Tap drill size calculator
Calculate tap drill sizes for metric, UNC, UNF, BSP and NPT threads. Choose cutting or forming taps and check the drill for your operation.
Select thread
FiltrosAll
Calculation inputs
Additional settings (optional)
Leave these fields blank to use the automatic settings shown in each field. You can change them to adjust the calculation.
Result
Selecciona una rosca
Select a thread and enter the threading process, material, hole type and depth. Additional settings are optional.
⚠ Indicative tap-drill calculation: it does not replace the judgement of a qualified professional. Always check the drill diameter, depth, threading method and the result on the part against the drawing, a gauge and the manufacturer's catalogue before machining.
Workshop tips and common problems
Technique selection and troubleshooting for the method Tap. Change the threading method above for specific tips.
How to do it right
Tap: spiral flute, spiral point or straight flute
A spiral point (gun tap) pushes chips forward in through holes; a spiral flute evacuates upward in blind holes; straight flutes suit short-chipping materials such as cast iron or brass. Choose the helix angle according to the material's toughness.
Rigid vs. Rigid Threading floating
Rigid tapping (G84/CYCLE84) synchronizes spindle and feed: essential on modern CNC and blind holes. The floating tap holder compensates small sync errors on older machines, but gives less depth control.
Speed and lubrication by material
Carbon steel: 8–15 m/min with cutting oil. Stainless: lower to 4–8 m/min and lubricate abundantly to avoid harshness. Aluminum: 15–30 m/min with polished or TiN core to prevent clogging. Casting: dry or with air.
Useful depth in blind hole
Leave 2–3 pitches of run-out beyond the usable thread: the tap needs room for its lead chamfer and the accumulated chips. Program the hole bottom deeper than the thread so you don't jam the tap.
Go/No-Go gauge inspection
For production valid with Go/No-Go gauge, flank micrometer (3 wires) or plane criterion. The correct drill does NOT guarantee an accepted thread - the tolerance is checked on the flank, not the diameter of the drill bit.
If something goes wrong · symptom → cause → solution
⚠ Tap broken inside the hole
Causes: undersized pilot hole, insufficient lubrication, chips not cleared in a blind hole, misalignment or unsynchronized feed. Fix: open the drill toward the recommended thread %, improve coolant, use rigid tapping and clear chips in deep cycles (peck).
⚠ No-Go Gauge enters (oversized thread)
Causes: worn or oversized tap, excessive float runout, elastic recovery of the material or a tap wrong for the material. Fix: change the tap, reduce tap-holder clearance, lower the speed on springy materials and check the tap class.
⚠ Gauge Go does not fit (tight thread)
Causes: insufficient cutter compensation, insert not reaching depth, burr on the crest or a pilot hole too large with a forming tap. Fix: adjust compensation/depth, deburr the entry and check the forming drill isn't oversized.
⚠ Entrada acampanada (bell-mouth)
The thread ends up wider at the mouth than at the bottom. Causes: tap not perpendicular, unguided start, spindle play or too much float. Fix: start with a guide or feed synchronized from the first thread, check perpendicularity and reduce tool-holder play.
⚠ Poor finish or torn flanks
Causes: high cutting speed in soft/gummy material, worn edge, poor lubrication or a last pass with too much infeed. Fix: lower Vc on aluminum/stainless, change the edge, improve coolant and add a spring pass with almost no depth.
⚠ Incomplete thread at the bottom (blind)
Causes: usable thread programmed to the bottom of the hole with no reserve, or a straight-flute tap that doesn't reach. Fix: drill deeper leaving 2–3 pitches of run-out, use a bottoming tap only for the last threads and check the real usable length.
Other threading tools
Technical guide: how to calculate the pre-drill before threading
Reference article for this section. Switch goal above (drill, identify, CNC, method, repair or base plate) to see the guide for that tool.
To choose a tap drill, first identify the thread size and pitch and distinguish cutting taps from forming taps. The recommended diameter depends on the method, thread engagement and tool; also check material and hole depth.
Find the size and pitch, choose cutting or forming and check the reference drill. Confirm hole preparation with the tap manufacturer.
Why is "major diameter minus pitch" not the whole story?
Subtracting pitch from nominal diameter is an approximation for a cutting tap: M8 x 1.25 → 8 − 1.25 = 6.75 mm. It does not establish actual thread engagement or replace a drill chart. Use the thread reference and confirm the commercial drill size with the tap manufacturer.
Our calculator starts from the ISO 68-1 geometric formula (60° triangular profile) and adjusts the result to the % of effective thread you choose, before rounding up to the nearest commercial drill bit.
Cutting tap vs. form tap: the drill size changes a lot
A cutting tap removes chips, so the tap drill is smaller (more material to remove). A forming tap does not cut: it pushes and displaces the material to form the thread, so it needs a noticeably larger drill and a ductile material (elongation >5%) to avoid cracking the crest.
If you roll in a material that does not flow well (cast iron, very hard steels), the thread may come out incomplete or cracked no matter how much you adjust the drill: in those cases, use a tap or thread mill instead.
Inch threads (UNC, UNF): number, letter or fraction drill
UNC and UNF charts express the drill as a number, letter or fraction of an inch. A geometric calculation and a commercial reference drill can differ: check the family chart and tap instructions, especially when changing thread engagement.
If the shop only has metric drills, it also gives the metric drill that works: 5.1 mm for 1/4"-20 UNC or 10.8 mm for 1/2"-13 UNC. The difference from the inch drill is a few hundredths of a millimetre.
Pipe threads (NPT, BSP): the drill comes from a table, not a formula
NPT, BSPT and NPTF are tapered threads (1:16 taper): the diameter changes along the thread and the fit is set by the number of turns to the gauge plane. So their drill does not come from subtracting the pitch but from the tap makers' tables: 1/4" NPT is drilled at 7/16" (11.1 mm) without reaming, G 1/4" at 11.8 mm and Rc 1/4" at 11.2 mm.
Never apply the metric "major minus pitch" rule to an NPT or BSPT. The calculator gives the table drill for NPT, G (BSP) and Rc (BSPT) up to 1"; for NPTF, NPS and NPSM, check against the tap maker's table and with a gauge.
Blind hole vs. intern: the margin that is forgotten
In a blind hole you must drill deeper than the usable thread length, to leave room for the tap's lead chamfer and for chips that cannot escape forwards. In a through hole the chips exit the other side and the margin needed is minimal.
A spiral-point tap (gun tap) pushes the chip forward and is the best choice in through holes at high speed; in blind holes, a spiral-flute tap that lifts the chip upwards cuts the risk of jamming and breakage.
Frequently asked questions: how to calculate the pre-drill before threading
How do you calculate the exact diameter of the threading bit?
For metric threads the base ISO formula is major diameter minus pitch, adjusted for the % of thread engagement. For example, M8 x 1.25 at 75% engagement gives a theoretical drill of 6.75 mm, rounded to the commercial 6.8 mm drill. In production, always validate with a Go/No-Go gauge.
Does the drill switch between cutting tap and rolling tap?
Yes, quite a lot: a forming tap needs a larger drill because it displaces the material instead of removing it. Using a cutting-tap drill with a forming tap usually stops the tap from forming the full thread.
What drill does an NPT or BSP thread take?
It comes from a table, not a formula. 1/4" NPT: 7/16" (11.1 mm) without reaming or 27/64" (10.7 mm) with a taper reamer. G 1/4" (parallel BSP): 11.8 mm. R/Rc 1/4" (tapered BSP): 11.2 mm. On tapered threads, the final fit comes from the number of turns to the gauge.
What drill does a 1/4"-20 UNC tap take?
A #7 drill (0.201", 5.11 mm) for 75 % thread; with metric drills, the 5.1 mm. For 1/4"-28 UNF, a #3 (0.213", 5.41 mm) or the 5.5 mm metric drill.
How much more do you have to drill in a blind hole?
As a guide, add between 2 and 4 thread pitches beyond the usable length for the tap's chamfer and chip evacuation, adjusting for the tap geometry (spiral point, spiral flute or straight flute).
What happens if I increase the effective thread percentage?
More % of effective thread gives more thread strength, but also more threading torque and more risk of breakage of the tap, especially in small taps (M3-M6) or demanding materials such as stainless or hardened steel.
Third-party trademarks and technical standards are cited for identification and descriptive purposes only; they belong to their respective owners and GetGCode is not affiliated with, authorised or endorsed by them. See the details in the Legal notice.
Related tools
Cutting parameters calculator
Cutting speed (Vc), rpm, feed and theoretical surface finish for turning, milling, drilling and threading by material and tool. A starting point.
GSM Code List
List of G and M Codes for CNC Programming. Search and filter ISO commands by control, machine or function.
CNC G-code Simulator
CNC IDE: editing with G/M tooltips, line inspector, conversion between controls and 2D/3D toolpath.