Internal Threads Have a Third and Fourth Route: Drill-Threading and Helical Thread-Forming

Internal Threads Have a Third and Fourth Route: Drill-Threading and Helical Thread-Forming｜CNC57 helical thread forming, Punch Tap, drill threading, Taptor, internal thread machining, synchronous tapping, undercut, fibre structure, form tap, thread forming https://cnc57.com/en/technical_information/Punch-Tap-and-Drill-Threading-Guide https://cnc57.com/api/cnc57/image/20260908091206872.png en 2026-09-08 2026-10-31

Internal threading is not limited to cutting and forming. Two newer routes each remove a different slice of process time: helical thread-forming compresses many revolutions of feed into half a turn, and drill-threading swallows the pilot-hole operation itself. Both carry a cost you must accept up front, and both share one non-negotiable machine requirement. This article puts all four routes side by side and states exactly where the cost falls.

1. All Four Routes, Side by Side

The difference between internal threading methods reduces to one question: how many operations does a single tool absorb? Reading down the table, each route absorbs more than the one above it.

Route	Pilot hole	How the thread is made	What this route removes
Cutting tap	Separate operation	Tap cuts the material	- (baseline)
Cold-forming tap	Separate operation	Plastic deformation, no chips	The chip evacuation problem itself
Helical thread-forming	Separate operation	Plunge to depth, then form in half a turn	The back-and-forth multi-revolution feed path
Drill-threading	Same tool	Drill point cuts the hole while the forming section behind it makes the thread	The pilot-hole operation, and the tool change in between

The trade-off between the first two is covered in Cutting Tap vs Forming Tap; this article takes up the other two. For how the operations themselves are sequenced, see Drilling and Tapping Process Guide; for the map of the whole threading line, see Thread Machining Complete Guide.

2. Helical Thread-Forming: Many Revolutions Compressed Into Half a Turn

A conventional tap, cutting or forming, must feed in one pitch per revolution all the way to depth, then unwind out the same way. The tool path equals hole depth divided by pitch, counted twice. Helical thread-forming replaces that with three moves: plunge (straight to depth, no rotation), form (a single half turn completes the thread), and retract (straight out). Half a turn is enough because of a special tooth form plus the helical groove pressed in during the plunge.

The tool itself has three sections: a reinforced punch tooth that presses the groove and steers material flow, a threading section that forms the thread in one motion, and an orientation mark so the tool is clamped in the correct position. Coolant supply is compatible with ordinary taps - both internal coolant and MQL work.

Manufacturer example: for M6 x 15 mm of effective thread depth, the tool path is roughly 1/15 that of a conventional tap, which converts to a threading cycle time saving of up to 75% (manufacturer's stated figure; test conditions and sample size were not given).

The cost is stated in the manufacturer's own table: the thread carries a helical groove mark. That is not a defect - it is the local geometry you trade for path efficiency - but the customer must know in advance that this feature is normal, or it gets rejected at incoming inspection.

3. Drill-Threading: Swallowing the Pilot-Hole Operation

What this route saves is not mainly cutting time, but the tool change. The bottleneck the manufacturer identifies is not how fast the thread is cut; it is the travel and dwell between finishing the pilot hole and bringing the tap in - non-cutting time.

This is worth remembering on its own: when someone claims a time saving, first ask whether it comes out of the main time or the auxiliary time. The two are improved by completely different means.

Step	What happens
1 Zero position	Tool waits above the workpiece
2 Drill-threading	The drill point cuts the hole while the forming section behind it threads the wall just produced
3 Transition to undercut	At the hole bottom, a relief undercut is produced
4 Reversal point	Spindle reverses
5 Transition back to thread	The forming section re-engages the finished thread
6 Exit along the thread	The tool unwinds along the thread without scoring it
7 Back to zero	Thread complete

Steps 3 and 4 are not an extra design choice - they are geometrically unavoidable. The drill point sits ahead of the forming section, so when the forming section reaches its deepest point, the drill point is already deeper; and the spindle needs a length free of thread in which to stop and reverse. Both reasons point at the same outcome: the hole bottom must carry a length without a full thread.

The way the manufacturer handles this cost is to show that it falls in a length that was never usable anyway: the undercut length corresponds to the lead-in chamfer length of a conventional tap, and a screw could never engage that length in the first place, so effective engagement length is not reduced. This is a very typical engineering argument - the cost is not eliminated, it is shown to fall inside a length that was already being given away. Evaluate it on those terms; do not simplify it into "no cost".

Manufacturer example: an M6 thread 12 mm deep saves roughly 2 seconds each. The process uses patented technology belonging to Audi AG - it is not the tool maker's own development.

4. Why High-Load Applications Favour Non-Cutting Methods

The four methods do different things to the material, and that difference carries all the way through to how much load the thread will take. The table below is drawn from the TU Dortmund study cited by the manufacturer.

Method	Material fibre structure	Effect on load capacity
Cutting tap	Fibres severed; thread profile may carry an angular error	Lower load limit, unfavourable stress distribution, reduced effective contact area
Thread milling	Continuous fibres, work-hardened material	Higher strength
Conventional cold forming	Continuous fibres, work-hardened material	- (the forming baseline)
Helical thread-forming	Continuous fibres, plus one helical groove	Comparable to cold forming

The key line in that table: the cutting tap is the only one of the four that severs the fibres. That is why aerospace and medical work tends to favour non-cutting methods - not because cutting cannot produce a conforming thread, but because severed fibres are inherently worse for load capacity and stress distribution. Another route that forms rather than cuts is Thread Whirling.

5. Two Questions to Ask Before Anything Else

First, does the machine have synchronous tapping? This is a hard prerequisite, not a recommendation; drill-threading additionally requires the dedicated tool holder from that series. Second, can the design accept the cost? Drill-threading always leaves an undercut at the hole bottom, and helical thread-forming always leaves a groove mark on the thread. If either is unacceptable, there is no point costing the rest.

Once both are cleared, the remaining boundaries:

Item	Detail
Hole type	Drill-threading works in both blind and through holes
Workpiece material	The catalogue targets cast aluminium and similar light alloys; do not extrapolate to steel or cast iron
Inspection	Thread form conforms to DIN ISO 965 and can be checked with commercial thread limit gauges to DIN ISO 1502 - no special gauging required
Strength	The manufacturer reports that first tests show strength at least equal to a conventional thread; test conditions and sample size were not given, so treat it as a stated figure
Flexibility	The more operations one tool absorbs, the more tightly it is locked to one part specification; change the size and it is a different tool

In other words, both routes earn their keep on high volumes of one repeated specification. For low-volume, high-mix work, a cutting or forming tap is usually still the better economics. For the selection baseline see Form Tap Complete Guide, and for pilot hole sizes see the Tap Drill Size Chart.

Published: 2026-09-08 | Last updated: 2026-10-31