Toledos Precision CNC: What the Tolerance Actually Costs

• 1
  How a tolerance of ±0.005 mm is actually held
• 2
  When 5-axis earns its setup time and when it does not
• 3
  Material choice changes the achievable finish
• 4
  Inspection is where the number is proven
• 5
  Where precision CNC is the wrong process
• 6
  Matching the process to the part

A tolerance is not a promise a machine makes on its own. On a CNC, the finished size is the sum of thermal drift, tool wear, fixture stiffness, spindle error and the probing routine that catches all four. ±0.005 mm (±0.0002 in) is reachable on a 5-axis center, but only when the part is small enough that the error budget divides cleanly among those sources.

The first control is thermal. A spindle that has run for two hours is not the same size as one that has run for twenty minutes. Shops that hold tight tolerances rough the part, let it cool, then finish it in a second setup. On aluminium this matters more than on steel because the coefficient of expansion is roughly twice as high.

The second control is the fixture. A part held on three points behaves differently from one clamped in a vise. Thin walls move when the clamp releases, so the measured size on the machine is not the size on the bench. This is why we measure after unclamping, not before.

The third control is probing. In-process measurement on the machine catches drift before the finishing pass, and it lets the operator offset a tool rather than scrap the part. Without probing, a 0.004 mm drift is invisible until final inspection, which is too late.

• 1
  Rough, cool, finishTwo setups beat one when the tolerance is under ±0.01 mm.
• 2
  Measure unclampedClamping force can shift a thin wall by more than the tolerance.
• 3
  Probe in processOffset the tool instead of scrapping the part.

Five-axis machining is often sold as a general upgrade. It is not. Simultaneous 5-axis matters when the feature cannot be reached from a single tool direction, or when the number of setups is the real cost driver. A part with pockets on five faces and a true position callout between them is a good candidate. A flat bracket with four holes is not.

The reason is setup error. Every re-clamp adds a datum shift. On a 3-axis machine, a part with features on four sides needs four setups, and each one can introduce 0.01–0.02 mm of positional error. A 5-axis center reaches those faces in one setup, so the accumulated error stays inside one machine coordinate system.

The trade-off is cycle time and programming. Simultaneous 5-axis toolpaths are slower to program, and a rotary table with a Ø400 mm envelope limits part size. For a 4,000 mm long extrusion, a 3-axis or 4-axis machine is the practical choice.

We run 16 simultaneous 5-axis centers, 12 four-axis mills and 27 three-axis machines. Matching the part to the machine is a bigger cost lever than pushing every job onto the newest spindle.

• 1
  Choose 5-axisFeatures on 4+ faces, tight true position between them, or organic contours.
• 2
  Choose 3-axisFlat plates, single-face work, long parts up to 4,000 mm.
• 3
  Watch the envelopeØ400 mm rotary table limits what fits on simultaneous 5-axis.

The same cutter and the same parameters give different results in 6061 aluminium and 17-4PH stainless. Aluminium cuts clean at high speed and takes a mirror finish easily. 17-4PH in the H900 condition will work-harden under a light finishing pass if the feed is too low, and the surface tears instead of shearing.

Titanium TC4 (Ti-6Al-4V) is the harder case. It conducts heat poorly, so the cutting edge carries most of the temperature. Rushing the finishing pass shortens tool life and leaves chatter marks that no bead blasting will hide. Inconel is slower still, and it is usually worth asking whether the part really needs it.

Plastics behave in the opposite way. POM and PEEK machine well but move with temperature and absorb moisture. A PEEK part measured straight off the machine can be 0.05 mm off after it equilibrates. For tight plastic parts, the drawing should say when the measurement is taken.

When a part needs both hardness and a fine finish, the sequence matters more than the material. Machine soft, heat treat, then finish grind or finish machine to size. Machining a hardened blank to ±0.005 mm is possible, but the tool cost and inspection time go up.

• 1
  Aluminium6061-T6, 7075, 2024, 6082 — fast cuts, easy Ra 0.8–1.6 μm.
• 2
  Stainless303 and 316L cut predictably; 17-4PH needs a firm feed to avoid work hardening.
• 3
  PlasticsPOM, PEEK, PA — specify when the measurement is taken.

A certificate that says ±0.005 mm without a measurement method is not evidence. The drawing and the inspection report have to agree on datums, on which features are critical, and on the gauge used. A CMM with a 2 μm stated accuracy is not the right tool to sign off a 5 μm tolerance without an uncertainty budget.

We check raw material on arrival, monitor in process and inspect before shipment, with 100% inspection before parts leave. Reports are available on request. For a first article, the report is worth more than the parts, because it tells you whether the process is stable or whether the good parts were luck.

Capability matters more than a single reading. A shop that holds ±0.005 mm on one part and ±0.02 mm on the next has a process problem. Ask for the spread across a run, not the best single result. Our recorded qualification rate is 99.99%, and that figure only means something alongside the inspection routine behind it.

Surface finish is measured the same way. Ra 0.2–0.8 μm is a fine finish, Ra 0.8–1.6 μm is a high finish, Ra 1.6–3.2 μm is as machined. The number should match the function: a sealing face needs the low value, a structural bracket usually does not.

• 1
  Agree on datumsInspection follows the drawing datum scheme, not a convenient one.
• 2
  Ask for spreadA run average plus range beats one hero measurement.
• 3
  Match finish to functionDo not pay for Ra 0.2 μm on a non-contact surface.

CNC machining removes material one part at a time. That is an advantage for geometry and a disadvantage for volume. Past a few thousand identical parts, die casting, vacuum casting or 3D printing can beat it on unit cost, even after tooling. The crossover depends on the part, not on a fixed number.

Very thin walls are a second boundary. A 0.3 mm aluminium wall can be machined, but it will deflect under clamping and chatter during the finishing pass. If the design allows 0.8 mm, the part gets cheaper and more repeatable.

Deep small holes are a third. A Ø1 mm hole at 20× diameter needs a long, thin tool that breaks easily. Drilling from both ends, or specifying EDM, is often cheaper than forcing it on a mill.

Finally, cost scales with the number of critical features, not with part size. A small part with twelve tight bores can cost more than a large plate with one flat face. When a quote looks high, the useful question is which tolerance is driving it.

• 1
  VolumePast a few thousand identical parts, casting or printing usually wins.
• 2
  Thin wallsBelow roughly 0.8 mm in aluminium, deflection and chatter take over.
• 3
  Deep small holesPast 10× diameter, plan for a pilot drill or EDM.