Tapping drives a tap into a drilled hole, cutting the thread form in one pass; thread milling interpolates a thread mill around the hole in a helical path. The two processes are not interchangeable for every feature, and the decision is not "which is better" but "which fits this hole, this material, this depth, this coating, and this quantity." Tapping is fast and simple for common sizes in soft materials; thread milling is slower but flexible, cuts hard and tough alloys, clears chips in blind holes, and adjusts the thread for tolerance or coating. This guide gives a decision sequence for a specific thread feature, the geometry planning for blind holes, and the cost logic that includes tap breakage.
The Decision Sequence for One Thread Feature
Work through the feature in order, and the answer usually appears before the end of the list.
- Diameter and pitch. Large diameters push the tap cost up and the torque up, and standard thread mills cover a range of diameters with one tool. Above a few millimeters of pitch, thread milling is usually the practical route.
- Material. Soft, machinable materials tap well; work-hardening alloys and hardened steel break taps. If the material is Inconel, titanium, or hardened steel, thread milling is the default unless the hole is tiny and the quantity is huge.
- Hole type. Through holes clear chips behind the tap; blind holes trap them. Deep blind holes in gummy materials favor thread milling because the chips break short and clear.
- Coating and tolerance. If the thread will be anodized or plated, the coating changes the fit, and thread milling adjusts the path diameter to compensate without a special tap. If the class must hold tightly, the mill can be programmed to a size.
- Quantity and tooling. A standard size in aluminum at high volume taps faster and cheaper per hole; a mixed thread suite with several sizes favors one thread mill over a tap per size.
The sequence is a filter: the first variable that clearly rules out tapping decides the process. A large-diameter thread in 6061 still thread-mills because of tool cost; an M6 through-hole in 12L14 still taps because of cycle time.
| Variable | Lean tapping | Lean thread milling |
|---|---|---|
| Thread size | Common, small to medium | Large diameter, non-standard pitch |
| Material | Soft, free-machining | Work-hardening, hardened, tough |
| Hole type | Through or shallow blind | Deep blind, chip-sensitive |
| Coating | No coating, or special tap | Coating allowance by program |
| Quantity | High, one size | Mixed sizes, low to medium |
Blind Holes: Depth, Relief, and the Chip Problem
A blind hole changes the geometry planning. The drilled depth must exceed the thread depth by a margin that clears the tap's chamfer or the mill's approach, and the drawing should state both the thread depth and the full hole depth so the machinist can plan the tool path.
For tapped blind holes, the risk is chips packing at the bottom: the tap pushes chips ahead of the cut, and in gummy materials the packed chips stall the tap or leave a poor thread at the floor. For thread milling, the chips are short and broken, and the mill can cut to a controlled depth with a defined approach, so deep blind holes in aluminum, stainless, and nickel alloys are usually thread-milled for reliability even when tapping would be faster.
Thread relief matters at the bottom of a blind hole. A thread that must run close to the hole floor needs a recess or a chamfer that the tap or the mill can finish into, and the drawing should call out the relief diameter and depth. Without it, the thread stops short or the tool crashes into the floor, and the part is scrapped or reworked.
Coating and the Gauge Strategy
Coating changes the thread fit, and the inspection point must be defined relative to it. An anodized or plated thread grows, so a thread machined to the nominal size before coating can fail a GO gauge afterward. The two workable strategies are to machine the thread with a coating allowance, or to mask the thread before coating, and the drawing must say which.
Thread milling handles the allowance cleanly: the program adjusts the path diameter to leave the coating margin, and the same mill cuts the pre-coat size. Tapping needs a tap ground for the allowance, which is a special tool and a longer lead time. The gauge strategy follows: inspect before coating to verify the machined size, after coating to verify the final fit, or both, and the acceptance criteria should state which condition is being gauged.
The Cost of Tap Breakage
The cost comparison between tapping and thread milling is not just cycle time; it includes the failure cost. A broken tap in a part is expensive to remove, and in a nearly finished, high-value part the removal can exceed the value of the part. Tap breakage risk rises with hardness, diameter, blind depth, and chip packing, which is exactly the envelope where thread milling becomes attractive.
The honest comparison for a specific feature includes tool cost, cycle time, the expected scrap and removal cost, and the inspection method. A 20 mm internal thread in Inconel is not a tap-versus-mill question in the abstract; it is the combined risk of tap breakage, cycle time, tool consumption, inspection, and the cost of scrapping a nearly finished part. When those variables are added, the mill wins in most hard, large, or deep cases, and the tap wins on the fast, soft, shallow cases.
The cycle-time comparison also deserves a reality check. Tapping a single M6 hole in aluminum may save seconds per part, which matters at tens of thousands of parts; on a run of hundreds, the difference is minutes, and the tool flexibility and risk profile of thread milling can be worth more than the cycle saving. The quantity at which the tap's speed wins should be calculated with the actual cycle times, not assumed from the general rule.
Drawing Callouts for Threads
- Thread standard, size, pitch, and class
- Thread depth and full hole depth for blind holes, with the drilled depth
- Relief diameter and depth at the bottom of blind threads
- Coating requirement and the inspection point: before, after, or both
- Gauge method: plug gauge, pitch diameter measurement, or both
- Material grade, because the process choice depends on machinability
- Critical threads marked for gauging, with the datum and measurement setup
Conclusion
Choose per feature, not per habit: tap the common sizes in soft materials with clean chip paths, and thread-mill the large, hard, deep, coated, or high-value threads where breakage and chip packing dominate. Plan the blind-hole depth and relief on the drawing, define the coating and gauge strategy, and include tap-breakage cost in the comparison. The thread that costs nothing extra is the one whose process was decided on the feature's actual variables.
FAQs
When does a blind hole favor thread milling over tapping?
When the hole is deep and the material is gummy, tapping pushes chips ahead of the cut and risks packing or stalling at the bottom, while thread milling produces short broken chips that clear easily. Blind holes in aluminum, stainless, and nickel alloys are therefore often thread-milled for reliability even when tapping would be faster.
How do I plan thread relief and drilled depth for a blind tapped hole?
The drilled depth must exceed the thread depth by a margin for the tap chamfer or the mill approach, and the drawing should state both depths. If the thread must run close to the hole floor, add a relief diameter and depth that the tool can finish into, because a thread with no relief stops short or risks tool contact with the floor.
How does coating change thread gauge strategy?
Anodizing or plating adds thickness, so a thread machined to nominal size before coating can fail a GO gauge afterward. Machine with a coating allowance or mask the thread, state which on the drawing, and decide whether inspection happens before coating, after coating, or both.
What does a broken tap cost versus switching to thread milling?
The cost is the removal of a broken tap from a part, which can exceed the part's value on nearly finished, high-value components, plus scrap and schedule impact. When tap breakage risk, from hardness, diameter, depth, or chip packing, is added to the comparison, thread milling wins on the risk profile even where its cycle time is longer.
Sources
- 6CProto CNC Machining Services
- 6CProto CNC Milling Services
- 6CProto Standards and Tolerances
- ISO 2768-1:1989 – General tolerances for linear and angular dimensions
- ISO 9001:2015 – Quality management systems