CNC Machining Accuracy Guide: The Five Types Explained
This guide separates the five accuracy types engineers actually argue about, shows what drives each one, and explains when a tight callout is worth the cost. Written for designers and buyers who sign off on drawings.
What the five types of CNC accuracy actually mean
Accuracy gets used as one word in most RFQs, but a shop measures it five different ways. Dimensional accuracy is how close a finished feature sits to the CAD dimension. A 20 mm bore that comes out at 20.003 mm is dimensionally accurate. Positional accuracy is where that feature lands relative to a datum. That number decides whether parts assemble. Surface accuracy covers roughness left by the tool path, measured in Ra or Rz. Geometry or form accuracy is straightness, flatness, roundness and perpendicularity. Repeatability is how closely the same machine repeats a cut across a batch.
Confusing these five is the fastest way to a rejected first article. A part can hold every dimension and still fail because two holes sit 0.05 mm off their true position. The reverse happens too. Loose dimensions on a cosmetic cover are harmless, yet a Ra 0.4 μm callout on a non-sealing face adds polishing time for no functional gain.
The practical rule: decide which type carries the function, then loosen the rest. A hydraulic manifold lives or dies on positional and surface accuracy. A bracket usually needs dimensional accuracy and nothing more.
Tolerance stacking follows the same logic. Each type draws on a different part of the error budget, so a ±0.005 mm positional callout is a different request than a ±0.005 mm size callout. We quote them separately, and the price gap is large.
What drives error on a real machine
Thermal growth is the largest single error source on long cuts. A spindle running for hours adds heat to the structure. Aluminum grows about 23 μm per meter per °C, so a 4,000 mm part on a warm machine can move past 0.1 mm before the tool touches it again. Shops fight this with climate control, warm-up cycles and probing between operations.
Tool deflection scales with load and overhang. A 12 mm end mill hanging 60 mm out of the holder bends under cutting force, and the wall it leaves is thinner at the top than the bottom. Short holders, light radial engagement and climb milling reduce the effect. A spring pass with no added depth cleans up what is left.
Material behavior matters as much as the machine. Titanium (TC4, Ti-6Al-4V) work-hardens at the cut and pushes back on the tool. Thin aluminum walls move after clamping releases. Stress-relieved stock, symmetrical material removal and a rough-then-finish sequence keep the part stable.
Fixturing sets the floor for everything else. A vise with three points of contact on a rough casting lets the part rock. Vacuum tables and custom soft jaws spread the load. On 5-axis work, the setup also has to reach the feature without the holder colliding, which sometimes forces a second operation.
How to set tolerances that hold
Start from the fit, not from habit. If a bearing sits in a bore, the bore tolerance comes from the bearing manufacturer's spec, not from a default ±0.01 mm block. Everything outside the functional chain can move to general tolerances.
Use GD&T where location matters. A true position callout with a datum reference frame tells the shop exactly what to control. A stack of plus/minus dimensions on a bolt circle does not, and it usually costs more to inspect.
Match the finish callout to the job. Ra 0.8–1.6 μm is a normal machined finish and holds on most faces. Ra 0.2–0.8 μm needs a dedicated finishing pass, sometimes hand work, and should only sit on sealing or sliding surfaces.
Respect the ratio between tolerance and feature size. A ±0.005 mm tolerance on a 200 mm aluminum part is a different risk than the same tolerance on a 20 mm steel pin. Long parts accumulate thermal and deflection error across their length.
Ask for a DFM review before the drawing freezes. A 12-hour quote turnaround includes manufacturability notes, and moving one datum early is cheaper than scrapping a first article later.
When the machine choice decides the outcome
Three-axis work covers flat plates, pockets and simple profiles. It holds tight dimensions well as long as the part can be reached from a few directions. Most brackets, heat sinks and housings never need more.
Four-axis adds a rotary table, so features on multiple faces get machined in one setup. That removes re-clamping error, which is often the biggest single contributor to positional spread.
Five-axis simultaneous motion handles impellers, turbine blades, medical implants and organic surfaces. The controller tilts the tool to keep a constant contact angle, which also lets you use a shorter, stiffer tool. GreatLight runs 16 simultaneous 5-axis centers, alongside 12 four-axis mills and 27 three-axis machines.
Machine size is a separate constraint. Our largest travel is 4,000 × 400 × 150 mm, with medium envelopes at 750 × 1,150 × 550 mm and 600 × 600 × 600 mm. If a part does not fit, no tolerance discussion matters.
Inspection closes the loop. We check raw material, monitor in process and inspect 100% before shipment, with reports on request. CMM data on the first article shows whether the process, not just the part, is in control.
Five accuracy types and what moves them
Typical achievable values at GreatLight; your part geometry may shift these.
| Accuracy type | What it controls | Main error source | Typical target |
|---|---|---|---|
| Dimensional | Feature size vs CAD | Tool wear, thermal drift | ±0.005 mm |
| Positional | Feature location vs datum | Machine geometry, setup | ±0.01 mm |
| Surface | Ra / Rz roughness | Tool marks, vibration | Ra 0.8–1.6 μm |
| Form | Flatness, roundness | Deflection, clamping | 0.01 mm / 100 mm |
| Repeatability | Part-to-part spread | Backlash, wear | ±0.005 mm |
Where to spend the tolerance budget
If the feature carries a fit, seal or motion, hold it tight and inspect it. If it is cosmetic or clearance-only, open the tolerance to general and put the savings into the surfaces that matter.
Common questions
Can you hold ±0.005 mm on every part in a run?
±0.005 mm is our stated capability, and it is checked per feature, not per part. A 20 mm bore on a rigid steel part is a different proposition than a thin aluminum wall 300 mm from the datum.
We confirm what is realistic during the DFM review, before the first chip is cut. If a callout cannot hold repeatably, you hear it early, not after a failed first article.
Why does a tighter surface finish cost so much more?
Ra 0.8–1.6 μm comes off a normal finishing pass. Ra 0.2–0.8 μm needs a smaller stepover, a fresh tool and often a separate operation, which adds spindle time.
On internal bores and deep pockets, polishing may be manual. Put the fine callout only where the surface does work, such as a seal land or a sliding bore.
Does a tighter tolerance always mean a better part?
No. Tolerances beyond what the function needs add cost and inspection time without improving the assembly.
They can also force process changes that hurt other features, like extra clamping that distorts a thin wall.
How do you check positional accuracy on a complex part?
We use CMM inspection with a datum reference frame taken from the drawing. Free-form surfaces are compared against the CAD model rather than measured point by point.
For critical features, in-process probing on the machine catches drift before the part leaves the fixture.
What materials are hardest to hold tight on?
Titanium grades such as TC4 (Ti-6Al-4V) and nickel alloys like Inconel work-harden and deflect. Thin aluminum walls move after unclamping.
Stress-relieved stock, symmetrical cuts and a rough-then-finish sequence keep them in range. Plastics like POM and PEEK need slower feeds to avoid melting.
Can a prototype and a production run hold the same accuracy?
They can if the process is the same. Moving from a 5-axis setup to a dedicated fixture usually improves repeatability, not the reverse.
What changes is inspection volume. We still inspect 100% before shipment and can supply reports on request.
Send the drawing, get an accuracy answer
Upload your CAD files for a quote and free DFM analysis within 12 hours. No minimum order quantity, from one prototype to 10,000+ parts.
12-hour quote100% inspectionNDA on request
More machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
