Charts

Tap Drill Size Chart: Metric and Imperial

Complete workshop tables for choosing metric and Unified tapping drills, with thread-engagement guidance and material adjustments.

A tapping drill controls how much material remains for the tap to form into a thread. Too small a hole creates excessive engagement, torque and heat; too large a hole weakens the thread. These charts provide common cutting-tap starting sizes for ISO metric coarse and fine threads and Unified UNC and UNF threads. They target roughly 70–75% engagement, the practical region that gives strong threads without needless tapping load.

Metric coarse tap drill sizes: M1.6–M24

Coarse pitch is the default when an ISO metric callout gives only the major diameter. The drill sizes below are widely stocked workshop choices. Engagement is an estimate because real drill holes, tap limits and material recovery vary.

Metric fine tap drill sizes: M1.6–M24

Fine threads have shallower thread depth and therefore use a larger tapping drill than a coarse thread of the same major diameter. Always include pitch in stores requests and setup sheets: “M10” alone normally means M10 × 1.5, not M10 × 1.0 or M10 × 1.25.

UNC and UNF tap drill sizes: #4–1 inch

Number, letter and fractional drills are mixed because the closest standard drill differs by thread. Decimal equivalents remove ambiguity when choosing from a metric-indexed cabinet. Typical engagement is shown as a range because unified calculations depend on truncation assumptions and practical drill availability.

Understanding thread engagement

Percentage engagement describes the proportion of theoretical full thread height left for the tap to cut. A nominal 75% thread is not three quarters of the hole diameter; it is three quarters of the available radial thread depth. Testing has long shown diminishing strength returns above this region. Moving toward 100% dramatically raises torque, tap wear and breakage risk while adding little useful pull-out resistance.

For a metric 60-degree thread, the familiar workshop estimate is tap drill = major diameter − pitch. Thus M8 × 1.25 suggests 6.75 mm, rounded to the common 6.8 mm drill. A more explicit engagement estimate compares the major diameter and drilled hole against the effective 60-degree thread depth. Drill runout, point walking and material spring-back mean the measured hole may not equal the drill marking.

Coarse versus fine threads

Coarse threads tolerate dirt, damaged starts and soft materials well. Their deeper form often gives better stripping resistance in aluminium, castings and short engagement lengths. Fine threads offer more minor diameter, smaller lead per turn and finer adjustment. They can suit thin walls and applications needing greater tensile stress area, but are easier to cross-thread and require closer pitch identification.

UNC is the Unified coarse series and UNF is the fine series. The number after the dash is threads per inch, so 1/4-20 advances 1/20 inch per revolution while 1/4-28 advances 1/28 inch. Never select the drill from major diameter alone. A pitch gauge and a known fastener are useful cross-checks, particularly on repaired equipment where metric and inch threads can look deceptively similar.

Adjusting the drill for material

In mild steel and free-machining brass, the listed drill generally gives a dependable cutting-tap result. In stainless, titanium and high-strength alloys, selecting the next standard drill size larger can reduce torque and galling with little loss of functional strength. For soft aluminium, adequate engagement is useful, but a hole that is too tight encourages chip packing and torn flanks. Cast iron is brittle and normally taps dry; avoid excessive engagement that can chip the tap or crumble the thread crest.

Forming or roll taps displace material instead of cutting it, so they require a substantially larger pre-hole than this chart. Their correct hole is usually close to pitch diameter and is tightly controlled because a small diameter change strongly affects formed thread height. Use the forming-tap manufacturer's chart for the exact material. Spiral-point, spiral-flute and straight-flute cutting taps can use the sizes here, subject to their maker's recommendations.

Hole preparation and drilling accuracy

Spot accurately, use a sharp drill and minimise runout. A worn drill can cut oversized, bell-mouth the entrance or work-harden stainless before tapping starts. Measure critical holes with pin gauges rather than assuming the drill produced its marked diameter. Add a small chamfer slightly larger than the thread major diameter; this guides the tap, prevents a raised first crest and makes inspection easier without sacrificing useful engagement.

Blind holes need extra drilled depth for the tap's chamfer, incomplete bottom threads and chip space. A plug tap cannot cut full-form threads to its tip. Bottoming taps reduce the incomplete length but still need clearance. Through holes suit spiral-point gun taps because chips are driven ahead. Spiral-flute taps lift chips out of blind holes. Straight-flute taps work well in short-chipping materials such as brass and cast iron.

Lubrication and tapping technique

Use a tapping compound suited to steel and stainless, an aluminium-compatible lubricant for aluminium, and usually tap cast iron or free-cutting brass dry unless the tool supplier specifies otherwise. Keep the tap square to the hole. On a machine, use rigid or tension-compression tapping appropriate to spindle synchronisation. By hand, apply steady torque with a guide; do not force a tap that suddenly tightens.

Traditional hand advice to reverse periodically can break chips with a straight-flute hand tap, but repeatedly reversing a modern spiral-flute or spiral-point tap may damage its intended chip flow. Follow the tap maker's method. Stop and investigate a rising torque trend, squeal or rough flank. The likely causes are a small or work-hardened hole, poor alignment, packed chips, incorrect lubricant, a damaged tap or the wrong tap geometry.

Tolerances and production use

These are general reference sizes, not inspection limits. Thread class, plating allowance, heat treatment and safety requirements can dictate a different pre-hole. Aerospace, pressure-boundary and other controlled work must follow the drawing, process specification and calibrated gauging plan. After tapping, verify with the specified GO/NO-GO gauge; a bolt is not a substitute because it cannot confirm pitch diameter limits.

For production, record the actual drilled diameter, tapping torque trend, gauge result and tap life. If torque is high but gauges show generous engagement, trial the next drill increment under engineering control. If threads strip in a soft workpiece, investigate engagement length and material strength rather than automatically chasing nearly 100% thread height. A longer, well-formed 65–75% thread is often stronger and much more reliable to manufacture than a short, overloaded full thread.

Frequently asked questions