for a plug tap and 1 to 2 for a bottoming tap.
  • In soft aluminium and plastics, higher thread percentages hold better; in hard steels, go lower to save the tap.
  • Engagement length matters as much as thread percentage. One to one and a half diameters is typical in steel; use more in aluminium or cast iron.
  • For Class 2B or 6H fits, check that the drill falls inside the minor diameter limits in ASME B1.1 or ISO 965 for critical parts.

Frequently asked questions

How do you calculate tap drill size?

For a cutting tap, tap drill = major diameter − 0.01299 × percent of thread × pitch. At 75% that is about major − 0.974 × pitch, which is why "major minus pitch" works as a quick metric rule. For inch threads use pitch = 1 / TPI.

What drill size for a 1/4-20 tap?

A #7 drill (0.201 in, 5.1 mm) gives about 75% thread with a cutting tap and is the standard chart size. For a form tap use a #1 drill (0.228 in) or 5.8 mm, which gives about 65% thread.

What does percent of thread mean?

It is how much of the full basic thread depth is left in the tapped hole, measured on the diameter. A 75% thread has a minor diameter that leaves three quarters of the 1.299 × pitch basic double depth for the screw to bear on.

Why is 75% thread the standard for tap drills?

Strength tests show a 75% thread is only slightly weaker than a full thread because the screw usually breaks first, while tapping a 100% thread needs about three times the torque and breaks far more taps. 75% is a practical compromise for most steels.

What is the tap drill size for M8 x 1.25?

6.8 mm, which gives about 74% thread with a cutting tap. A form tap at 65% needs about 7.45 mm, so a 7.4 or 7.5 mm drill depending on the tap maker's chart.

How is a form tap drill size different?

Form taps displace material instead of cutting it, so they need a larger pilot hole. The formula is major diameter − 0.0068 × percent of thread × pitch, and 60 to 70% thread is normal. Using a cutting tap drill with a form tap overloads and breaks it.

Can I use a metric drill for a UNC thread?

Yes. The thread does not care what system the drill is labelled in, only its diameter. A 10.8 mm drill is closer to the ideal 1/2-13 hole than 27/64 in, and a 5.1 mm drill is a fine stand-in for a #7 on 1/4-20.

Is there an in-depth guide to the Tap Drill Size Calculator?

Yes. “Tap Drill Sizes and Percent of Thread: Choosing the Right Hole” covers the background, how it works, common pitfalls and worked examples. Read the full guide.

Related Tools You May Like

Free, in-browser tools that pair well with this one.