CNC Machine Tolerance: What a Shop Can Actually Hold

• 1
  What CNC machine tolerance actually measures
• 2
  Where the practical limits come from
• 3
  Seven factors that eat your tolerance
• 4
  How to set a tolerance that buys function, not ego
• 5
  How we hit tight tolerance on a real job
• 6
  Typical tolerance by process and feature

Tolerance is the allowed spread on a dimension. A 25 mm bore drawn at ±0.05 mm may land anywhere from 24.95 to 25.05 mm and still pass. The number says nothing about the machine alone. It describes a system: spindle, tool, fixture, material, thermal state, and the person deciding when to stop cutting.

So the honest answer is a range, not a single figure. In our shop, ±0.005 mm (±0.0002 in) is the working production tolerance on critical features in metals, checked at 20 °C. That is a repeatable number across a run, not a lucky single part.

Two more numbers matter as much as the dimensional one. Surface finish and geometric tolerance decide whether a part assembles and seals. A shaft can sit dead-center on diameter and still fail if it is bowed 0.03 mm over 200 mm.

When you write a tolerance, you are really writing a test plan. Ask what instrument will check it, at what temperature, and how often. If nobody can answer that, the callout is decoration.

• 1
  DimensionalDiameter, length, slot width. Measured with a micrometer or CMM.
• 2
  GeometricFlatness, concentricity, position. Measured against datums.
• 3
  SurfaceRa in μm. Affects friction, sealing, and fatigue life.

A three-axis mill with a 40-taper spindle and a vise can hold ±0.025 mm all day. Push toward ±0.010 mm and you start fighting thermal drift, tool push-off, and chip evacuation. The machine is not suddenly inaccurate. The error budget just gets used up faster.

Five-axis simultaneous machining changes the picture. On our 16 simultaneous 5-axis centers, we cut contoured features in one setup, so stacked datums disappear. That removes one of the largest error sources: re-fixturing a part four times and adding four locating errors.

Spindle speed and tool runout set the floor for surface finish. A balanced holder at 12,000 rpm with 0.005 mm runout gives a predictable Ra. The same tool in a worn holder at 0.03 mm runout will chatter and smear, and no amount of feed adjustment fixes it.

Machine geometry also limits size. Our largest travel is 4,000 × 400 × 150 mm. A 3,000 mm rail can be milled in one pass, but holding ±0.01 mm over that length requires temperature control and a warm-up cycle before the first cut.

• 1
  3-axis±0.025 mm typical, ±0.010 mm with care
• 2
  4-axisAdds rotary positioning to ±0.01 mm on indexed faces
• 3
  5-axisContoured features in one setup, fewer datum stacks

Thermal expansion is the biggest silent killer. Aluminum grows about 23 μm per meter per °C. A 500 mm part that warms 5 °C during roughing moves 0.0575 mm before finishing starts. That is why we rough, cool, then finish.

Tool deflection scales with stick-out cubed. A 6 mm end mill hanging 40 mm out of the holder bends far more than the same tool at 20 mm. For tight slots, use the shortest tool that reaches, and take lighter radial cuts.

Fixture rigidity decides whether the part moves. Thin walls and unsupported bosses deflect under clamping force and spring back after unclamping. Soft jaws machined to the part profile fix most of this.

Material behavior matters too. 6061-T6 machines cleanly and holds ±0.005 mm well. 316L stainless work-hardens, pulls tools, and needs slower speeds. Inconel and Ti-6Al-4V move more after cutting because residual stress releases.

Tool wear drifts dimensions across a run. On a 500-piece order, the tenth part and the five-hundredth part come off different tool edges. In-process probing or scheduled offsets keep the spread tight.

Machine condition is the last item but not the least. A spindle with 0.002 mm runout cannot produce a ±0.005 mm bore reliably, no matter what the control says.

Finally, the programmer sets the outcome. Conservative speeds and a spring pass cost seconds. Chasing a scrap bin costs hours.

• 1
  ThermalRough, cool, finish. Measure at 20 °C.
• 2
  DeflectionShort tools, light radial engagement, rigid fixtures
• 3
  WearProbe or offset every 20–50 parts on long runs

Start from the fit, not the machine. If a bearing sits in a housing, look up the recommended fit for that bearing size and load. That number comes from the bearing maker, not from what feels precise.

Tolerance only the features that touch something. A mounting face, a bore, a locating pin hole. Free surfaces, clearance holes, and cosmetic edges can carry ±0.1 mm or a general title-block tolerance. This one habit cuts cost more than any other.

Watch stacked tolerances. Four parts in an assembly, each at ±0.05 mm, can put the last feature 0.2 mm off nominal. Sometimes the right fix is a tighter single datum feature and looser everything else, not four tight parts.

Ask about the inspection plan before you freeze the drawing. If a ±0.005 mm callout needs a CMM with a temperature-controlled room, that is fine. It just belongs in the quote conversation, not in a surprise email after delivery.

Also decide early whether the tolerance applies to the finished part or the as-machined part. Anodizing adds 5–25 μm per surface. A hardcoat can add more. Plating and coating change dimensions after the last cut.

• 1
  Tight only where it touchesFit surfaces tight, everything else general
• 2
  Check the stackSum the tolerances before you tighten one part
• 3
  Finish firstAccount for coating thickness in the drawing