Tap Drill Calculator

Estimate a tap-drill hole diameter from basic thread diameter, TPI or metric pitch, tap process, and specified desired thread percentage using Guhring formulas.

Your inputs

Inches accept decimals and fractions. Millimeters accept decimals. Changing units reinterprets the numbers; it does not convert them.

Positive basic diameter in the selected dimension unit. Enter an actual diameter, not a screw number such as #10.
Positive decimal, always per inch regardless of dimension unit.
Positive pitch in the selected dimension unit. Select the M/MF family only for the corresponding thread.
Greater than 0 and no more than 100. Use the value specified for your application; 75 is a hypothetical example, not a universal recommendation.

Enter your values or load the labeled example.

Your result

Waiting for your inputs

Your results will appear here after calculation.

Guhring special-percentage formulas for UNC/UNF or M/MF cutting/forming taps. Basic thread dimensions and desired percentage are supplied by you. Formula diameter is not a selected drill, hole tolerance, actual thread percentage, strength rating, or permission to modify a door or frame. Verify actual tap, material, drilling process, and required thread limits.

Estimate the starting hole for a specified thread

Before tapping an approved hardware preparation, identify the actual thread and whether the tap cuts or forms it. A cutting tap removes material. A forming tap displaces material and requires a different starting-hole calculation. Using a cutting-tap hole for a forming tap can therefore be a substantial input error, even when the thread diameter and pitch match.

This tool applies the special-percentage formulas in Guhring’s “Common Formulas for Tapping,” printed page 240. It estimates a hole diameter for UNC/UNF or M/MF threads from a desired thread percentage that you specify. It does not choose that percentage, a numbered drill, a thread class, or an acceptable hole tolerance.

Basic diameter, pitch, and percentage describe different things

Use the thread’s basic major diameter, not a measured screw crest or a screw-number label. For a numbered thread, obtain its basic diameter from the applicable drawing or thread data before entering it. A label such as #10 is not a length.

For the UNC/UNF family, enter threads per inch. The axial pitch is 1/TPI inches. For M/MF, enter the axial pitch as a length in the selected dimension unit. That pitch is the spacing between adjacent threads along the axis. It is separate from the lead and travel per turn of a multiple-start thread.

Desired thread percentage is the percentage used by the cited hole-size formula. It is not a percentage of joint strength, screw engagement length, or load capacity. Guhring notes that actual percentage can vary from the desired value because of drilling runout. A formula result cannot confirm the actual thread produced by a drill and tap.

The formula depends on process and thread family

Let D be basic major diameter, N be TPI, p be metric axial pitch, and q be the entered percentage as a number such as 75. Guhring gives:

Thread family and process Formula hole diameter
UNC/UNF cutting D − 0.01299 × q/N, in inches
UNC/UNF forming D − 0.0068 × q/N, in inches
M/MF cutting D − q × p/76.98, in millimeters
M/MF forming D − q × p/147.06, in millimeters

The tool preserves these published coefficients. Inch and metric formula families use slightly different rounded constants, so switching the thread family is not just a unit conversion. Keep the family that describes the actual thread. Changing only the dimension unit, while entering equivalent lengths, preserves the physical result within that family.

At the same diameter and percentage, a finer pitch removes a smaller diameter allowance and leaves a larger starting hole. Increasing the desired percentage reduces the formula hole diameter. Forming and cutting use different reductions; one process must not be substituted for the other.

Guhring also lists D − pitch for general cutting-tap requirements and D − pitch/2 for general forming-tap requirements. Those shortcuts are distinct from the explicit-percentage formulas used here. None is a universal specification for every material, tap, thread form, or required fit. Pipe threads and other thread forms are outside this calculator.

Compare two hypothetical quarter-inch cases

Assume a 0.25 in basic diameter, 20 TPI, and a specified 75% desired thread. These are arithmetic examples, not recommended settings for a door assembly.

For a cutting tap:

Reduction = 0.01299 × 75/20 = 0.0487125 in

Formula hole = 0.25 − 0.0487125 = 0.2012875 in = 5.1127025 mm

For a forming tap with the same diameter, TPI, and desired percentage:

Reduction = 0.0068 × 75/20 = 0.0255 in

Formula hole = 0.2245 in = 5.7023 mm

The larger forming-hole estimate follows the different process formula. It does not establish that either process is appropriate for the actual workpiece. The main displays round to 0.201 in / 5.113 mm and 0.225 in / 5.702 mm, respectively; the unrounded hole value remains available. Do not select a drill solely by rounding this display.

For a separate metric example, M8 × 1.25, cutting, at a specified 75% gives 8 − 75 × 1.25/76.98 ≈ 6.782151208 mm. Its three-decimal result is 6.782 mm, not a selected commercial drill size.

Resolve the actual preparation before drilling

Check the current tap manufacturer’s application data, actual material, required thread dimensions and limits, hole-making accuracy, depth, and inspection method. A positive formula diameter only means the supplied values produce a positive number; it does not validate the thread designation or prove the tapping operation will succeed.

The machining-input record keeps these inputs separate from countersink geometry and drilling speed. Use the speed and feed calculator only with independently specified cutting parameters. Neither calculator grants permission to alter a listed door, frame, lock, or other assembly.