Thread Turning Calculator: Speed and Passes
Cutting a thread means sinking a triangular helix into the work: the tool goes in over successive passes until it reaches full thread depth, advancing exactly one pitch per revolution. This calculator gives the spindle speed, but above all the number of passes and the infeed of each one — that is where a thread is won or lost, far more than in the choice of speed.
The passes get progressively lighter: the first one bites hard, the last ones barely skim. Because the thread form is triangular, a constant infeed would engage an ever-wider chip until the insert broke. So the passes are set for constant chip area, which gives increments that follow √i.
For a tapped hole, see the companion page: tap drill size and tapping speed.
Thread to cut
Threading terms marked with an asterisk are defined in the glossary.
Anatomy of a 60° ISO thread: H, h3, pitch diameter, root clearance
An ISO metric thread is an equilateral triangle at 60°, with the points trimmed off. H is the height of that full triangle: H = (√3/2) · P, about 0.866 times the pitch*. Nobody machines H. The crest is truncated and the root is rounded. The thread depth* fed in on an external thread is h3 ≈ 0.6134 P. An internal thread stops sooner: H1 ≈ 0.5413 P. The gap is root clearance: mating crests do not bottom in the roots, and the oil has a pocket to sit in.
H = 0.866 · P · h3 ≈ 0.6134 · P (external) · H1 ≈ 0.5413 · P (internal)
Pitch diameter* d2 (D2 on the nut) is the cylinder that meets the flanks halfway through the useful height. The fit is decided there, not on the crests. A ring gauge, or a set of wires, reads d2. A calliper across the outside of a bolt reads major diameter, which can be correct on a thread whose pitch diameter is out. The helix wanders, and the gauge refuses.
The calculator feeds to h3, or to H1 once the form is switched to internal. One extra scrape past that depth — “a bit more, to be sure” — is how a 6g becomes an 8g, and how a die loses its teeth. Depth stops at h3. A spring pass* at the same setting comes before the gauge.
Radial, flank and modified-flank infeed: what the approach angle changes
Radial infeed*, a straight plunge with the topslide at 0°, pushes both flanks at once. The chip is a V, and the load is high. On a fine pitch, in brass, on a short thread, the plunge is enough. A coarse pitch in 4140 is another matter: the tip, the weakest millimetre of the insert, does all the cutting on every pass.
Flank infeed sets the topslide at 29–30°, or calls a G76 with a 60° included angle and an infeed angle. Most of the cut sits on one flank; the other only shaves. The chip leaves as a single curl, and heat and force both drop. That is the usual CNC choice, and the topslide setting on a manual lathe. Modified-flank infeed — alternating, or zigzag — swaps the loaded flank. A notch does not grow in the same place on the insert. Coarse pitches, stainless, a thread repeated a hundred times: the swap earns its place.
A radial plunge is what the cross-slide invites. The insert was ground for a flank infeed. The table on this page keeps the chip area equal from pass to pass. Cumulative depth grows with the square root of the pass number. First pass thick, last pass thin.
depth after pass i = h3 · √(i / N)
Threading on a manual lathe: change gears, thread dial, picking up an existing thread
The leadscrew has to advance one pitch for each turn of the spindle. Change gears, or a gearbox whose plate is labelled with the pitch, set that ratio. A wrong gear cuts a tidy helix that the nut will never accept. Inch pitches on a metric leadscrew, and the reverse, need a 127-tooth translation gear or a Norton quick-change box. A 1.5 mm pitch is not “nearly” a 16 TPI train (TPI: threads per inch). The two helices diverge, and the nut jams.
The thread dial shows when the half-nut may close and put the tool back in the same groove. Even metric pitches on a metric screw often allow any line. Odd pitches and half pitches do not. Inch work on an inch leadscrew follows an even-and-odd chart: 8, 12 and 16 TPI on any line when the screw itself is 8 TPI, and 13 TPI on the numbered lines only. Where the chart is in doubt, the half-nut stays engaged and the spindle is reversed out. The withdrawal is slow, and the tool cannot pick up the wrong groove.
Picking up an existing thread — a repair, or a second operation — means seating the tool in a groove cut earlier. Marking blue, a magnifier, a jog of the topslide, a whisper of a pass, and a look at both flanks. When the faint mark on each flank is even, the setting is locked. The digital readout is set from the groove.
CNC threading: G76 and G92 cycles, lead-in and run-out lengths
- G76 — the full multi-pass cycle: first-pass depth, a minimum pass, a finish allowance, the infeed angle, a taper where the thread has one, and spring passes. Fanuc uses two blocks. Some controls pack the same idea into one block.
- G92 — each diameter is written in the part program, the way a manual lathe is wound in.
- G32 — one raw helix. The rest is written by hand: a peculiar lead, or a worm that G76 should not “help”.
Lead-in is the distance before the full thread, where the axis accelerates up to Vf = n · P. Too short, and the first millimetre is drunken: pitch error, a gauge that goes on for two turns and jams. A coarse pitch, a high spindle speed or a heavy saddle needs a longer lead-in. Run-out is the exit: a chamfer, a groove, or a programmed pull-out keeps the insert off a shoulder at full feed.
The cutting speed* fixes the spindle speed for the diameter in hand. After that choice the control stays in G97, one spindle speed locked, and not in G96. Diameter changes along a taper thread only, and on a taper constant surface speed fights the lead: the axis has to chase a spindle whose speed keeps changing. The pitch is a feed per revolution, tied to the encoder, not a millimetres-per-minute figure borrowed from a milling move.
Thread milling: one cutter for every diameter of a given pitch
A thread mill is a form cutter, solid or indexable, that interpolates a helix. One cutter at a pitch of 1.5 mm will cut M10×1.5, M12×1.5 and M16×1.5, internal, and on a different path, external. The tool drawer shrinks. A blind hole can carry a full profile closer to the bottom than a tap’s chamfer allows. A broken mill comes out in pieces that can be picked up. A broken tap stays in the hole.
The machine needs helical interpolation and a rigid spindle. The pitch is the Z advance for each full turn in X and Y, not a figure that lives only in the feed box. In a small hole the mill is a short boring bar travelling around the wall: chip thinning, a climb or a conventional path (climb on the finish), and a spring pass round the helix. Cutting speed sits higher than in single-point threading, because the edge itself is moving. The number belongs with milling speeds, not with a lathe threading speed carried over from the job before.
A tap is faster on a 500-hole plate in aluminium. A thread mill is the more sensible choice on a one-off in 17-4, a large diameter, a thin wall, or any hole that cannot be scrapped for a tap.
Dies and hand taps: when the simple answer is still the right one
A die in a stock, a tap in a tap wrench: no encoder, no G76, no toolpath. An M6 in a bracket, a stud dressed on site, a repair on a machine that cannot come to the lathe. The start has to be square, with cutting fluid on the teeth, two turns forward and half a turn back to break the chip. A die that is not square cuts a drunken thread, and every nut run on it shows the error.
A die will not hold 6g the way a single-point pass and a ring gauge will. It makes a fastener that works. A split die adjusts a little. A solid die does not. Hand taps come as a set — taper, second and bottoming — a long chamfer to start, a short chamfer to finish a blind hole. A thread on a drawing is not always a CNC cycle.
Once the drawing asks for a production 6H in stainless, the die goes back in the drawer. The hole moves to a machine tap or to a thread mill. The simple tool is the right one until the tolerance on the drawing rules it out.
Metric, UNC, UNF, BSP and trapezoidal: reading a designation and finding the pitch
M10×1.5 is a 10 mm major diameter and a 1.5 mm pitch. M10 with no pitch beside it means the coarse pitch for that diameter, 1.5 mm. M10×1 is a fine pitch. UNC and UNF are Unified inch threads, 60° like metric. 1/4-20 UNC is a quarter of an inch, 20 threads per inch, a pitch of 1.27 mm. UNF is the fine series, 1/4-28. Pitch in millimetres is 25.4 divided by the threads per inch. The form accepts threads per inch: shop drawings mix the two families.
BSP, the G series, is a Whitworth pipe thread at 55°. G1/2 is a pipe size, not a 12.7 mm major diameter, and the pitch is implied by the size — 14 TPI on a G1/2. A 60° metric insert does not cut that form. Trapezoidal Tr24×5, or a 29° Acme on an inch drawing, is a leadscrew thread: broad flanks, power to transmit, a backlash that can be measured. Different insert, different depth, different infeed. A 60° triangle is the wrong tool.
The designation is read twice. A 3/8-16 UNC bolt, 9.53 mm across with a 1.59 mm pitch, looks like an M10×1.5 on the bench. It starts in the M10 nut for about a turn and jams. The pitches belong to different families.
Multi-start threads: lead versus pitch, and how to set the feed
Pitch P is crest to crest along the same start. Lead* L is how far the nut travels in one turn. With n starts, L = n · P. A two-start thread of 4 mm pitch has an 8 mm lead: fast travel on a shallow thread, a bottle cap or a leadscrew in a hurry.
L = nstarts · P · Vf = nspindle · L
On the CNC the feed per revolution is the lead, not the pitch. Fed at the pitch, the cycle cuts an ordinary single-start thread whose lead is half the one required, and the nut will not go on. Fed at the lead, the axis moves twice as fast for the same spindle speed, which is why the lead-in grows. Indexing the next start is a spindle shift of 360°/n, or an axial shift of one pitch, depending on the cycle. The first start is checked with a gauge, or against the mating part, before the second is treated as finished.
On a manual lathe the thread dial may refuse the job. The half-nut stays closed, the tool is reversed out, and the next start is indexed from a marked chuck jaw or a dividing head. A guessed half-turn of the chuck crosses the grooves into a scroll.
Tolerance classes 6g, 6H, 4h: checking with ring and plug gauges
The number is the grade, the width of the band. The letter is where that band sits. External threads use a lowercase letter. 6g is the everyday bolt, a little under the basic size, with room for a coating and for a 6H nut that goes on over it. 4h is tighter, a precision external with less room for a zinc bath. Internal threads use an uppercase letter. 6H is the everyday nut, its lower limit on the basic size, the same arrangement as an H7 hole.
The go ring has to go. The no-go ring must not go more than a turn or two. Plug gauges tell the same story on an internal thread, and what they catch is pitch diameter. A thread that screws on by hand and tightens at the end has not been inspected. It has been lucky. Worn gauges pass scrap. A master, or a new set, settles the argument.
A 6g taken until the go gauge accepts one extra turn is already close to an 8g. A spring pass follows, and the gauge decides. The extra 0.05 mm “for luck” is how an assembly starts to rattle.
The run-out groove at the end of a thread, and why it saves the tool
A thread that runs into a shoulder needs somewhere for the insert to stop cutting. That place is the run-out groove — undercut, relief, thread relief. Width about 1.5 to 2 times the pitch, diameter at the root or under it, and a radius that does not become a stress raiser on a fatigue shaft. Without the groove, G76 pulls out on a ramp that either leaves a partial thread hard against the shoulder or drives the tip into a wall at full lead.
On a fatigue part the groove is a drawing feature, not a convenience added at the machine, and the radius is specified. On a cheap stud a chamfer and a programmed pull-out may be enough. The insert prefers the groove. A 60° tip meeting a 90° shoulder is the same class of crash as a grooving blade meeting a chuck jaw, only smaller, and more expensive per millimetre of edge.
Threading stainless and soft materials: burrs, tearing, built-up edge
Stainless work-hardens, and it welds to the tip. Cutting speed stays moderate — often 40–80 m/min on carbide, slower on high-speed steel — with flank infeed, a sharp coated edge, flood coolant on the point, and no dwell in the groove. A built-up edge* looks like a torn flank, and the gauge goes on one side only. A notch more speed, or a better oil, is the useful change. A heavier radial plunge, taken “to get it over with”, is not the remedy.
Aluminium, copper and nylon leave burrs on the crest, a fluffy major diameter, and a die that loads up. The edge has to be sharp and positive: a drop of paraffin, or a proper aluminium cutting oil, and a brush-off between passes. Plastics melt if the tool lingers. Air, a generous lead-in, and a prompt exit. A torn thread in nylon will not clean up on the nut. It grabs, and it strips.
A stainless thread is not finished by plunging the remaining h3 in one pass, on the excuse that the previous cut almost got there. The tip is a 30° half-angle on a stick. That is the pass that snaps it.
Thread rolling: the chipless method, faster and stronger
Rollers, or flat dies, squeeze the blank and the metal flows up into the crests. There is no chip. The fibres wrap the thread rather than being cut across it. Fatigue life and shear strength rise, the flank is burnished, and a dedicated roller finishes in seconds. Blank diameter sits near the pitch diameter, not the major. Too fat, and the crest splits. Too thin, and the major never fills.
External, ductile, and a production quantity: rolling wins. Hardened steel, cast iron, a one-off, an internal thread: the job goes back to cutting. A rolled thread that will be plated needs the 6g allowance in particular, because the metal is already at size. A rolled 6g blank is not “cleaned up” with a cutting program. That mix makes scrap.
Partial-profile versus full-profile inserts: one tool, many pitches
A partial-profile insert is a 60° point with a small nose radius. Within a range the same seat takes a 1.5 mm pitch, a 2 mm pitch or 16 TPI, and it does not finish the crest: the major is turned or chamfered first. A full-profile insert belongs to one pitch. It cuts flanks, root and crest for the family it was ground for — a tidier major, a stronger tip, the crest support ground in, and a separate insert for every pitch.
A jobbing shop keeps the partial profile and turns the major to size before the thread. Production of one pitch keeps the full profile. Mixing the two in a G76 without giving the cycle the nose radius is how the last pass gouges the root. The nose radius is part of h3. A 0.1 mm tip is not a 0.2 mm tip. The radius belongs in the offset, or in the cycle.
The first pass is the one that snaps the tip
Equal-area infeed makes the first radial bite the fattest, and that is the pass that meets a raw outside diameter — scale, or a weld. A 0.4 mm first infeed on a 2 mm pitch is not timid. It is what √(1/N) produces. When the insert chips, a tougher grade is not the first answer. More passes, a smaller first depth (the first-pass cap in G76), or a skin cut into clean metal come before a grade change.
An interrupted thread — a hexagon, a keyway, a milled flat — hammers that first pass once or several times a revolution. Cutting speed comes down, the pass count goes up, and a tougher grade earns a place. The feed per revolution stays equal to the pitch. The lead is the part. Speed and the number of passes are the levers left.
A light turning pass that skins the bar before the thread starts is the cheapest insurance the tip can be given.
Internal threading: bar stick-out meets a helix
An internal thread is boring with a helix added. The bar is already a cantilever, and it has to start and stop that helix without rubbing the opposite wall. The bar stays well under the minor diameter, which is the bore the thread is cut into. On a through hole the chip leaves at the front. On a blind hole the coolant comes through the bar. Modified-flank infeed leaves a curl that can be pumped out, not a V jammed in the groove.
Depth is the internal figure, 0.5413 P, when the part is the nut. The external depth, used inside a hole, is a classic overcut. This page switches when internal is selected. The number is checked before a G76 is copied from the external program. Stick-out cubes the deflection. A drunken internal thread is often a singing bar, not a pitch error in the encoder.
A blind internal needs a relief at the bottom, a thread mill, or a tap. A single-point tool cannot put a full profile into a square floor. “Thread to 2 mm from the bottom” means a chamfer length plus an honest relief, not a hope.
Catching a thread after a tool change on CNC
Once the insert is changed, the new tip is not in the old groove. On a manual lathe the topslide picks the groove up. On a CNC, if the new insert is the same height, X can stay and only Z is touched. If the heights differ, the thread is recut: Z unchanged, X starting clear, the tool brought in until the witness is even on both flanks, and the wear offset locked. G76 will not find the groove. An X error of 0.2 mm cuts a second thread beside the first.
After a crash, recovery starts from the spindle orientation — a thread-start angle, Q on some G76 blocks — or from a skim at reduced depth until the tool sits in the groove. One spring pass, and the gauge. Two helices on one shaft are scrap, not a repair.
Glossary
- Pitch
- Distance from crest to crest along one helix, P. On an ISO metric thread it is given in millimetres per revolution. On an inch thread it is often named as threads per inch, and the pitch in millimetres is 25.4 divided by that count. On a single-start thread the feed per revolution equals the pitch.
- Thread depth
- The radial height that is cut, not the full generating triangle. An external thread is fed to h3 ≈ 0.6134 P. An internal thread is fed to H1 ≈ 0.5413 P. The triangle height H ≈ 0.866 P is a construction, not a machining depth.
- Pitch diameter
- d2 on a bolt, D2 on a nut: the cylinder that meets the flanks halfway through the useful height. Ring gauges, plug gauges and wires read it. The fit depends on it. Major diameter, measured across the crests, can be right on a thread whose pitch diameter is not.
- Spring pass
- An extra pass at the same radial setting, with no added depth. It takes up the elastic give in the tool and in the work. On many threads it is the pass that lets the ring gauge go.
- Infeed
- Radial depth added on one pass. A radial infeed plunges straight in, topslide at 0°, and cuts both flanks. A flank infeed comes in at 29–30° and loads one flank. Cumulative depth after pass i follows h3 · √(i / N), and each new infeed is smaller than the one before it.
- Cutting speed
- Surface speed of the work past the edge, in m/min. With the diameter it fixes the spindle speed. Threading then locks the resulting spindle speed with G97. On carbide in stainless the band often quoted is 40–80 m/min, and high-speed steel runs slower. A thread mill is run faster than a single-point tool: the cutter’s own edge is moving.
- Lead
- Distance the nut advances in one full turn, L. On a single start, lead and pitch are the same length. On n starts, L = n · P, and the CNC feed per revolution is the lead. A two-start thread of 4 mm pitch has a lead of 8 mm.
- Built-up edge
- Workpiece metal stuck to the tip and torn off later. On a thread the flank looks torn, and a gauge may enter on one side only. Stainless and aluminium, cut too slowly, are the usual cases. A modest rise in speed, or a better oil, clears it. A heavier radial plunge does not.