What a CNC precision machining expert actually controls

• 1
  Key takeaways
• 2
  Where precision is actually lost on a CNC machine
• 3
  Axis count: what each configuration can and cannot do
• 4
  Why setup count matters more than machine resolution
• 5
  Material and geometry set the real tolerance floor
• 6
  Inspection decides whether the tolerance is real
• 7
  Choosing the setup that matches the part

A CNC machine positions a tool tip in space. That sounds simple until you count the error sources. The ballscrew has pitch error. The linear guide has clearance and wear. The spindle grows as it heats. The tool bends under cutting force. The workpiece moves in the fixture. Each source contributes a few micrometres, and they add up in ways that are hard to predict from a spec sheet alone.

This is why a machine rated at ±0.002 mm positioning accuracy does not automatically produce a ±0.005 mm part. Positioning accuracy is measured at the tool tip with no load, at a stable temperature, on a test block. Production cutting adds load, chips, coolant, and time. A CNC precision machining expert spends most of their attention on the gap between the brochure number and the part on the table.

The practical consequence for engineers: ask what the tolerance applies to. A single bore can be held tight because you can measure it and adjust the offset. A 300 mm bolt circle with eight holes at the same tolerance is a different problem. The cumulative angular error around the circle often dominates, and it comes from the rotary table, not the linear axes.

• 1
  Positioning accuracyMeasured unloaded, at stable temperature, at the tool tip.
• 2
  RepeatabilityHow close the machine returns to the same point over many cycles. Matters more for production.
• 3
  Thermal driftSpindle and ballscrew growth over a shift. Can reach 10–20 μm on a long run.
• 4
  Tool deflectionScales with length³/diameter⁴. A long small end mill flexes far more than it looks.

Three-axis machining moves the tool in X, Y, and Z with the part fixed. It is the most rigid and the most predictable setup. For prismatic parts with features reachable from one direction, three axes will match five-axis accuracy at lower cost. GreatLight runs 27 three-axis machines for exactly this reason. The limit appears when a feature faces a direction the tool cannot reach without re-fixturing.

Four-axis adds rotation about one axis, usually A or B. The part turns, so you can machine four sides in one setup. This is common for shafts, housings with bores on multiple faces, and parts with a repeating pattern around a centerline. Twelve four-axis mills handle this class. The gain is not speed. The gain is removing setups, and each removed setup removes a stack of alignment errors.

Five-axis adds two rotary axes, so the tool can approach the part from nearly any direction. Sixteen simultaneous five-axis centers cover contoured surfaces, undercuts, deep cavities, and impeller or blade geometry. The trade-off is that rotary axes add their own error and reduce stiffness at extreme angles. A five-axis machine cutting at a steep angle with a long tool is less rigid than a three-axis machine cutting the same feature straight on.

So the decision is not five-axis versus three-axis in general. It is: how many setups does this part need, and how much error does each setup add? A part that needs five faces machined to ±0.02 mm relative to each other is usually cheaper and more accurate on one five-axis setup than on three three-axis setups. A simple bracket is not.

• 1
  Three-axisBest rigidity and predictability. One face per setup.
• 2
  Four-axisAdds rotational symmetry. Good for shafts and multi-face housings.
• 3
  Five-axis simultaneousContoured and undercut geometry in one setup. Less rigid at steep angles.
• 4
  Five-axis positional (3+2)Machine tilts and locks. Keeps rigidity, still cuts many faces in one setup.

Every time a part comes off the fixture, it must be located again. The new position differs from the old one by a small amount. That amount becomes a positional error between features machined in different setups. On a well-prepared fixture with a dialled-in datum, the shift might be 5–15 μm. On a quick vise setup, it can be 40 μm or more.

This is the strongest argument for fewer setups. It is not about cycle time, although that improves too. It is that relative position between features is the hardest thing to control, and it is controlled by the fixture, not by the machine's resolution. A ±0.005 mm machine with three setups can produce a part worse than a ±0.01 mm machine with one setup.

GreatLight's maximum processing size is 4,000 mm, with travels including 4,000 × 400 × 150 mm, 750 × 1,150 × 550 mm, 600 × 600 × 600 mm, and compact 500 × 500 × 450 mm and 500 × 310 × 200 mm envelopes. A Ø400 mm rotary table handles parts that need rotation. The reason to list these is practical: the machine envelope decides how many setups a part needs, and that decides the achievable tolerance.

• 1
  Single-setup partsRelative feature position is set by the machine, not by the operator.
• 2
  Multi-setup partsAdd one alignment error per re-fixture. Budget for it.
• 3
  Datum choicePick a datum that is machined, not cast or raw stock.

Aluminium 6061 and 7075 cut cleanly and hold tight dimensions. Stainless 304 and 316 work-harden, which pushes cutting forces up and can move thin walls. Titanium TC4 (Ti-6Al-4V) and Inconel resist cutting, generate heat, and spring back after the tool passes. Each of these changes what tolerance is realistic at a given wall thickness.

Geometry matters just as much. A solid block with a bore has a stiff load path. A 1.5 mm wall on a 100 mm long pocket does not. The wall deflects away from the tool during cutting and springs back, so the finished dimension depends on how much material is left and how it was removed. Roughing, stress relief, and finishing passes in sequence give a different result than one heavy pass.

For thin walls the practical rule is to leave more stock for the finish pass, use a smaller radial depth of cut, and accept that the tolerance band widens. A 0.5 mm wall on aluminium is achievable but usually needs a wider band than a solid feature on the same part. A CNC precision machining expert will flag this in DFM before quoting, not after the first article fails.

Temperature is part of the material story. A part measured hot will measure differently when it cools. Aluminium expands about 23 μm per metre per °C. A 1,000 mm aluminium part that is 5 °C warmer than the inspection room measures about 0.1 mm long. That alone can exceed a tight tolerance.

• 1
  Stable and easyAluminium 6061, 6082, brass C36000, mild steel 1018.
• 2
  Work-hardeningStainless 304, 316. Control chipload and avoid dwelling.
• 3
  Heat and springbackTitanium TC4, Inconel. Expect more passes and more inspection.

You cannot claim a tolerance you cannot measure. A CMM with a stated accuracy near the tolerance is not enough. The rule of thumb is that measurement uncertainty should be under one-fifth of the tolerance band. For ±0.005 mm that means a measurement system good to about ±0.001 mm, plus a temperature-controlled room and a stable part.

GreatLight runs raw material checks, in-process monitoring, and final inspection, with 100% inspection before shipment and reports on request. In-process checks matter most. Measuring after the part is finished only tells you whether to scrap it. Measuring between passes tells the operator whether to adjust the offset while there is still stock to remove.

For tight features, the inspection method changes the number. A micrometer on a bore reads a different value than a CMM touch probe, especially on a thin wall, because the micrometer squeezes the material. Both can be correct; they answer different questions. Agree on the method with the customer before production, not after the report is written.

• 1
  Rule of fiveMeasurement uncertainty under one-fifth of the tolerance.
• 2
  TemperatureInspect at 20 °C or record the deviation and correct for it.
• 3
  Method agreementFix the inspection method in the drawing notes or the PO.