UK CNC machining quality and accuracy for every cut

• 1
  Key takeaways
• 2
  What UK CNC machining quality and accuracy actually means on the shop floor
• 3
  How tolerance stacks up across a feature
• 4
  Thermal behavior and why the first part lies
• 5
  The 5-axis setup error nobody talks about
• 6
  Which features are hard to hold, and when to loosen the callout
• 7
  How we verify quality before parts ship
• 8
  The 7 checks that keep accuracy repeatable
• 9
  Where machining error enters the loop
• 10
  When a tight callout is realistic

Accuracy is how close a feature lands to its nominal position. Repeatability is how close it lands on the next part, and the one after that. A machine can be accurate on a warm Monday morning and repeatable only if nothing in the loop changes. Buyers usually ask for the first number and pay for the second.

In practice, the finished dimension is the sum of five moving parts: machine geometry, workholding, tool condition, thermal state and the measurement itself. Each contributes a small error. None of them is visible on a drawing. When a part drifts out of tolerance mid-run, the cause is almost always in that list, not in the CAM program.

GreatLight runs 127 high-precision CNC machines across three wholly-owned plants, with 16 simultaneous 5-axis machining centers. That capacity matters for scheduling, but it does not by itself produce accuracy. What produces accuracy is deciding which machine, which fixture and which probing routine suits a given feature.

This page is about the mechanism, not a sales pitch. We explain where error enters, which features are hard to hold, and which checks catch a problem before the parts ship.

A ±0.005 mm callout does not mean every dimension on the part sits inside ±0.005 mm. It means the features you flagged can be held at that band, and only when the process is set up for it. Position tolerance, form tolerance and surface finish share the same physical space. Tighten one and the others get harder.

Take a bearing bore. The diameter can be dead on while the roundness is 8 μm out, and the bearing still feels rough. Or the bore is round and on size, but the shoulder face runs out by 15 μm, so the bearing seats at an angle. Two dimensions passed, the assembly still fails. This is the most common gap between inspection reports and real function.

Surface finish interacts with tolerance too. A Ra 0.8–1.6 μm finish on a sealing face is not cosmetic. Tool marks create leak paths under pressure. On the same face, a Ra 0.2–0.8 μm finish may be needed for a dynamic seal, and that pushes you toward slower feed rates and a finishing pass that adds cycle time.

The practical rule: budget your tolerance in writing before the quote. Say which features are functional, which are reference, and which can float. A supplier who receives a fully dimensioned drawing with no priorities will default to the loosest interpretation that still passes inspection.

• 1
  Functional featuresBores, sealing faces, mating pilots. Hold these tight.
• 2
  Reference dimensionsCan shift without affecting assembly. Let them float.
• 3
  Cosmetic surfacesFinish matters, size often does not. Separate the two.

Metal grows when it warms. Aluminum expands about 23 μm per meter per degree Celsius. A 300 mm aluminum part that heats 5 °C between the roughing pass and the finish pass moves roughly 35 μm. That is seven times a ±0.005 mm tolerance. The machine is not wrong. The part has simply changed size.

This is why the first article can pass and the tenth part can drift. Roughing dumps heat into the workpiece. If finishing follows immediately, the part is still hot and gets cut undersize. When it cools to room temperature, the dimension shrinks past the lower limit.

The fix is boring and effective. Rough, then let the part rest. Finish on a machine that has run a warm-up cycle. Keep coolant at a stable temperature. For long parts, probe the feature before the finish pass and offset the tool path by the measured deviation.

We see the same effect on the machine itself. A spindle that has run for ten minutes is not at the same thermal state as one that has run for four hours. Shops that hold ±0.005 mm routinely schedule warm-up blocks and re-probe the datum after them. It costs cycle time. It buys repeatability.

Invar and titanium behave differently from aluminum. Titanium conducts heat slowly, so the tool edge gets hot while the bulk of the part stays cool. That shifts the problem from part growth to tool wear, and the answer is different: lower surface speed, more coolant pressure, shorter tool life windows.

Five-axis machining removes the need to refixture a part on multiple faces, and that is where most of its accuracy gain comes from. Every refixture adds a new setup error. A 5-axis machine that cuts five faces in one clamping eliminates four of those errors before the tool ever touches metal.

But 5-axis introduces its own stack. Rotary axis centerline offsets, pivot distance errors and thermal growth in the trunnion all shift the tool tip. A 10 μm error at the rotary center becomes a much larger error 300 mm out on the part, because rotation multiplies the offset by the distance from the pivot.

This is why we calibrate rotary axes with a sphere or a test piece rather than trusting the factory parameters. The measured pivot distance goes into the post-processor. Skip that step and the part looks fine near the center and drifts at the edges.

The same logic applies to our 4,000 mm maximum processing size. Long parts amplify every angular error. A 0.01° tilt over 4,000 mm is 0.7 mm of deviation at the far end. If you are quoting a long part, ask how the machine is leveled and how often the geometry is checked.

Thin walls are the classic problem. A 1 mm aluminum wall deflects under clamping force and cutting pressure. The finished part springs back after unclamping, and the measured dimension depends on where you measure it. If the wall is under 1.5 mm, expect to hold ±0.05 mm at best without special fixturing.

Deep holes are the second. A hole with a length-to-diameter ratio above 8:1 needs a pilot hole, peck drilling and high-pressure coolant. Below 4:1, standard drilling holds ±0.05 mm on diameter without drama. Between the two, it depends on the material.

Small radii in hard materials are the third. A 0.5 mm internal corner in 17-4PH stainless needs a small-diameter tool, and small tools deflect. The corner will not be sharp. It will carry a radius roughly equal to the tool radius plus deflection. If the design needs a sharp corner, add a relief or accept a larger radius.

The counter-rule matters as much. Some callouts are tighter than the function requires. A bolt clearance hole does not need ±0.01 mm. A cosmetic edge break does not need a ground finish. Every unnecessary tight callout adds cost and cycle time without adding value, and it can push the shop toward a process that is less stable overall.

Inspection starts with the raw material certificate and the incoming dimensional check. It continues with in-process monitoring during the run and a final inspection before shipment. All parts are inspected; reports are available on request.

For critical features we use a CMM with a calibrated probe. For high-volume runs, we build fixtures that hold the part the same way every time, because measurement repeatability is part of the accuracy budget. A gauge that varies by 3 μm on the same part cannot be used to judge a ±0.005 mm tolerance.

Our quality system is certified to ISO 9001:2015, IATF 16949:2016, ISO 13485:2016 and ISO 27001:2022. Those certificates cover process control, traceability, medical device work and information security. They do not replace a first article inspection, and we do not treat them as if they do.

If a part fails inspection, we do not ship it and hope. We identify the root cause, correct the process and re-run. Our historical late-delivery probability is below 2%, which comes from catching problems at the machine rather than at the loading dock.

Surface finish is checked alongside dimensions. Anodizing, plating, bead blasting and polishing all change the surface, and some of them change the dimension. Hardcoat anodizing adds roughly half the coating thickness to each side. If a bore is held to ±0.005 mm and then hardcoated, the coating must be masked or the tolerance must be adjusted before plating.