Precision CNC Service: Expected Accuracy You Can Actually Hold

• 1
  Key takeaways
• 2
  What accuracy to expect by part and feature
• 3
  What cnc service expected accuracy really means
• 4
  What actually moves your dimensions off target
• 5
  Which process route fits which part
• 6
  How to judge a supplier's accuracy claim
• 7
  Common mistakes that cost tolerance on the floor
• 8
  Step by step: specifying and verifying cnc service expected accuracy

Accuracy is how close the finished feature lands to the nominal on the drawing. Repeatability is how close the next part lands to the first one. A shop can hold ±0.005 mm on one bore and still ship a run that drifts 0.02 mm across 500 pieces. Those are different problems, and your drawing needs to say which one matters.

The number on a quotation is usually a floor, not an average. When a supplier writes ±0.005 mm, that figure belongs to a defined condition: a certain envelope, a certain material, a controlled temperature, a single fixturing setup. Change any of those and the number changes with it. Ask what envelope the claim covers.

Three terms show up on every drawing. Tolerance is the allowed band. Surface finish is the texture left by the cutter. Datum is the reference the measurement hangs from. If the datum is unclear, two inspectors can measure the same part and disagree without either being wrong.

One more distinction matters for buyers. Dimensional accuracy covers size and position. Geometric accuracy covers flatness, perpendicularity, and concentricity, which is where tight-tolerance programs usually fail first. A CMM report should cover both, or you only see half the picture.

Thermal growth is the largest single factor nobody plans for. Aluminium expands roughly 23 μm per metre per degree Celsius; steel sits near 11 μm. A 300 mm aluminium part in a shop swinging 5 °C can move 0.035 mm before the spindle ever touches it. That is several times a ±0.005 mm band.

Spindle and tool deflection come next. A long end mill at high feed pushes away from the wall, and the wall springs back after the cutter passes. Tool runout adds a constant offset on every feature that tool cuts. Worn carbide shows up as a slow drift you only catch by measuring across the run.

Workholding sets the baseline. A part clamped in a vise with 2 mm of unsupported wall will move when the jaws release. Residual stress in a rolled plate relieves itself as you remove material, so a roughing pass followed by a rest before finishing is not wasted time.

On five-axis work, rotary axis error stacks on top of linear error. A Ø400 mm rotary table with a few arc-seconds of tilt error turns into a visible position error at the edge of a long part. This is why simultaneous five-axis is good for complex geometry and not automatically good for tolerance.

Three-axis milling handles flat plates, open pockets, and prismatic housings with faces reachable from one direction. Tolerances of ±0.01–0.02 mm are routine, and the setup is simple. If the part needs four or five faces machined, you are paying for extra setups and inheriting re-chuck error with each one.

Four-axis and mill-turn routes cut down on setups. A shaft with cross-holes and a turned OD usually belongs on a mill-turn center, where one setup holds concentricity that two machines cannot match. This is the cheapest way to buy accuracy: remove a setup rather than tighten a tolerance.

Simultaneous five-axis is for contoured surfaces, undercut features, and parts that cannot be reached any other way. The trade is that the machine has more error sources, so the tolerance you get depends on the geometry and the post-processor. Use it where the shape demands it, not as a default.

On material, 6061-T6 and 17-4PH behave very differently. Aluminium cuts fast and moves with heat. Stainless work-hardens if feed is too light. Titanium and Inconel need lower surface speed and more attention to tool life. Material choice changes the tolerance you can hold before any machine is picked.

Ask for the measurement method before you ask for the number. A CMM with a stated uncertainty is a different level of evidence than calipers and a pin gauge. On a claim of ±0.005 mm, hand tools are not even in the conversation, because their own uncertainty is close to the band.

Ask what happens when a feature misses. A shop that inspects 100% before shipment and can show in-process records is telling you something about how it catches drift. Raw material checks, in-process monitoring, and a final inspection report on request are the three stages worth confirming.

Certifications help narrow the field but they are not accuracy. ISO 9001:2015 covers quality management. IATF 16949:2016 applies to automotive work. ISO 13485:2016 covers medical devices. ISO 27001:2022 covers information security, which matters if your drawings are sensitive. None of them measure a bore.

Finally, look at the commercial terms that affect tolerance. No minimum order quantity lets you run one prototype and check the result before committing. A 12-hour quotation with DFM feedback tells you whether the supplier reads the drawing. Production start within 24 hours is useful, but only if the first article is right.

Blanket tolerancing is the most expensive habit. Marking every dimension at ±0.005 mm raises cost across the part and hides the two features that actually need it. Tolerance the fits, the sealing faces, and the assembly datums. Leave the rest at general tolerance.

Ignoring the temperature at inspection is the second. A part measured straight off the machine is warm; a part measured the next morning is not. If the drawing calls for a tight band, both parties need to agree on the temperature at which the part is measured.

Chasing tolerance with more finishing passes has a limit. Below a certain depth of cut the tool rubs instead of cutting, which makes finish worse and burns the edge. If a feature will not hold, the answer is usually the setup or the tool, not another pass.

Skipping the first article is the last one. On a new program, the cheapest insurance is to measure the first part against the drawing before the run continues. Catching a datum error at part one costs a setup change. Catching it at part 500 costs the run.