Choose between tapping and thread milling using the thread, material, machine and production quantity. A process that is flexible for one job may be unnecessarily complex for another.
| Decision factor | Tapping | Thread milling |
|---|---|---|
| Basic motion | Rotation synchronized with axial feed | Helical interpolation with a smaller cutter |
| Diameter adjustment | Primarily tool and process dependent | Often adjustable through programmed path |
| Machine capability | Suitable tapping synchronization or holder | Required interpolation and validated CAM/post |
| Tool coverage | Usually tied closely to thread size/pitch | Some tools cover multiple diameters of a pitch |
| Typical evaluation | Cycle time and reliable chip control | Flexibility, size control and toolpath access |
Separate speed from total process cost
A tap can be efficient for a repeated, proven thread. Thread milling introduces an interpolation path and may take longer, but can offer useful size compensation and process flexibility. Include setup, tool changes, gauging, tool life and the consequence of a failed thread—not just spindle cutting time.
A thread mill still needs a suitable pre-hole for internal threading. Its cutting diameter must fit with enough room for the intended path. Multi-form and single-form thread mills have different coverage and programming requirements; do not assume one cutter makes every pitch.
Blind holes and chips
Check usable thread depth separately from drilled depth. Tap lead, thread-mill reach, tool neck clearance and bottom clearance all affect the feature. Chip evacuation is particularly important in blind holes. Cutting taps and forming taps are themselves different processes with different pre-hole and material requirements.
If a thread mill’s path needs a centerline feed correction, establish whether CAM has already applied it. Internal and external circular paths use different center radii. The linked calculator illustrates the simplified planar correction, not a universal helical feed command.
A practical selection checklist
Record thread specification and gauge requirement; available machine motions; material and hole depth; quantity; and acceptable cycle time. Compare actual supplier tooling options. Prove the selected program and inspect pitch diameter, full-form depth and surface condition. Neither process eliminates the need for thread gauging, and neither is universally immune to tool breakage.
Compare the same finished thread, not just tool time
For an illustrative internal thread needing 15 mm of usable full-form length, document each route’s pre-hole, drill-point allowance, tool lead or cutting-edge reach, and bottom clearance. A 15 mm drilled depth does not establish 15 mm of full thread. Obtain these dimensions from the actual tap or thread-mill drawing before comparing cycle time.
| Decision input | Tapping route | Thread-milling route |
|---|---|---|
| Size correction after gauging | Review tool limits and process; do not assume a CAM diameter edit | Check the permitted path/compensation adjustment |
| Blind-hole access | Tap lead and evacuation or forming requirements | Cutter diameter, neck reach and bottom clearance |
| Total cost | Setup, cycles, tool life, gauging and rejected parts | The same items, including programming/proving |
Why a thread mill may need a different programmed feed
In a simplified planar internal circular path, a 6 mm cutter following a 12 mm feature has a cutter-center radius of (12−6)/2 = 3 mm versus a 6 mm feature radius. If the intended peripheral feed is 300 mm/min, the corresponding center-path feed is 300 × 3/6 = 150 mm/min. This is an illustrative geometry calculation, not a complete helical-thread feed recommendation.
Sandvik’s threading application guide, page 42 explains why peripheral and centerline feed differ for internal thread milling. Confirm whether the CAM system has already applied the correction; applying it twice can produce the wrong feed. Compare a proven tap cycle and a proven milling path using the same gauge requirement and accepted quantity before deciding which route is economical.
Content updated October 8, 2026. Sources and numerical examples are explained above; examples are not production test results. Editorial method · Report a correction.
References and verification
Original explanations and worked examples by MfgWorkbench. Sources below support the stated concepts or selected reference data; they do not certify every example or a production application.
For a correction, send the page URL, the affected value and supporting documentation through our contact page.