CNC machining accuracy: where the error comes from

• 1
  What CNC machining accuracy actually measures
• 2
  Where CNC machining accuracy goes wrong: the seven sources
• 3
  Why hole position and hole size need separate budgets
• 4
  Material behavior changes the achievable number
• 5
  How we hold CNC machining accuracy in a production run
• 6
  Tolerance bands and what they cost in process

Accuracy is how close a finished feature lands to the nominal dimension on the drawing. Repeatability is how close repeated cuts land to each other. They are not the same number, and the difference matters when you are planning a run of 10,000 parts. A machine can be repeatable to ±0.002 mm and still be off nominal by 0.01 mm if its ballscrew compensation is stale.

In a shop, accuracy is quoted as a working limit, not a machine spec sheet number. When we say ±0.005 mm on a metal part, that figure already includes the machine, the fixture, the tool, the material, and the temperature of the room at the time of the cut. It is an end-to-end number, and it only holds for features we can actually reach with a probe or a CMM.

Positional accuracy and profile accuracy are separate budgets. A hole center can be right where the drawing says while its diameter runs 0.01 mm large, because those errors come from different places. Boring a hole to size depends on tool wear and spindle runout; putting it in the right place depends on axis scale feedback and fixture repeatability. Keep them apart when you write the drawing.

The last piece is surface finish, which is not accuracy but is often bundled with it. A tight tolerance on a rough surface is hard to inspect and hard to hold. Ra 0.8–1.6 μm is a normal machined finish for aluminum and steel; Ra 0.2–0.8 μm needs a finishing pass or a secondary operation and adds cost.

• 1
  AccuracyDistance from nominal to actual measured value.
• 2
  RepeatabilitySpread between repeated cuts under the same setup.
• 3
  Position vs sizeTwo budgets. Do not merge them on the drawing.

Machine geometry comes first. A three-axis mill with worn linear guides will show straightness error over a 500 mm travel long before it shows a bad diameter. On a five-axis center, rotary axis tilt and center offset stack on top of the linear axes, and a small rotary misalignment gets multiplied by the distance from the rotary center to the cutting edge. That is why long parts on a five-axis table need a probe check after clamping.

Thermal drift is the second source and the one people underestimate most. A spindle running at 12,000 rpm for two hours grows a few tens of microns in Z. Aluminum expands roughly 23 μm per meter per degree C, steel about 11 μm. A part that measures on size at 8 am can measure 0.01 mm over at 2 pm if the shop warms up and no one compensates. We run roughing and finishing on separate setups for tight parts so the finishing cut happens on a settled machine.

Tool deflection is third. A 6 mm end mill hanging 40 mm out of the holder bends under cutting force. In aluminum at moderate feed, deflection can reach 0.02–0.05 mm on a finishing pass. The fix is not always a slower feed; often it is a shorter gauge length, a larger diameter, or a different toolpath that keeps radial engagement low. Long thin tools will always walk.

Workholding is fourth. A part clamped in a vise distorts. Release it and the hole you just bored is no longer round. Thin-wall parts, rings, and housings are the usual victims. Light clamping with soft jaws, or holding on a surface that gets machined away later, keeps the geometry honest.

Spindle runout, ballscrew backlash, and servo following error round out the list. Runout shows up as a lobed bore. Backlash shows up as a step when the axis reverses. Following error shows up on corners where the machine decelerates. None of these are fixed by slowing down the program. They are mechanical or control issues and they need maintenance or compensation, not a feed override.

Metrology closes the loop. If the inspection method has 30% of the tolerance band in its own uncertainty, you cannot tell a good part from a marginal one. A caliper on a ±0.005 mm bore is not a measurement. Use a bore gauge, a micrometer, or a CMM, and match the instrument to the tolerance.

• 1
  GeometryWorn guides, rotary offset, scale error.
• 2
  ThermalSpindle growth, shop temperature swing.
• 3
  DeflectionTool bending under cutting force.

A bolt pattern is a position callout. It depends on how well the machine can move the part under the spindle and how well the fixture locates it. If your fixture has 0.02 mm of play and your position tolerance is 0.03 mm, most of the budget is already gone before the first chip. Probing the fixture datums on the machine recovers some of it.

A bore diameter is a size callout. It depends on tool wear, spindle runout, and thermal growth of the tool and part. A reamed hole in aluminum can hold ±0.01 mm for a few hundred parts; after that the reamer wears and the hole drifts small. This is why high-volume bores go to a boring head or get measured every 50 parts and offset in the control.

When a drawing puts position and size on the same hole with a tight band, the shop has to satisfy both, and the cost is set by the harder of the two. Often loosening one by a factor of two keeps the function and removes a whole inspection step. Talk to the designer about which one the assembly actually needs.

True position at MMC lets you trade size for location. If the hole is at its maximum material condition, you get bonus tolerance for position. Engineers who understand this can open a pattern from 0.05 mm to 0.08 mm without changing function, and that is the difference between a probe check and a full CMM layout on every part.

• 1
  PositionFixture repeatability and axis feedback.
• 2
  SizeTool wear, runout, thermal growth.
• 3
  MMC bonusTrade size for location on the drawing.

Aluminum cuts clean and holds tight tolerances well, but it moves. 6061-T6 and 7075 machine to ±0.005 mm on a stable setup. Thin walls deflect and spring back after unclamping. A 1 mm wall on a 100 mm long pocket will not hold ±0.02 mm without a stress-relieved blank and light finishing passes. If the part is hogged from plate, expect movement after material removal.

Stainless 303 and 304 work harden. If the tool rubs instead of cutting, the surface hardens and the next pass deflects more. Sharp tools, positive rake, and no dwell in the cut keep the tolerance stable. 17-4PH in the H900 condition is harder and needs more passes at lower depth of cut. Surface finish on stainless tends to run Ra 1.6–3.2 μm unless you add a finishing pass.

Titanium Ti-6Al-4V is the hard case. Low thermal conductivity means heat goes into the tool and the part. Deflection and thermal growth both increase, and tool life drops. Tolerances of ±0.02 mm are routine; getting to ±0.005 mm means slow finishing, plenty of coolant, and a check on the machine after the part cools. Inconel is slower again and usually lands around ±0.05 mm unless the feature is ground.

Plastics and composites behave differently. POM and PEEK move with temperature and humidity. Carbon fiber delaminates if the tool pushes instead of shears, and the cut edge can fray. For these materials, accuracy is often limited by fixturing and edge quality, not the machine. Sharp carbide, high spindle speed, and low feed per tooth give the best result.

• 1
  Aluminum±0.005 mm reachable, watch thin walls.
• 2
  StainlessWork hardening, keep the tool cutting.
• 3
  TitaniumHeat and deflection dominate. Plan slower.