Metric vs Imperial Machining

Metric vs imperial machining is shorthand for the two unit systems a shop works in: the millimetre, standard across most of the world, and the inch, still the working unit of North American drawings and tooling. A CNC machine moves where it is told and has no opinion about units; the numbers in a program become a part only once the unit system is fixed. Because the systems meet at 25.4, reading one set of numbers as the other scales every feature by that factor — a mistake that can scrap a job before a tool spins.

The two unit systems a machinist meets

The metric system is decimal. Its base unit is the metre, but the working units are the millimetre (mm) and the micrometre (µm), one thousandth of a millimetre. Tolerances read naturally as decimals: ±0.1 mm for a rough feature, ±0.02 mm for a normal one, ±0.005 mm for a demanding one.

The imperial system has no clean decimal history, but shop practice settled on decimal subdivision. The working unit is the thousandth of an inch, the “thou” (the “mil” in North America), and a “tenth” is 0.0001 in. Shop talk is “hold this to a thou” or “within two tenths”, and drawings are read in decimal inches even when the ruler that made them was fractional.

The two systems are joined by an exact number: since 1959, 1 inch = 25.4 mm exactly. So 1 mm ≈ 39.37 thou, and 1 thou = 25.4 µm, close to a 0.025 mm tolerance. North America draws and buys tooling in inches; most of the rest of the world works in millimetres, and the two meet constantly — a metric drawing in an American shop, an inch-dimensioned spare made in Europe — which is where the machinist must not slip.

Where units live on a CNC machine

Unit choice is a property of the program and the control, not of the machine’s mechanics. A program declares its units with a modal G-word: G21 selects metric (millimetre), G20 imperial (inch), on the Fanuc-derived controls that dominate, while Siemens uses G71/G70. It belongs at the top of the program, and a well-formed program keeps one unit system throughout; everything downstream — the X, Y and Z words, arc radii, I/J/K offsets, work and tool-length offsets, and the feed numbers — is interpreted in those units.

The trap is that G20 and G21 interpret, they do not convert. Change the unit word without converting the numbers and every coordinate is re-read in the wrong unit, scaling each feature by 25.4. The classic cause is a CAM mismatch: a model built in millimetres, a postprocessor set for inches, and nobody checking that the unit word the post writes matches its coordinates. Newer controls can tag offsets with the unit system they were created in and convert them automatically, but the machine’s basic unit system is still set once in machine data — so every program should state its own.

Why metric mode has the resolution edge

There is one genuine technical argument for metric. A control accepts coordinates only down to its least input increment, the smallest value it can command. Typical settings are 0.001 mm in metric and 0.0001 in in inch mode — and they are not equivalent: 0.0001 in is 2.54 µm, while 0.001 mm is 1 µm. The same control commands a step roughly two and a half times finer in metric.

That shows where steps matter. Across a 0.001 in (0.0254 mm) tolerance band, metric mode offers about twenty-five discrete positions against inch mode’s ten, and interpolated arcs stay closer to the programmed path when increments are smaller — which is why shops on tight inch work sometimes run the control in metric while thinking in inches. This is resolution, not accuracy: a finer grid does not make a machine land more truthfully, a distinction covered in the wiki’s entry on accuracy, repeatability and resolution.

Units follow the rest of the job

Choosing the unit system decides the units of everything that derives from it. Feed rate is millimetres per minute in a metric program and inches per minute in an inch one, and per revolution (mm/rev, inches per revolution) in turning. Constant surface speed in turning runs in feet per minute or metres per minute; the conversion is ×0.3048, the metres per foot.

Threads are where the systems refuse to talk. An imperial Unified screw is specified by threads per inch — 1/4-20 UNC has twenty threads per inch — while a metric ISO screw is specified by pitch, the millimetres between crests, as in M6 × 1. They are the same spacing in different units, linked by pitch in mm = 25.4 ÷ TPI. Twenty TPI is a 1.27 mm pitch; a 1.25 mm pitch is 20.3 TPI. “Equivalent” charts line up diameters, not interchangeability — the pitches differ, and only the 60° form is shared. On a lathe the divide is mechanical: an imperial thread cut on a metric-leadscrew lathe needs a 25.4 ratio in the change gears, classically a 127-tooth gear.

Converting without losing the part

The arithmetic is trivial because 25.4 is exact; what ruins conversions is what it leaves behind. Convert the whole job or none: coordinates, work offsets, tool-length compensations, feed numbers and the unit word must move together. Round deliberately — a drawing tolerance of ±0.0005 in is ±0.0127 mm; express it as 0.013 mm or keep the program in inches, but do not round looser. The other way, a metric tolerance stated in micrometres has no exact even thousandth, so rounding to the nearest 0.0001 in can silently eat the allowance. When a millimetre drawing reaches an inch shop, convert the geometry once in CAD or set the machine up in metric and work in millimetres. Then prove it: run a prove-out, or cut and measure one feature, before trusting the job.

Which system should a shop use

Follow the drawing: a part dimensioned in inches gets an inch program in an inch-region shop, and a metric drawing a metric one. Follow the supply chain, because tooling, inserts and mating parts carry the same units. Do not mix systems inside one program or one job. The machine’s basic setting is only a default — most controls run either system if the program declares it — so for new work the honest answer is metric for anyone outside North America and for any shop with metric drawings, with the resolution argument nudging close-tolerance and finishing work toward metric regardless of the drawing’s units.

Two cautions close it out. Never trust a thread to the nearest size on a conversion chart. And never assume a value’s units — a caliper, a DRO and a program may each be showing numbers, but a job scaled by 25.4 looks perfectly reasonable on screen and is perfectly wrong on the part.

Metric vs imperial machining is decided once, at the top of a program and on the drawing, yet its consequences run through the feeds and speeds every cut depends on, the tolerances the machine can hold, and every job the CNC machine is asked to make.