CNC Precision Parts Guide: How Tolerance Really Adds Up

• 1
  Key takeaways
• 2
  What CNC precision parts actually mean
• 3
  Tolerance stack-up: the arithmetic that decides feasibility
• 4
  Machine and setup choices behind precision
• 5
  Surface finish, burrs, and edge condition
• 6
  Materials and how they behave at the cut
• 7
  Inspection data and what a report should show
• 8
  Which process fits which geometry

Precision in machining is not one number. A part is precise when every feature that matters lands inside its own tolerance band, in the same run, on the same machine, at the same temperature. Two features can each hold ±0.01 mm and still fail when they are checked against each other across a 300 mm span. That gap is why drawings with tight individual tolerances sometimes ship late while looser drawings run smoothly.

The second thing to fix is the reference. A feature is only as accurate as the datum it is measured from. If the datum face is a rough casting surface, or a face that gets recoated later, the tolerance is being applied to something that moves. Engineers who pick a machined face as the primary datum, and keep it clamped in one orientation, get far more repeatable results from the same machine and the same tolerance block.

Third, precision has a time dimension. A shop that holds ±0.005 mm on the first part is doing something different from a shop that holds it on part 500. Repeatability depends on tool wear, chip load, coolant, and how often the operator re-probes the fixture. When you review a quotation, ask what happens to the tolerance at the end of the run, not just at first article.

• 1
  Feature toleranceWhat the drawing asks for on one feature.
• 2
  Stack-upHow several tolerances combine across a distance.
• 3
  Datum strategyWhich face the measurement is tied to.
• 4
  RepeatabilityWhether the same result holds across the run.

Worst-case stack-up is simple addition, and it is the fastest reality check on any drawing. Take the tolerances that sit between the two features you care about and add them. If a bolt hole sits ±0.05 mm from a face, that face sits ±0.08 mm from a bore, and the bore sits ±0.03 mm from the mounting plane, the hole-to-plane error can reach ±0.16 mm. A ±0.1 mm clearance hole may not accept the fastener.

Statistical stack-up assumes errors cancel and gives a smaller number. It is valid only when the processes are independent and stable, which is not true when the same tool cuts all three features in one setup. On a single fixture with one tool, errors correlate and tend to add rather than cancel. Treat one-setup features as worst-case unless you have data that says otherwise.

There is a practical escape. Move the critical relationship into one setup. When a bore and its mating face are cut without releasing the part, the tolerance between them is the machine's positioning accuracy, not the sum of three operations. On a 5-axis center with a Ø400 mm rotary table, that is often what separates a workable design from a redesign.

Watch out for tolerance transfer during finishing. Anodizing adds 5–25 μm per surface depending on coating type, and it adds on both sides of a slot. A ±0.02 mm slot can close up after hardcoat. Specify pre-plate dimensions or mask the feature.

• 1
  Add before you quoteSum the chain by hand; it takes two minutes.
• 2
  Correlated errors addOne setup, one tool means worst-case behaviour.
• 3
  One-setup featuresMove critical pairs into a single operation.
• 4
  Coating shifts sizeAnodizing changes slot width on both walls.

A 3-axis mill cuts three faces with the part repositioned between operations. Each reposition adds fixture error, and each fixture is another chance for chips or burrs under the part. That is fine for plates with one critical face, brackets, and housings where the tolerances live on one side. It is a poor fit for parts with angular features, deep pockets on multiple faces, or bores that must stay coaxial.

A 5-axis center cuts angled faces and compound features without releasing the part. Coaxial bores, port faces, and impeller-style geometry come off the machine with their relative position set by the machine kinematics, not by a second fixture. GreatLight runs 16 simultaneous 5-axis machining centers, 12 four-axis mills, 27 three-axis machines, and 16 mill-turn centers, so the setup question is usually about geometry rather than capacity.

Turning deserves its own note. Long shafts, thin walls, and anything with a diameter-to-length ratio above about 8:1 will deflect under cutting force. A steady rest, a tailstock, or a mill-turn operation reduces that. If your drawing has a Ø6 mm pin 80 mm long with a ±0.01 mm diameter, expect the shop to ask about support before quoting.

Maximum part size matters less than you think. The largest travel we run is 4,000 × 400 × 150 mm, and the rotary table is Ø400 mm. Parts beyond a cavity size are not automatically impossible; they just move to a different machine class and often a different cost band.

• 1
  3-axisBest when tolerances sit on one side of the part.
• 2
  5-axisKeeps compound features in one setup.
• 3
  Mill-turnHandles shafts and features needing both motions.
• 4
  Slender partsSupport the work or the tolerance will drift.

Surface finish and dimensional accuracy are separate purchases. A part can hold ±0.005 mm with an as-machined Ra 1.6–3.2 μm surface, and a part can look mirror-bright while drifting out of tolerance because the polishing removed 15 μm of material. Specify finish where it does work: sealing faces, sliding contacts, optical paths, flow surfaces. Leave the rest as machined.

The usual sequences are straightforward. As-machined covers most brackets and housings. Ra 0.8–1.6 μm comes from a finishing pass with a smaller stepover or a wiper insert, and it is the common choice for mating faces and O-ring grooves. Ra 0.2–0.8 μm needs slower feed, sharper tooling, and often tumbling or polishing afterward. Ask what the measurement method is, because a visual check and a profilometer reading are not the same claim.

Burrs are the failure mode nobody puts on a drawing. A 0.2 mm burr on a fuel passage or a medical cannula is a functional defect, not a cosmetic one. Deburring by hand is variable; tumbling and electrochemical deburring are repeatable but affect all edges. Call out the edges that must stay sharp and the edges that must be broken.

Laser marking has a floor. The minimum character height we can mark legibly is 1.5 mm. Below that, characters smear and traceability codes stop scanning. If your part number has 14 digits, plan the marking area before you finalize the geometry.

• 1
  Specify finish by functionSealing and sliding faces, not every surface.
• 2
  Polishing removes materialAccount for it in the tolerance budget.
• 3
  Burrs are functionalCall out sharp and broken edges separately.
• 4
  Marking floor1.5 mm minimum character height.

Material choice sets the achievable tolerance more than most engineers expect. Aluminium 6061-T6 and 7075 machine cleanly and hold tight tolerances, but they move with heat. The coefficient of thermal expansion for aluminium is roughly 23 μm per metre per °C. A 500 mm aluminium part that is 5 °C warmer than the inspection room measures about 58 μm longer than it will at 20 °C. On a ±0.02 mm callout, that is the whole budget.

Stainless 303 and 304 cut differently from each other. 303 is free-machining and holds size well. 304 work-hardens, so light passes with a dull tool raise the surface hardness and push the next pass off size. 17-4PH holds good strength and machinability together, which is why it shows up in valve and pump work. Titanium Ti-6Al-4V and Inconel cut hot, transfer heat into the tool, and need lower speeds and more coolant; tolerances hold, but cycle time grows.

Plastics behave in the opposite direction. POM and PEEK are dimensionally stable and machine to tight limits, but they have high thermal expansion coefficients and they relax after machining. A PEEK part measured an hour after cutting may be 20–40 μm different the next day. For plastics, agree on a measurement window and a conditioning period before you argue about the number.

Certification requirements can narrow the material list. Medical work under ISO 13485:2016 and automotive work under IATF 16949:2016 both need material traceability, so a substitute alloy is not a free swap. Bring the standard into the conversation early.

• 1
  AluminiumMachines well, moves with temperature.
• 2
  304 stainlessWork-hardens; light passes punish dull tools.
• 3
  PEEK and POMRelax after cutting; fix a measurement window.
• 4
  Regulated industriesTraceability limits material substitution.

A dimensional report is only meaningful when it states the setup. Which datum was used, how the part was clamped, what the ambient temperature was, and which instrument produced each number. A CMM result from a part held in a vise on a granite table does not describe the same part that was clamped in a fixture during machining. Free-state and restrained-state measurements differ, and both are legitimate if they are labeled.

Sampling strategy matters as much as the instrument. Checking one part from a 500-piece run tells you the setup was right at the start. Checking first article, mid-run, and last article tells you whether the process drifted. We run a raw material check, in-process monitoring, and a final inspection before shipment, with reports available on request, and 100% inspection before shipment on the parts that need it.

Not every feature needs a CMM. Bore diameters, depths, and thread positions can be verified with gauges and micrometers faster and just as reliably. Save the CMM time for position tolerances, profile callouts, and features that are hard to reach. That keeps inspection cost proportional to risk.

If a feature is critical, put a number and a method on the drawing. "Critical surface" is not inspectable. "Ra 0.8 μm max, measured with a profilometer along the axis" is. The same applies to flatness, runout, and concentricity; each one needs a datum and a direction.

• 1
  State the setupDatum, clamping, temperature, instrument.
• 2
  Sample across the run
• 3
  Match method to featureGauges for simple, CMM for positional.
• 4
  Make it inspectableNumber, datum, and method on the drawing.