Tap Drill Size and Tapping Speed Calculator
Tapping is the one machining operation where the tool breaks inside the workpiece — and where breaking it ruins the part as thoroughly as the tap. Three numbers decide how it goes: the tap drill diameter, the torque needed to form the thread, and how much the tap can take before it snaps. This calculator gives all three.
The tap drill size is not a convenient rounding: it is what sets the thread engagement percentage. Going from 77% (the familiar “diameter minus pitch”) to 100% raises the torque by roughly 40% — and the risk of breakage with it — for less than 5% more thread strength. It is the worst trade in all of machining.
For an external thread or one cut on a lathe, see the companion page: thread turning speed and passes.
Thread to tap
An asterisk marks a tapping term defined, once, in the glossary.
Reading a tap drill chart, and why “diameter minus pitch” works so well
A cutting tap is not asked for a 100% thread. A full sharp internal is how the tool snaps in the hole. On a 60° thread — metric, and Unified as well — the cutting-tap shortcut is one line.
Dtap drill = D − P
Read down the nominal size, across the pitch, and the cell is the drill. M10×1.5 lands on 8.5 mm. M8×1.25 lands on 6.8 mm. M6×1 lands on 5.0 mm. That hole leaves about 75% of the theoretical thread height, or 76.98% when the factor this calculator uses is applied exactly. Pull-out strength sits close to the full-thread figure. Torque on the tap is not. Printers differ in the last rounding, to the nearest 0.1 mm or to a letter drill, and underneath it is the same rule.
The shortcut ceases to be the drill on a form tap*, on a pipe thread, on a 55° Whitworth, and on a 100% thread written onto a drawing out of caution. Those four belong in the percentage box. For a bog-standard metric coarse thread in steel, D − P is what the drawer is labelled for, and the labels have lasted because the hole works.
A drill 0.1 mm under that figure is not a slightly stronger thread. Torque jumps, and breakages with it.
Thread engagement percentage: the trade between pull-out strength and broken taps
Thread percentage* is the fraction of the V-height the nut carries. 100% is the theoretical sharp internal. 75% is the everyday cut. 50–60% is the sensible band in a hard material, on a small tap, or on a job where a tap that comes back out is worth more than a heroic shear area.
thread % = 76.98 · (D − Ddrill) / P
Shear strength of a steel fastener sitting in a steel nut flattens past about 60–70%. The extra 30% of engagement buys little further pull-out and a great deal of torque. In aluminium, or in a thin boss, 70–75% together with a longer engagement (1.5 D of thread) beats a 90% thread cut in a 0.8 D boss. Once the curve has left its steep part, depth does more than percentage.
The result table at 60 / 65 / 70 / 77 / 85 / 100% is that trade set out in numbers. The 77% line is the D − P hole. Relative torque rises with the annulus the tap has to remove, everything else held equal. 100% in 316 on an M6 leaves the tap in the hole. 65% in 316 on an M6 is a part that leaves the shop.
Hand taps, machine taps and forming taps: three ways to make a thread
Hand taps are a square on the shank, a tap wrench, and a set of three. The taper, with an 8-thread chamfer*, starts the hole square. The plug, with a 4-thread chamfer, covers through holes and most of the ordinary work. The bottoming tap, on 1–2 threads of lead (1.5 on the selector here), finishes a blind hole. Torque arrives in the wrist. That feel is the safety system. Slow and cheap, and the right kit for a single hole held in a vice.
Older British lists call the medium lead a second tap and the short lead a plug. The selector here prints taper, plug and bottoming, and the counts to trust are 8, 4 and about 1.5. A longer lead thins the chip on each tooth and lowers the torque, taking more depth before the first full thread. A short lead reverses that: a thicker bite, and a full thread closer to the floor.
Machine taps carry a shorter lead, a shank for a chuck or a holder, and on many of them a coating. They expect a spindle that can reverse, a fluid, and a hole drilled on size. They do not survive the wobble of a worn drill-press chuck pressed into service as a tapping head at 800 rev/min in stainless.
Forming taps — roll taps, fluteless — carry lobes, not flutes. The lobe pushes the drilled wall out into the flanks: no chip, a stronger burnished thread, and a larger drill, about D − P/2 for a 75% form. Cast iron will not flow; it powders and jams. Aluminium, mild steel and a lot of stainless will form on a rigid machine with the right oil. Offered a cutting-tap drill, the same tap behaves as a punch.
Straight flute, spiral point, spiral flute: where the chip goes in each case
- Straight flute. Chips fall where they fall, or they pack. Brass, cast iron, a short through hole, a hand tap.
- Spiral point* (gun tap). The point drives the chip forward and out of the exit of a through hole. Fast, modest torque, the usual machine tap for a through hole. In a blind hole the same point packs a nest on the floor, and the tap comes back in pieces.
- Spiral flute. The helix draws the chip back up the hole, past the shank. 15° suits an ordinary blind hole; 40° and steeper suits a deep hole in gummy stock. The last full thread can sit closer to the floor than a gun tap reaches, the lead being free to stay short once the chip is no longer stuffed forward.
A spiral flute in a through hole in iron will cut. Clearing is slower, nothing more. A gun tap in a blind stainless pocket is the familiar snap at about 90% of the depth. Depth was not the cause. The chip had run out of places to go.
Rigid tapping versus a tension-compression holder: synchronising spindle and axis
Rigid tapping* — synchronous, G84 on a mill whose spindle carries an encoder — holds feed and rotation together on the way in and on the reverse out. The holder is solid. Pitch is a number in the program, on a machining centre or a turning centre with live tooling, or on any spindle that reverses without losing the count. No spring travel remains to eat into a blind hole.
Vf = n · P
A tension-compression holder is a spring. It forgives a spindle that is only approximately in step with the pitch: a drill press fitted with a tapping attachment, an older control whose feed is merely close, a worn leadscrew. The tap finds the pitch. The holder breathes a few millimetres. Depth becomes less certain. A machine that cannot rigid-tap needs that float. A machine that can has no use for it, but extra float on a rigid cycle is how a tap walks out of a collet or runs on through a blind floor.
An alarm on the G84 reverse points at the encoder, or at a parameter. It does not point at a richer feed. Feed is the pitch. There is no second number to “improve”.
Form tapping (chipless): a different drill size, and a stronger thread
The form tap’s drill is larger, the metal having to come from the wall that will become the flank. A common size for a 75% form is about D − 0.5 P, sometimes published as D − 0.45 P to 0.5 P according to the maker. An M10×1.5 form drill sits near 9.25–9.3 mm, not 8.5 mm. An 8.5 mm hole in front of that tap asks the lobes to displace a wall that is not there. Torque spikes, the tap welds to the work, and the hole work-hardens* into scrap.
The gains are no chip packed in a blind hole, a cold-worked flank, better fatigue life, a size kinder to a 6H* gauge, and a tap that keeps cutting while the oil film holds. It calls for ductility, a hole round enough to start on, a true EP oil or a paste specified for forming, and a spindle that does not hesitate. Forming aluminium with no oil galls a lobe, and the afternoon goes into an extractor.
A 75% cut thread in a long steel nut is already stronger than the bolt it holds. Forming earns its place in aluminium, in a thin wall, in a blind hole that must stay free of chips, and in stainless where a cutting tap has been dying. It is the wrong tap for GJL-250.
Removing a broken tap: extractors, EDM, and why prevention is cheaper
A broken tap is hard, fluted, and lodged in a hole the part needs. A square extractor of the easy-out type, seated in the flutes and turned in reverse with oil and patience, works when the tap is loose and the flutes are open. It works poorly when the snap came from too much torque: the stub left behind has become a wedge. A left-hand drill can open the core, where a core remains. Heat on a steel part is available when the drawing allows it. None of those routes looks acceptable inside a finished aluminium housing.
Sinker EDM burns HSS or carbide out without machining the parent metal. Costly per hour, it remains cheaper than a replacement housing. A carbide tap in a steel block is an EDM job almost at once. Extractors skate on carbide.
Prevention is a drill on size, a spiral matched to blind or through, oil on the tap, a speed that does not die mid-thread, a 70% thread in a difficult material, and a tap started square to the hole. Left to chance, tapping stays the cheapest line on the routing until the tap that dies at 16:40 on a 200-part run.
Tapping lubricant: paste, cutting oil, and the special case of gummy aluminium
Taps fail from heat and from welding. They do not fail from a shortage of coolant colour. A paste — sulphur, chlorine, or a modern EP compound without that smell — clings inside a hand-tapped hole. Neat cutting oil on a machine tap is the usual film for steel and for stainless. Emulsion will serve on aluminium through-holes at a proper speed, when the tap is coated and the hole is short. In a blind stainless hole the same emulsion is a weak film: most of it is water.
Gummy aluminium is its own case. 6061, 6082, and anything else that smears, can be stained by a sulphur paste. A tapping oil made for aluminium, or a rapeseed-based fluid, suits it, with a polished or bright tap, TiN or TiCN if either is on the shelf, and a spiral flute that lifts the chip. A coated tap run dry in aluminium beats a dull HSS tap standing in a puddle of the wrong fluid. Loaded flutes are cleared before the tap goes back in. A loaded tap cuts like a reamer for a moment, and snaps.
Cast iron is run dry, or with a single drop of oil. The chips are short and a straight flute is enough. Titanium wants the paste used on stainless, only more of it, and a lower speed. The open bottle has to match the metal, not whichever cap was off.
Tapping stainless: work hardening, constant speed, never stopping mid-thread
304 and 316 harden under a rubbing tap in the same way they harden under a rubbing drill. The edge has to cut. Polishing the surface is how the next tooth meets a harder skin. The workable combination is a moderate cutting speed — often 5–10 m/min on HSS, a little higher on a coated tap — a form tap where the hole and the oil allow it, a cutting tap held at 65–70% thread where they do not, and a motion that never parks in the cut. A hand tap rested in the hole “to feel it” sits there pushing the surface towards 40 HRC before the next tooth arrives.
The rigid cycle goes in and reverses straight out, with no dwell on the floor. A stalled motor means the hole is the wrong diameter or the flute is packed. Retract on the reverse and clear the chips before any question of a drill 0.1 mm small. Forcing through the stall is how the tap stays in the hole and the part goes to the EDM shop.
A 100% thread programmed in austenitic stainless does not make a stronger boss. It makes a tap shank, and a job for the EDM shop.
Tapping blind holes: dead space, pecking, the last full thread
Every tap has a lead. The first full thread lies that many pitches above the point. A bottoming tap, on a 1.5-thread chamfer, needs room for chips and for the point itself. The hole is drilled past the last full thread that the drawing cares about. Dead space of 1.5–2 × P is a starting habit, and more of it when the chips are long. The minimum drilling depth on this page is that sum, lost floor included.
Spiral flute, a paste or an oil that stays down at the bottom, and on a deep hole a hand-tap peck: out, clear, back in. A CNC rigid cycle can peck as well. Every reverse can drag a chip under the first full thread and gall the flank. A single stroke avoids that once the drill, the flute and the dead space allow it. A gun tap in a blind hole remains a poor idea, however elaborate the cycle looks.
The last full thread on the drawing is three things at once: a depth, a chamfer, and a gauge. Where the go side of the plug must reach a shoulder, the tap has to be a bottoming tap and the hole has to have been drilled to suit it. A plug tap will mislead. The thread looks finished, the last two pitches are lead, and the stud seats on chamfer.
Thread inserts (helical coils): repairing or reinforcing a thread in soft material
A helical coil — the everyday name is a trade mark — seats a stainless spring in a larger tapped hole, and the bolt meets steel. Aluminium housings, a stripped M6 in a cover, a repair after the broken tap has come out: the drill comes from the insert chart, not from D − P of the nominal size. The hole is drilled to that chart, cut with the matching STI tap*, and the coil is wound in. Where the style has a tang, the tang is broken off. The nominal bolt fits after that, not before.
The plain tapped hole is the weak one. In a thin aluminium boss the insert is the difference between a 4 Nm specification and a stripped hole at 3. In steel the coil is mostly a repair. Length of coil — 1 D, 1.5 D, 2 D — is pull-out, and 1.5 D is the usual pick. A coil wound into an oval hole becomes an oval coil. The hole is trued first, bored or bushed, and tapped for the insert only after that.
A form tap and an STI chart do not mix. The insert tap is a cutting tap, and its diameter is its own. Where the stripped hole has also wandered off axis, a boring bar is what brings the axis back before that tap goes in.
Checking with a plug gauge and the 6H tolerance class
The go plug carries a full thread and has to enter to the required depth by hand. The no-go is a short thread and must not enter more than 1.5–3 turns. 6H is the everyday internal class, made to sit with a 6g screw. 4H is tighter, a special, and a hole cut small will refuse a 6H go. That is the opposite mistake from a loose 7H into which the no-go sails.
A bolt taken from the bin only shows that some 6g happens to enter. It is not a 6H check. A worn go passes a small hole; a worn no-go starts rejecting good ones. Gauges stay marked, and they stay off the chip tray. A tapped hole that accepts both plugs is large: the tap ran out of square or wobbled in its holder, it carried a built-up edge, or a formed hole was over size. A worn tap does the opposite and cuts small.
Aluminium brings temperature into the same check. An aluminium hole gauged warm at 4 pm is larger than it will be the next morning: a go plug that entered then can refuse once the part is cold. Size is read at the temperature the part ships at, or the morning disagreement is built in.
Spindle RPM and tap feed: the pitch is the feed
There is no chip load to choose. One revolution of the spindle, one pitch of travel. Cutting speed sets the revolutions in the usual way, n = 1000 · Vc / (π · D), and the feed follows, Vf = n · P. An M8×1.25 at 8 m/min is about 320 rev/min and 400 mm/min. Keying 800 mm/min, on the grounds that the figure resembles a small end mill, either draws the tap out of the holder or turns it into a grim sort of thread mill.
Inch taps obey the same relation, written with TPI. Feed in inches per minute equals RPM divided by TPI. A 1/4-20 at 400 RPM wants 20 inches/min. A dual-mode control will perform the conversion when it is allowed to, and will commit a 25.4-fold error when pitch and TPI are mixed up. P or TPI belongs on the setup sheet beside n. The bare code G84 does not carry the pitch.
A single-point thread uses that same Vf = n · P. The tap is the helix with twenty teeth in a row, and with no second pass to correct the first.
Metric coarse versus fine: the tap drill moves more than habit suggests
M10 is not one drill. M10×1.5, the coarse pitch, takes 8.5 mm. M10×1.25 takes 8.8 mm. M10×1 takes 9.0 mm. M10×0.75 takes 9.3 mm. The hole grows as the pitch grows finer, D − P shrinking with P. Remembering “M10 is 8.5” puts a fine-pitch tap into an 8.5 mm hole. On a 1 mm pitch the formula above returns more than 100%: the tap is asked for a full sharp thread and more, and the torque belongs to a different job.
Fine pitches are shallower. Pull-out per turn is lower. A thin wall prefers them. They turn up on adjusters, on a length of thread along a shaft, and in a hard material that will not accept a coarse tap. Each pitch wants the drill printed next to it. A shared sleeve marked only “M10”, full of 8.5 mm drills, is a coarse-pitch drawer. Fine-pitch drills left unlabelled vanish into that drawer.
75% of a fine pitch removes less metal than 75% of a coarse pitch. On a short boss, a coarse thread or a coil beats a fine thread pushed to 90%.
Left-hand threads and the reverse cycle
Left-hand taps keep a shaft from unscrewing in service: a grinding-wheel arbor, a left-hand turnbuckle, a gas fitting under some standards. The drill diameter does not change. The spindle direction does. Rigid tapping runs a left-hand cycle, or the holder is arranged for the reversed tool. The tap winds in on reverse and comes out on forward, or the control swaps the M04 and M03 pair inside the cycle. With that pair reversed the wrong way, the tap winds inward until it has become a stud.
A left-hand spiral flute looks like a right-hand one when the job is rushed. The stamp on the shank reads LH. The plug gauge is LH as well. A 6H go plug of the ordinary right-hand sort tells nothing useful in a left-hand hole, except that the wrong box is open on the bench.
Pipe threads (NPT, BSPT): taper, dope, and a different drill chart
NPT and BSPT are both tapered at 1:16, ¾ inch per foot on the diameter, but the thread angles differ: 60° for NPT, 55° for BSPT. The drill chart is not D − P. The tap is a taper tap, and the seal is made on the flanks. An NPT hole opened with a “near enough” metric jobber either leaks or splits the fitting. The sequence is the pipe-tap drill, the taper tap, and dope or PTFE on the male thread. A pipe thread has no 6H. It has L1, L2, a count of turns to make-up, and a pressure test.
Parallel BSP, the G series, is a different thread again: 55°, a fastening thread, often closed by a washer or an O-ring. A 60° metric insert, or a metric cutting tap, run into a G hole is a leak with extra operations attached. A drawing that reads R, Rc, G, NPT or 1/4-18 is a reason to set this page’s metric 75% aside and open the pipe chart. Torque and breakage follow the same physics. The diameter does not.
A pipe tap in dry stainless repeats the metric story, except that the tap costs more and the hole usually sits in a manifold. It needs oil, a taper that matches the standard named on the drawing, and the pipe-tap drill size. A hole made deliberately small, in the hope of a tighter seal, is how a taper tap becomes a taper reamer and, a moment later, a taper stub.
Glossary
- Thread percentage
- The share of the full sharp V present on the internal thread. On this page it is 76.98 · (D − Ddrill) / P. 100% is the theoretical sharp form; the everyday cutting-tap hole sits near 75%.
- Chamfer
- The tapered lead at the tip of a tap, counted in threads. Eight threads on a taper tap, four on a plug, about one and a half on a bottoming tap: a longer lead shares the cut over more teeth and lowers the torque, at the cost of unused depth in a blind hole.
- Form tap
- A fluteless tap whose lobes displace metal into the flanks rather than cutting a chip. The drill is larger than the cutting-tap size, about D − P/2 for a 75% form, and the metal has to be ductile enough to flow.
- Spiral point
- Gun-tap geometry. An angled point at the end drives the chip forward, out through the exit of a through hole. In a blind hole that chip has nowhere to go and packs against the floor.
- Rigid tapping
- A cycle, G84 on a mill with a spindle encoder, that locks feed to pitch: Vf = n · P, both into the hole and back out. The holder is solid. Pitch is not left to a spring.
- Work hardening
- A rise in hardness where the surface is rubbed or deformed instead of cut cleanly. Austenitic stainless does this readily; a tap that pauses in the hole can leave a skin near 40 HRC for the following tooth.
- STI tap
- The cutting tap used before a helical coil insert. It is larger than the tap for the nominal bolt. The drill comes from the insert chart, not from diameter minus pitch.
- 6H
- The everyday ISO tolerance class for an internal metric thread, meant to mate with a 6g screw. A go plug must enter to depth by hand; a no-go must not go beyond 1.5–3 turns.