Select the correct drill size for any tapped hole. Accounts for tapping method, workpiece material, thread engagement target, and blind hole depth requirements.
Cross-section view of the drilled hole wall relative to the full thread crest. The shaded zone represents material engaged in the thread
Moving from 60% to 100% thread engagement increases joint tensile strength by less than 5%. Tapping torque, however, increases by over 200%. For most applications, 65% in hard alloys and 75% in ductile metals delivers the optimal combination of joint reliability and tap longevity.
In tough materials like Grade 5 titanium and 316 stainless steel, thread pull-out is rarely the failure mode. Failure occurs in the bolt or at the bearing surface first. Setting engagement at 60 to 65% reduces cutting forces, extends tool life, and produces cleaner thread surfaces without sacrificing joint performance.
Standard commercial taps have 3 to 5 incomplete threads at the point lead before the full thread profile begins. Without sufficient clearance at the bottom of a blind hole, the tap contacts the floor before completing the required thread depth. Always drill to: thread depth + 6x pitch. Mark the required depth explicitly on blueprints.
For cutting taps: D = d_major – (1.082531 x P x % / 100)
For cold form taps: D = d_major – (0.5 x P x % / 100)
The constant 1.082531 derives from the ISO 68-1 basic profile: it equals twice the theoretical internal thread engagement depth, 5H/8, where H = 0.86603P.
The same geometric relationship applies, substituting threads per inch (TPI) for pitch.
Cutting: D = d – (1.082531 x %) / (100 x TPI)
Cold form: D = d – (0.5 x %) / (100 x TPI)
Since pitch in inches equals 1/TPI, these formulas are mathematically identical to the metric version and resolve to the same engagement depth ratio defined in ASME B1.1. Run both standards side by side in this calculator to confirm a converted print dimension before release to the shop floor.
In hard alloys, tap breakage is the dominant failure mode, not thread strip-out. Engagement above 65% adds disproportionate torque for negligible strength gain.
| Engagement % | Tensile strength (vs. 100% engagement) | Tapping torque (vs. 100% engagement) | Failure mode at this level |
| 50% | 91% | 48% | Tap breakage risk if material is work-hardening |
| 55% | 94% | 56% | Safe for Grade 5 Ti, 316 SS |
| 60% | 96% | 64% | Recommended floor for hard alloys |
| 65% | 98% | 70% | Recommended standard for hard alloys |
| 75% | 100% (baseline) | 100% (baseline) | Standard default, ductile metals only |
| 85% | 100.5% | 142% | No strength benefit, high breakage risk |
Standard taps carry 3 to 5 non-full-profile threads at the tip, known as the lead chamfer. If hole depth equals only the required thread depth, the lead chamfer reaches the bottom before the thread is fully formed. Adding 6x the pitch to the drill depth provides clearance for the chamfer, chip accumulation, and a safety margin against tool contact with the floor.
Mark this extended depth explicitly on the engineering drawing rather than leaving it to shop interpretation, and confirm the resulting minor diameter clearance against the part’s stack tolerance using the ISO 2768 general tolerances when the hole sits near a critical wall section.
Cold form tapping suits ductile metals with elongation above 12%, including aluminum alloys, brass, mild steel, and copper. Benefits include zero chip evacuation, a work-hardened thread surface with improved fatigue resistance, and longer tap life.
Cold form taps are not suitable for hard alloys, cast metals, or engineering plastics, since these materials lack the plastic flow needed to displace material into the thread form rather than cut it. The pilot hole runs larger than for a cutting tap at the same nominal size; this calculator adjusts the recommended drill automatically when Cold Form / Roll is selected.
The Theoretical Tap Drill Diameter is the exact calculated size from the ISO 68-1 or ASME B1.1 formula at your target engagement percentage. This value rarely matches an off-the-shelf drill.
The Recommended Stock Drill Bit is the nearest commercially available size pulled from the standard ISO metric series (0.70mm to 80.00mm) or the Imperial series (wire gauge, letter, and fractional sets).
The Actual Thread Engagement card reports the engagement percentage that stock bit actually produces once rounding is applied, which is the figure to carry onto the production drawing rather than the theoretical one.
The 75% default is a conservative legacy figure from general-purpose steel and aluminum applications, not a hard physical limit.
| Engagement % | Tensile capacity (relative) | Marginal strength gain per 5% step | Tapping torque (relative) | Tap breakage risk |
| 50% | 87% | — | 44% | Low |
| 55% | 91% | +4% | 52% | Low |
| 60% | 94% | +3% | 60% | Low |
| 65% | 97% | +3% | 70% | Moderate |
| 70% | 99% | +2% | 84% | Moderate |
| 75% | 100% | +1% | 100% | Elevated |
| 80% | 100.3% | +0.3% | 122% | High |
| 85% | 100.5% | +0.2% | 148% | High |
For fastener-critical joints, size the engagement target from the actual bolt tensile stress area in the bolted joint calculator rather than defaulting to 75% out of habit.
A cutting tap removes material to form the thread profile, so the pilot hole only needs to clear the tap’s minor diameter. A cold form tap displaces material radially outward into the thread form without removing any of it, so the starting hole has to be close to the finished pitch diameter or the displaced metal has nowhere to go.
Undersizing the pilot hole on a form tap spikes torque dramatically and is the leading cause of form tap breakage in production. This calculator’s automatic pilot hole adjustment for Cold Form / Roll selection exists specifically to prevent that error.
Most printed tap drill charts hardcode a single engagement percentage, typically 75%, and round to the nearest common fractional or metric size without showing the underlying math.
This calculator computes the theoretical diameter at your specified engagement percentage first, then separately maps that to the nearest stock bit, so any deviation from 75% or any non-standard material selection will shift the recommended size away from a generic wall chart. Treat the wall chart as a 75%-engagement special case of this calculator’s broader output, not a contradicting source.
| Material class | Tap type | Engagement % range | Elongation at thread root | Why |
| Ductile metals (Al 6061, brass, mild steel) | Cutting or cold form | 65-75% | >12% | Plastic flow supports form tapping |
| Hard alloys (stainless, titanium, tool steel) | Cutting tap only | 50-65% | 2-8% | Insufficient ductility for form tapping |
| Engineering plastics (Delrin, nylon, PEEK) | Cutting tap only | 50-60% | <2% at thread root | Cracks under radial displacement |
| Filled composites (glass/carbon-filled) | Cutting tap only | 45-55% | <1% | Fiber pullout under form tap loading |
Engineering plastics behave more like hard alloys than ductile metals: minimal elongation at the thread root makes them prone to cracking under cold form displacement. Avoid Cold Form / Roll for thermoplastics or filled composites regardless of the percentage entered.
Yes, when the field is left synced to the calculator’s default. The depth value updates automatically to the minimum engagement depth plus the appropriate chamfer clearance whenever you change thread size, tap type, or hole condition.
If you manually override the depth field, the calculator flags it as a custom value and stops auto-syncing, since at that point you are asserting a specific shop or drawing requirement that should not be silently recalculated.
Upload your 3D model to the Xometry Instant Quoting Engine for DfM feedback, material options, and pricing in seconds.
Europe 
Türkiye 
United Kingdom 
Global 
Login with my Xometry account 