Internal-thread machining engine for manufacturing and process engineers: 75 % tap-drill sizing for metric and UNC threads, material-based tapping speeds with RPM and feed, empirical tapping torque and spindle power, and full thread-milling kinematics — cutter RPM, feed per tooth, and the corrected table feed Ftable = Ftool·(D−d)/D for helical interpolation — checked against machine RPM, torque and feed limits. Every input with selectable universal units and reference-standard values, every report with the full audit trail.
SectorCalc SC-022 plans internal-thread machining by cut tapping or thread milling. The engine resolves the 75 %-engagement tap drill for metric coarse and UNC threads, applies a material-based cutting-speed database to return spindle RPM and feed, estimates tapping torque and spindle power, and for thread milling computes cutter RPM, feed per tooth and the diameter-corrected table feed that helical interpolation cycles actually require. All results are checked against your machine's RPM, torque and feed limits. Results are reference-grade process estimates — final parameters must be proven out on the machine with the tool manufacturer's data.
A 75 % thread engages nearly the full strength of a 100 % thread while cutting torque drops by a factor of three — below roughly 60 % engagement the gain in strength is negligible while tap breakage risk climbs sharply. The engine returns the theoretical 75 % drill and the nearest standard drill at or above it, with the resulting engagement percentage.
Cut taps are HSS tooling: the material database caps cutting speed at 4–25 m/min depending on workpiece material. Feed is not free — one revolution advances exactly one pitch. Rigid (synchronous) tapping holders are mandatory above ~M12 or 1000 rpm; tension-compression holders absorb pitch error below that.
Tapping torque is dominated by friction and chip packing, not by the metal removed — the empirical cubic law above reproduces shop measurements within ±50 % across M3–M30. Use it for machine-limit screening, never as a guarantee: worn taps, poor lubrication or stainless work-hardening can double it. A 50 % reserve against the machine torque limit is enforced as a warning.
Thread milling runs carbide at 80–250 m/min — five to ten times tapping speed — with feed per tooth of 0.03–0.08 mm. Cutter diameter is limited to about 0.70×D for coarse pitches so the tool clears the minor diameter at full depth; larger pitches need multiple radial passes.
The programmed centreline feed must be reduced because the cutting edge travels a longer path than the tool centre. Programming the centreline at full peripheral feed over-feeds every tooth and is the single most common cause of broken thread mills. The engine returns both values — program Ftable, verify Ftool against the tool card.
Required RPM, torque and table feed are checked against the machine limits you enter. Exceeding the spindle RPM or the axis feed rate is blocking; torque is screened with a 50 % reserve because the empirical model scatters. Large taps in rigid holders at low RPM can stall spindles that look adequate on paper — check the continuous-torque curve at the working speed, not the peak rating.
Chip evacuation, almost always. Beyond 2.5×D depth in a blind hole the engine warns: switch to spiral-flute taps, reduce speed 20 %, peck-tap, or move to thread milling where chips are small and evacuation is intrinsic.
Above M16, in hardened or expensive workpieces, and wherever a broken tap would scrap the part. One thread mill covers a diameter range and both hands of thread, produces a better surface, and a broken mill never wedges in the hole.
No — it is the strength/torque optimum for general work. Thin sheets often use 60–65 % engagement drills for extrusion (forming) taps, which this engine does not cover: forming taps need a larger drill and generate no chips.
Within ±50 % for sharp HSS cut taps in the listed materials with proper lubrication. Roll/form taps run 30–50 % higher; worn taps, dry cutting and work-hardened stainless can exceed the band. That is exactly why the machine check carries a reserve factor.
