High precision CNC milling explains what really sets tight tolerances

• 1
  What high precision CNC milling actually means on the shop floor
• 2
  Where the error budget goes
• 3
  Which features can hold tight tolerance and which cannot
• 4
  How the workpiece material shifts the achievable window
• 5
  How tolerance is verified, and why that changes the design
• 6
  Which tolerance band fits which feature and material

High precision CNC milling is milling held to tolerances far tighter than general machining work: typically ±0.005 mm (±0.0002 in) on critical features, with surface finish down to Ra 0.2–0.8 μm when the drawing asks for it. That number is not a machine specification. It is a result that depends on the tool, the fixturing, the material and the temperature of the room on the day the part is cut.

The process itself is still subtractive. A rotating cutter removes material from a solid block along G-code paths. What changes at this level is the size of the error budget. At ±0.1 mm, a worn cutter and a warm spindle are noise. At ±0.005 mm, they are most of the budget.

So the useful question is never "can you hold this tolerance?" It is "on which feature, in which material, at which feature size?" A 6 mm bore in 6061 aluminium and a 6 mm bore in 17-4PH stainless are two different problems. The first is routine. The second needs a different cutter, a different feed, and probably a second pass.

• 1
  Tolerance is per featureA ±0.005 mm bore does not make the whole part a ±0.005 mm part.
• 2
  Finish is separateRa is set by tool edge radius and stepover, not by the tolerance block.
• 3
  Material sets the limitHarder, gummier or more abrasive alloys shrink the achievable window.

Roughly five things eat tolerance in a milling cut. Thermal growth comes first. Aluminium expands about 23 μm per metre per °C, steel about 11 μm. A 100 mm aluminium part that warms 5 °C during a roughing cycle grows 11.5 μm on its own, which is already more than half of a ±0.005 mm band. That is why tight work gets rough machined, cooled, then finished.

Tool runout is second. A cutter held 10 μm off centre cuts one flute deeper than the others. On a 3 mm end mill that shows up as a slot 20 μm wider than programmed and a rougher wall on one side. A shrink-fit holder or a good collet with a dial-indicator check before the finishing pass removes most of it.

Then there is machine geometry, fixturing deflection and cutter wear. Each contributes a few microns, and they add up in ways that are hard to predict on paper. The practical answer is measurement: probe the workpiece, set the work offset from the probed face, cut, measure, and compensate. GreatLight inspects 100% of parts before shipment for exactly this reason.

• 1
  ThermalLet the part stabilise before the finishing pass.
• 2
  RunoutCheck radially at the cutting edge, not at the holder.
• 3
  DeflectionThin walls and long tools bend under cutting force.
• 4
  WearIndex or replace the cutter before the last pass, not after.

Tight tolerance lives on features the cutter can reach in a single setup with rigid support. A bore, a flat face, a slot in a thick section, a bolt pattern drilled and reamed in one orientation: these are realistic at ±0.005 mm. Features that need three setups, a long reach, or a wall under 1 mm thick are not.

Deep cavities are the classic problem. A 4:1 depth-to-diameter cutter deflects under load, so the floor of a deep pocket tends to come out slightly convex and the corners slightly tight. If that floor is your datum, the error propagates into everything measured from it.

Sharp internal corners are the other common trap. A rotating cutter always leaves a corner radius equal to the tool radius. A 6 mm cutter cannot produce a 0.5 mm internal corner. The drawing should either call out the radius or the feature should be a relief, not a corner. On a 5-axis machine, tilting the tool lets a shorter, stiffer cutter reach more of a contoured surface, which helps accuracy on curved geometry but does not remove the corner-radius rule.

• 1
  One setup winsFeatures machined in the same orientation share one error stack.
• 2
  Depth-to-diameterKeep it under 3:1 when tolerance matters.
• 3
  Corner radiusThe smallest internal radius equals the smallest cutter you can use.

Aluminium 6061 and 7075 cut cleanly and hold ±0.005 mm on most features without drama. They also move the most with temperature, so a hot part measures differently than a cold one. Measure at 20 °C or accept that the number on the CMM depends on when you walked over to it.

Stainless 304 and 316 work-harden at the cut. Light passes with a dull cutter raise the surface hardness and push the next pass off line. 17-4PH in the H900 condition is stable and predictable, which is why it is common in medical and aerospace work. Titanium TC4 (Ti-6Al-4V) is the opposite: low thermal conductivity, high elasticity, and a strong tendency to chatter. Rigi­dity matters more than spindle speed.

Plastics behave differently again. POM and PEEK move with coolant and clamp pressure, and a part measured while still warm can read 0.05 mm off. For these materials it is often better to machine slightly oversize, stress-relieve, then take a light finishing cut. Inconel sits at the far end: it is machinable, but tool life is short and the tolerance band per cut is narrow.

• 1
  AluminiumEasy to cut, hardest to measure cold.
• 2
  StainlessWatch work-hardening on light finishing passes.
• 3
  TitaniumChatter is the main enemy; shorten the tool.
• 4
  PlasticsClamping and heat move the part more than the cutter does.

A tolerance is only real if it can be measured. On a 6 mm bore at ±0.005 mm, a caliper is not enough; the measurement uncertainty of the gauge has to be well inside the band. That usually means a bore gauge, a micrometer, or a CMM, and it means the drawing should say which features are actually inspected.

This has a direct design consequence. Every tight feature adds inspection time, and inspection is a real cost. If a bracket has one critical bore that locates a bearing, tighten that one. Leaving the other twenty dimensions at ±0.1 mm keeps the part affordable without affecting function.

GreatLight runs raw material checks, in-process monitoring during the cut, and a final inspection before shipment, with reports available on request. The reports matter most when a feature is a fit: a bearing seat, a dowel hole, a sealing face. Those are the dimensions worth paying to control.

• 1
  Gauge firstIf you cannot measure it, do not tolerance it.
• 2
  Tighten the fitSpend the tolerance on interfaces, not on the outline.
• 3
  Ask for reportsAvailable on request for critical features.