Helical thread milling for internal and external threads: spindle speed, the feed to program at the tool centre so the cutting edge gets the right chip, helix radius, radial passes, milling time and the helical toolpath. Metric, UNC and UNF, single-profile or multi-row thread mills.
Saved in this browser only. Use Export to keep a file you can back up, share or import on another computer.
Starting values: take the cutting speed, feed per tooth and number of radial passes from the thread mill maker for your material.
| Pass | Cut to Ø | Radial step | Helix R (I) | Z start | Z end |
|---|
The radial passes, spindle speed and feed are starting values: take the cutting data for your material from the tool maker.
Basic profile shown. Cutter radius compensation is not used (G40). To adjust thread size, change the radial depth / helix radius and re-check with a thread gauge.
The clearance plane Z5 mm (0.2 in) must be above every shoulder and clamp. It and the G28 Z0 return are examples: adapt them to your machine, fixtures and controller.
Toolpath summaryG-code output is temporarily disabled while we add controller-specific arc-centre handling (I/J mode) and a radial-offset input. The toolpath values above are complete; program them in your CAM or controller's thread-milling cycle and verify in a simulator.
Fanuc / Haas style, absolute coordinates, I and J incremental, hole or stud centre at X0 Y0, top of the thread at Z0. The full thread form runs from Z = −thread length up to Z0, so the cutting profile goes a ramp (half a pitch inside, a quarter outside) lower and the end of the tool one tip length lower still: drill the hole or leave room below the stud for that. M03 climb only, cutter compensation off, tool length offset H1. Verify it in a simulator and with a dry run before cutting.
Tick the box above to show the G-code.
The thread mill turns on its own axis and orbits the thread on a helix that rises one pitch per orbit. The feed you program moves the tool centre, but the chip is cut at the edge. Inside a hole the edge travels a longer path than the centre, outside a stud a shorter one, so the programmed feed is corrected by the ratio of the two paths.
The centre-feed correction is the one Sandvik Coromant, Kennametal and the Machinery's Handbook give for thread milling, with D the major diameter. The thread geometry is the basic 60° profile of ISO 68-1 (metric) and ASME B1.1 (UN): tolerances, crest flats and the root radius of the tool are not included, so check the first part with a thread gauge. Inside a hole the tool enters and leaves on half circles from the hole centre that rise half a pitch; outside a stud on quarter circles that rise a quarter pitch. The toolpath places the full orbits from Z = −thread length upward, so the full thread form reaches the bottom of the thread and the entry arc starts that ramp lower. For external threads the correction (D + Dt)/D is the handbook form with the major diameter: at the root of the thread it is slightly light (about 9 % for M10 × 1.5 with a Ø7.5 tool). The milling time uses the full-depth radius for every pass, so it is approximate. The toolpath cuts the basic profile. In the default class 6H the basic profile is the smallest allowed nut thread; in class 6g the major and pitch diameters of the bolt sit es below basic, so M10 × 1.5 has a major diameter of at most 9.968 mm. Cutter radius compensation is not used (G40). To adjust thread size, change the radial depth / helix radius and re-check with a thread gauge. Use a thread mill made for the kind of thread you cut: internal and external thread mills have different profiles. The pilot hole is the standard tap drill (ISO 2306 for metric threads, the class 2B minor diameter range for UNC and UNF); its full-diameter depth, not the drill point, must reach below the lowest programmed Z by more than the tool’s tip length. The feed is a feed per minute (G94). Spindle speed, feed and radial passes are starting values: take the cutting data for your material from the tool maker. Any program made from these values is only safe after you have checked it in a simulator and run it once in the air.
This calculator sets up helical thread milling with a single-profile or multi-row thread mill. It gives the spindle speed, the feed to program at the tool centre so the cutting edge gets the chip you choose, the helix radius, the thread depth and minor diameter, radial passes, milling time and a helical toolpath summary to program in your CAM or the controller's thread-milling cycle. CNC programmers use it for metric, UNC and UNF threads inside holes and on studs, especially in large, hard or blind holes where a tap would be risky.
Program S5093, F191 at the tool centre, ten G03 orbits of radius 1.25 mm climbing 1.5 mm each. Programming the edge feed of 764 mm/min at the centre would overload the edge four times.
Calculate the edge feed as for any milling cutter, vf = fz × z × n, then correct it for the tool centre path. For internal threads vfc = vf × (D − Dt) / D, for external threads vfc = vf × (D + Dt) / D, where D is the major diameter and Dt the tool diameter. Program vfc with G02 or G03; most controls apply F to the tool centre when cutter compensation is off.
With the spindle turning clockwise (M03) and climb milling, internal threads are cut with G03 (counter-clockwise) and external threads with G02. A right-hand internal thread climbs from the bottom upward; a right-hand external thread is cut from the top downward. For a left-hand thread keep the same G-code and reverse the Z direction.
For internal threads the tool must be smaller than the minor diameter, and catalogue thread mills are usually about 70–80 % of the thread diameter. A smaller tool gives a shorter contact arc and less profile error from the helix, but is weaker and slower. For external threads the tool size is free; larger tools are stiffer.
Fine pitches in free-cutting material are milled in one pass. For pitches of about 2 mm and more, tough materials, long tools or deep threads, split the thread depth into 2–3 radial passes and add a spring pass (the last pass repeated) to remove the taper caused by tool deflection.
A single-profile tool has one tooth form and needs one orbit per pitch over the thread length, so it is slower but one tool covers many lengths and pitches of the same profile. A multi-row tool has several rows of teeth at the thread pitch and cuts the whole length in one orbit, which is much faster but needs a separate tool per pitch and higher machine and tool stiffness.
Thread milling makes little chip at a time, so it works in hard materials, large diameters and blind holes up to the bottom, and a broken tool is easy to remove. One tool cuts right- and left-hand threads and several sizes of the same pitch, and the final size is set by adjusting the toolpath radius against a thread gauge. Tapping is faster for small threads in long production runs.
What you need to build, measure or check the result.
Thread plug gauge setGo / no-go check of internal threadsView on Amazon →Thread pitch gaugeIdentify the pitch before you startView on Amazon →Thread mill cutterSingle-profile tool for many sizesView on Amazon →As an Amazon Associate I earn from qualifying purchases. Prices and availability are shown on Amazon.