Threading Tools

Threads are formed one light pass at a time, not in one plunge. Single-point threading, thread milling and tapping each use a different tool, and the infeed method decides whether the insert chips. This page covers pitch, multiple passes and infeed in plain terms.

Concept

A thread is a helical groove cut to a pitch. Three ways to make it: single-point threading (a V-shaped insert traces the helix on a lathe, over many passes), thread milling (a rotating thread-form mill interpolates around a hole), and tapping (a tap cuts internal threads in one tool). The key idea: the full thread depth is built up over several shallow passes, because the insert cannot take the whole thread depth in one plunge.

Why It Matters

Threads fail by chipping because the tool rubs and overheats near the end of each pass. Two design choices control this: how deep each pass cuts (decreasing pass depth so total chip load stays sane) and how the insert feeds in (radial infeed loads both flanks; flank infeed cuts one side at a time and runs cooler). Get the infeed wrong and the insert chips before the thread is finished.

How It Works

Single-point threading passes

The first passes cut most of the depth; each later pass cuts less. The insert must retract at the end of each pass before returning, to avoid dragging on the finished thread.

Infeed methods

Thread milling vs tapping

Tapping is fast for standard internal threads but a broken tap in a hole is costly. Thread milling is flexible for large or tough holes and avoids tap-break risk, but needs a milling machine with helical interpolation.

Worked Example

Cut an external M10×1.5 thread on a lathe. The pitch is 1.5 mm per turn, so the Z feed equals the pitch. The full thread depth is reached in several decreasing passes rather than one. Use flank infeed in steel so the chip flows and heat stays manageable; retract at the end of each pass. The same thread could be tapped if internal, or thread-milled on a machining center for a large blind hole.

Threading at a glance

Threads are produced several ways: single-point turning on a lathe, taps for internal threads, and thread mills for larger or harder holes. Each cuts the same fundamental geometry — pitch, major/minor diameter, thread depth — but at very different productivity and setup cost. A tap is quick for standard holes but can snap if chip evacuation is poor; thread milling is flexible and avoids tap breakage in hard material; single-point threading is most controllable for odd or large forms. The critical machining detail is that feed equals the pitch per revolution, so the machine's feed and spindle are locked together. Whatever the method, start with the thread form and size from the drawing, then choose the tool that fits the machine and batch size rather than the other way around.

The tap-drill size you must set first

An internal thread is only as good as the minor (tap-drill) diameter you start with. Drill it too large and the tap has too little thread engagement; drill it too small and the tap is overloaded and snaps. For a metric thread, the common rule of thumb is tap drill diameter ≈ major diameter − pitch. For the M10×1.5 worked thread that gives roughly 10 − 1.5 = 8.5 mm pre-drill, which is why an 8.5 mm drill precedes an M10×1.5 tap. Get this backwards and no amount of speed or pecking saves the thread: a tap forced through an undersized hole breaks, and one through an oversized hole produces a thread that strips under load. This is the first decision in any tapping program, before spindle speed or peck cycles are chosen, and it links back to the drill and point-height planning on page 17 and the hole-quality ladder on page 18.

Why feed must equal pitch per revolution

In ordinary turning, feed per revolution sets how fast the tool advances relative to the cut; in threading it is locked to the thread pitch, not chosen. For an M10×1.5 thread the tool must advance exactly 1.5 mm for every one spindle turn, or the helix it traces does not match the pitch and the thread is ruined. This is why a lathe in threading mode synchronises the Z feed to spindle position rather than running an arbitrary feed rate, and why the spindle speed must be chosen carefully: too fast and the synchronised feed stretches or the tool cannot keep up, especially near the end of a long thread where acceleration and deceleration matter. It is also why a single-point threading pass must retract at the end before returning — on the return traverse the feed is no longer tied to the helix, and dragging the same path would scrape the finished flank. This pitch-locked feed is the fundamental difference between threading and any other turning operation, and it is why the thread program re-starts each pass in phase with the spindle rather than as a plain linear move.

Why a broken tap is feared, and how to avoid it

A tap failure is uniquely costly because the tool is inside the part when it snaps: a broken tap in a finished or near-finished hole often means scrapping the whole component, whereas a broken end mill can be pulled out and replaced. That asymmetry is why tapping has three design safeguards. First, the pre-drill (tap-drill) must be right — an undersized hole overloads the tap and is the most common breakage cause. Second, chip evacuation must work: in a blind hole, trapped chips bind the tap, so a spiral-flute or gun tap, or a peck cycle that retracts to clear chips, is required rather than a straight-flute tap run to the bottom. Third, tapping runs at much lower speed than drilling — the tap cuts a formed thread with weak chip flow and limited room to cool, so pushing spindle speed is a direct path to welding and snapping. This is exactly why thread milling exists for tough or large holes: it trades a rigid tapping operation with breakage risk for a milling cycle that cannot lock up inside the bore. When a tap breaks repeatedly, the diagnosis follows page 27 — pre-drill size first, then chip evacuation and speed, not a harder tap.

Why each later pass cuts less than the last

A threading pass is a V-shaped groove being widened incrementally, and the chip cross-section does not stay the same even if you took the same radial bite every time. If every pass plunged the same depth, the cutting edge would be engaged over a growing length of thread flank and the chip would swell, overloading the corner and heating the insert — which is why threading inserts chip toward the end of a long thread. The standard answer is decreasing infeed: the first passes take a meaningful bite, and each successive pass removes a smaller radial amount so the actual chip thickness stays roughly constant. This is the same logic as a chipbreaker window (page 06) applied to a groove: the edge wants a steady, manageable chip, not a growing one. It also means the number of passes is not arbitrary — the insert catalog prescribes the infeed schedule for the thread pitch and material, and a program that uses too few, too deep passes forces the edge to carry a chip it cannot break. When a threading insert wears fast or chips, check the infeed schedule before blaming speed; a too-coarse later pass is a common cause that the pass-count table exists to prevent.

Why threading runs at far lower RPM than turning

It surprises new operators that a threading pass uses a much lower spindle speed than the turning passes on the same part, and the reason is not that the edge needs more care — it is the pitch-locked feed. Because the Z axis must advance exactly one pitch per revolution, the feed rate (mm/min) is directly proportional to RPM: at 1000 RPM with a 1.5 mm pitch the tool travels at 1500 mm/min, and doubling the RPM doubles that synchronized feed. Two limits then cap the speed. First, the machine's feed and axis acceleration must keep up with a feed locked to the helix, especially at thread start and end where there is a short ramp before and after the cut; too fast and the first and last threads are out of phase. Second, the threading insert has a weak chip and limited clearance in the V-groove, so it generates heat quickly and wears if the surface speed climbs to normal turning values. The practical rule is to compute the threading RPM from a conservative surface speed for the thread insert, well below the turning speed of the same grade, and to leave a short overtravel at both ends so the helix is fully engaged before the cut reaches the shoulder and disengages before the tool decelerates. Low RPM here is a synchronization and heat constraint, not a sign that the operation is "slow work".

Why the thread depth is not just the pitch

It is easy to confuse pitch (the distance between threads, 1.5 mm on the M10) with how deep the V-groove must be, but they are different numbers. The thread depth is set by the 60° profile and the pitch, working out to a small fraction of the pitch — roughly 0.6 times the pitch for a standard metric form, so about 0.9 mm deep for M10×1.5. This is why a pass schedule is measured radially inward by that depth and not by the pitch, and why the tap drill at 8.5 mm leaves material in the minor diameter for the thread to form without going all the way to the major diameter. Getting this straight prevents the two most common setup mistakes: taking the tool to the full major diameter on the first pass (over-depth), or stopping short because "the pitch was 1.5 mm so we went in 1.5 mm." The drawing and thread standard define the depth; the pitch only sets the helical lead that feeds per revolution. Threads are geometry, and the geometry has to be calculated rather than approximated.

Why thread milling is the flexible alternative

Where a tap is a fixed-size tool — one tap per thread size — a thread mill is a multi-flute cutter that, by adjusting its helical path, can cut a range of pitches and diameters in the same material. That flexibility is the main reason it exists. On a large internal thread, buying a large tap is expensive and a broken one inside a big part is catastrophic, whereas a thread mill already on the shelf can be programmed to the required helix. In tough material where a tap would weld and bind, the thread mill cuts like an end mill, evacuating chips in controlled arcs and never locking into the hole. The trade is that it needs a machining centre capable of helical interpolation, and it runs several programmed arcs rather than one fast plunge — so it is slower than a tap on a simple, small, standard hole. The choice therefore follows batch and risk: tap a standard through-hole in easy material fast; thread-mill a large, blind or tough hole where tap breakage would be expensive. This page pairs the two so the tap-break fear above has a designed alternative rather than a workaround.

Threading is a multi-pass cut where every pass re-enters the same groove. Tool wear or a slight deflection on an early pass shows up as a thread that will not gauge later, so the edge condition and the programmed depth both matter. A worn threading tool produces undersize or torn threads that are easy to misread as a depth error; check the edge before adjusting the last pass.

Common Mistakes

• Taking the full depth in one pass. The insert overloads and chips. Fix: multiple decreasing passes.
• Using radial infeed on a tough alloy. Overheats both flanks. Fix: flank infeed.
• Forgetting to retract before returning. Drags on the finished thread. Fix: program the retract at each pass end.

Match the threading speed to the material and the tool, and remember that feed equals the pitch per revolution — any drive or screw error shows directly on the thread. Use the programmed infeed strategy, keep the edge sharp, and verify the first thread with a gauge before running the batch.

Practice