CNC Close Tolerance Processing Guide

• 1
  What CNC close tolerance processing really means
• 2
  Thermal growth: the error that hides until the third shift
• 3
  Tool deflection and why long tools break tolerance first
• 4
  Fixturing and datum strategy decide repeatability
• 5
  Where close tolerance processing stops being practical
• 6
  Which tolerance band fits which feature

A tight tolerance is a number on a drawing. Close tolerance processing is everything the shop does so that number stays true on part 1, part 50, and part 500. The two are not the same thing, and confusing them is how projects slip.

Most drawings mix two very different classes of requirement. Size tolerances, such as a bore at Ø20.000 +0.010/0 mm, are checked with a micrometer or bore gauge in seconds. Geometric tolerances, such as a 0.010 mm coaxiality between that bore and an outer diameter, force the shop to hold a datum, control machine geometry, and often build a fixture before the first cut.

In practice, the geometric callouts decide whether a job is routine or difficult. We work to ±0.005 mm (±0.0002 in) on qualified features, with surface finish from Ra 0.2–0.8 μm when the function demands it. Those numbers are not a marketing line. They are the edge of what a stable process can repeat across a batch, and only on features the shop can actually reach.

One more distinction matters. A tolerance applies at 20 °C on a part that has cooled down. Measure a freshly cut aluminum bore and it will read small. Let it sit, and it grows back. If the drawing does not state a temperature, assume 20 °C and plan the measurement accordingly.

Aluminum expands about 23 μm per meter per °C. Over a 200 mm part, a 5 °C swing moves a feature by roughly 0.023 mm. That is five times a ±0.005 mm band, and it happens without a single alarm on the machine.

The heat comes from two places. The spindle and axis motors warm the structure over the first two hours of a shift, and the cut itself pushes heat into the workpiece. Neither is constant. A machine that started the morning at 18 °C will not cut the same geometry at 11 a.m. unless someone controls it.

Shops that hold microns run spindles warm-up cycles before the first part, keep coolant at a set temperature, and machine in a temperature-controlled room. GreatLight runs three plants with 127 high-precision CNC machines, and the tightest cells sit in controlled environments rather than on the general floor.

The practical consequence for a designer is simple. A callout that is possible on a 50 mm bracket may be unrealistic on a 600 mm plate, not because the machine is worse, but because the same 5 °C now costs 0.070 mm.

Every cutting tool bends under load. A Ø6 mm carbide end mill hanging 60 mm out of the holder can deflect tens of microns at normal finishing feeds. The tool does not break. It just cuts a wall that is not where the CAM file said it would be.

Deflection scales with the cube of the length-to-diameter ratio. Going from 4×D to 8×D overhang makes the tool roughly eight times softer. That is why deep pockets and thin ribs are the features that miss tolerance, and why the fix is usually a shorter tool, a smaller step-down, or a different toolpath rather than a slower feed.

Climb milling with light radial engagement reduces the cutting force and therefore the deflection. On a finishing pass at 0.1–0.2 mm radial width, the wall comes out straighter than with a heavy conventional pass, even at the same feed per tooth.

There is a floor here. Below about Ø1 mm, tool runout and edge radius start to dominate, and the achievable tolerance widens. If a design needs a Ø0.8 mm slot to ±0.005 mm, question the design before questioning the shop.

A part is only as accurate as the way it is held. Clamp a thin plate on four corners and the middle bows upward while the vise jaws squeeze. Release it, and the part springs back to a shape that never matched the drawing.

The rule that survives contact with real parts is this: hold on the most rigid feature, support under the cutting zone, and never clamp across a thin wall. For a 2 mm aluminum web, that usually means a vacuum plate or a soft-jaw pocket rather than a vise.

Datum transfer is the other half. If the drawing calls a bore as datum A and the shop machines all other features from an outside edge, the relationship between them carries every error of the setup. One setup, one datum, and the stack-up disappears.

This is where 5-axis work earns its place. Turning the part in the spindle instead of moving it between fixtures removes a whole family of position errors. GreatLight runs 16 simultaneous 5-axis machining centers for exactly this reason.

Not every feature on a part needs the tight number. Tolerance is a cost, and it should sit where the function needs it. A mounting hole pattern for M4 screws at ±0.05 mm will assemble fine and cost a fraction of a ±0.005 mm pattern.

Some geometries resist tight control no matter how good the shop is. Thin walls under 1 mm deflect during and after cutting. Long slender bores drill off-axis. Sharp internal corners cannot be milled to a true radius smaller than the tool. Deep holes beyond 10×D wander even with peck drilling and piloting.

Material matters too. Aluminum and brass machine predictably. Stainless 316 work-hardens, titanium Ti-6Al-4V moves under heat, and Inconel wears tools fast enough that the last part in a batch cuts differently from the first.

The honest answer to a hard callout is a conversation, not a quote. Ask what the feature does. If the answer is clearance or appearance, relax it. If it locates a bearing or seals a gas path, keep it and pay for the process.