CNC tolerance control: how ±0.005 mm is actually held

• 1
  What CNC tolerance control really means
• 2
  Where the variation comes from
• 3
  What each machine class can hold
• 4
  Material behaviour and tolerance
• 5
  How you prove the tolerance was held
• 6
  Tolerance band versus process choice

A tolerance is the permitted spread between the largest and smallest acceptable value of a feature. CNC tolerance control is the practice of keeping every feature inside that spread, batch after batch, not just on the first article. Two parts made to the same nominal dimension can still fail to mate if the variation drifts in opposite directions.

Two families of tolerance show up on almost every drawing. Dimensional tolerance sets the size band for a length, diameter, or depth, such as a Ø10 mm shaft held at ±0.01 mm. Geometric tolerance, written in the feature control frame, sets the form, orientation, and location of that feature relative to a datum. Both matter, and they are checked with different equipment.

The practical question is never whether a machine can hit a number once. It is whether the process holds that number across a run of 50 or 5,000 parts, through tool wear, chip load changes, and the temperature swing between a morning shift and an afternoon shift. That repeatability is what a tolerance really buys.

Control starts before the spindle turns. Setup sheets, probing routines, and in-process checks decide whether the operator sees a drift while there is still stock to correct it. A shop that only measures at final inspection is sorting scrap, not controlling tolerance.

Every cut is a small collision. The tool pushes into the material, the material pushes back, and the whole loop of spindle, holder, tool, fixture, and part flexes by a few microns. On a light finishing pass in aluminium this deflection may be 2–5 μm. On a deep pocket in 4140 steel with a long reach tool it can be 20 μm or more.

Thermal growth is the quiet one. A spindle running at 12,000 rpm warms and grows axially. Aluminium expands roughly 23 μm per metre per °C, so a 100 mm aluminium part that warms 5 °C from a cold start moves about 11 μm. That alone can eat half of a ±0.01 mm band.

Tool wear adds a slow trend rather than a random error. A carbide end mill may wear 0.01–0.03 mm on diameter over a long run depending on material and coating. The first part and the last part from the same program are not the same size unless the offset is adjusted as the tool wears.

Fixturing decides how much of the cutting force reaches the part as movement. Thin walls, unsupported bores, and parts held only on a small pad will deflect under load and spring back after the cut, leaving a taper or a bell-mouth that no amount of slow feed will remove.

Three-axis vertical mills with a rigid setup hold ±0.02 mm comfortably on prismatic features and ±0.05 mm on long bores without special measures. That covers most brackets, plates, housings, and mounting faces. Pushing them to ±0.005 mm means slower finishing passes, temperature control, and more inspection time.

Four-axis and mill-turn centers add rotary positioning, so they hold angular relationships between features on different faces. The rotary table resolution matters more than the linear axes here; a Ø400 mm rotary table with a small angular error becomes a large linear error at the part edge.

Simultaneous 5-axis centers are where tight tolerances on contoured surfaces become practical. Cutting a curved face with the tool tilted keeps the contact point on the ball nose instead of the tip, which reduces scallop height and holds profile tolerance without hand blending. We run 16 simultaneous 5-axis machining centers for this reason.

Size changes the answer. A 4,000 mm part cannot be held to ±0.005 mm over its whole length, because thermal and geometric errors scale with distance. Tight local features on a large part are fine; a tight overall length is not. Split the callout so the tight band applies only where it functions.

Aluminium 6061-T6 and 7075 machine cleanly and hold tight tolerances, but they move after machining. A part hogged out of thick plate can distort 0.05–0.2 mm as internal stress releases. Rough, stress-relieve, then finish, and the final pass cuts the geometry the part will actually keep.

Stainless 304 and 316 work-harden under the cutter. A dull tool rubs instead of shearing, which raises cutting force and pushes the part away, so the tolerance drifts mid-run. Sharp tooling and constant feed per tooth matter more here than on aluminium. 17-4PH in the H900 condition behaves differently again and often needs a finishing allowance.

Plastics are the opposite problem. POM and PA absorb moisture and change size with humidity; PEEK holds dimension better but needs sharp tools and generous coolant to avoid melting. A tolerance of ±0.05 mm on a POM part is realistic, ±0.01 mm usually is not.

Titanium and Inconel generate heat at the cutting edge and conduct it poorly, so the tool and the part both grow. Roughing with high-pressure coolant, then letting the part stabilise before finishing, is standard practice for TC4 and Inconel 718 work.

The measurement method has its own uncertainty, and it must be smaller than the tolerance. Calipers read to 0.02 mm at best and are not a control instrument for a ±0.005 mm callout. Micrometers, bore gauges, and height stands get closer; a coordinate measuring machine with a calibrated probe is the usual answer for geometric tolerance.

Temperature matters at inspection too. A part measured straight off the machine at 30 °C and a part measured in a 20 °C inspection room differ in size. For tight work, let parts settle to room temperature before final measurement, or record the temperature alongside the reading.

Sampling strategy decides whether you catch a trend or only a single bad part. First article, then periodic checks through the run, then a final inspection catches drift. Checking only the last part hides everything that happened in between.

We inspect 100% of parts before shipment, covering raw material check, in-process monitoring, and final inspection, with reports available on request. For a ±0.005 mm feature that means probing or gauging at the machine, not only at the end of the run.