CNC Machining: An Accurate Solution
A plain explanation of how CNC machining holds tight tolerances, and where accuracy actually comes from. Written for design engineers and buyers who need to judge whether a part can be machined to tolerance. After reading, you will know which features are easy, which are risky, and when to switch process.
What Makes CNC Machining an Accurate Solution
Accuracy in CNC machining is not one feature. It is the sum of a rigid machine, a correct setup, a controlled cutting path, and a measurement loop that catches drift before the part ships. A good machine alone does not guarantee a good part.
The machine moves a cutter along programmed coordinates. On a three-axis mill, those coordinates are X, Y and Z. The tool stays square to the table, so any face that is not square to the table must be reached by re-fixturing the part. Every new setup adds a datum shift. Datum shifts are where most tolerance is lost.
Five-axis machining adds two rotary axes, usually A and B, so the tool or the workpiece can tilt. A contoured surface, an undercut, or a deep angled hole can be cut without releasing the part. Fewer setups mean fewer datum shifts, and that is the main reason five-axis work holds tighter position tolerance on complex geometry.
- 1Rigidity sets the floorA flexible setup will chatter before the tool wears out.
- 2Setups set the driftEach refixture adds stack-up error, often 0.01–0.03 mm.
- 3Measurement closes the loopIn-process probing catches drift while the part is still clamped.
Which Features Stay Accurate and Which Do Not
Flat faces, through holes, pockets with open corners, and stepped profiles are forgiving. A three-axis machine cuts them in one or two setups, and the tolerance depends mostly on tool wear and thermal drift. On aluminium 6061 with sharp tooling, holding ±0.025 mm on a 100 mm pocket is routine.
Accuracy gets harder as the tool reaches deeper. A long end mill deflects under cutting force, so a deep narrow pocket tends to bell out in the middle. The deflection scales roughly with the cube of the length-to-diameter ratio. A tool at 4:1 ratio is stable; at 10:1 it will push away from the wall on a finish pass.
Thin walls are the other common trap. A wall under 1 mm thick on aluminium will move when the material around it is removed, even if the cutter is perfectly rigid. The part relaxes after unclamping. A design that assumes the wall stays where it was machined will fail inspection.
Sharp internal corners also cause trouble. A rotating cutter always leaves a radius equal to its own radius. If a drawing calls for a true square corner, the only way to get it is EDM or a broach, not milling. Calling out a corner radius that matches a standard end mill avoids a redesign later.
- 1Fits three-axisPrismatic parts, open pockets, through holes, flat datums.
- 2Needs five-axisContoured faces, undercuts, angled ports, compound angles.
- 3Redesign insteadSquare internal corners, walls under 0.8 mm, holes deeper than 10× Ø.
How Tolerance, Finish and Material Interact
Tolerance and surface finish are linked. A finish pass at Ra 0.8–1.6 μm usually means a light depth of cut and a higher spindle speed, which reduces cutting force and helps hold size. A rough pass at Ra 1.6–3.2 μm leaves more material for the finish pass and is where most of the size variation is removed.
Material matters more than most drawings admit. Aluminium 6061-T6 cuts freely and holds ±0.005 mm on a stable setup. Stainless 316 work-hardens at the cut, so a dull tool pushes the surface instead of shearing it, and the next pass cuts a different depth. Titanium Ti-6Al-4V conducts heat poorly, so heat concentrates at the edge and the tool grows. All three can hit the same tolerance, but the process window narrows.
Very tight tolerance on a soft or gummy material is often cheaper to solve by changing alloy than by slowing the machine. Switching from 304 to 303 stainless, or from 6061 to 7075 where strength allows, can remove a finishing operation. That is an engineering trade, not a shortcut.
A tolerance callout should also say what it applies to. A general note of ±0.1 mm with ±0.005 mm only on the bearing bore is easier to make and cheaper than a blanket tight tolerance. Blanket tight tolerance forces every feature through the same slow finishing cycle.
- 1Ra 0.2–0.8 μmFine finish, often needs polishing or lapping after milling.
- 2Ra 0.8–1.6 μmStandard finish pass on most metals.
- 3Ra 1.6–3.2 μmAs-machined, fine for brackets and housings.
Why Accuracy Is a Measurement Problem Too
A part is only accurate if it can be measured. A CMM probe with a 2 mm stylus cannot reach into a 3 mm slot and report a true value. If the drawing tolerance is ±0.005 mm but the feature cannot be probed, the inspection report becomes an opinion. Designers should check that the tolerance can be verified before calling it out.
Temperature is the second measurement issue. Aluminium expands about 23 μm per meter per degree Celsius. A part measured at 28 °C that was machined at 20 °C will read roughly 0.18 mm longer over a 1,000 mm length. That is larger than many tolerances on the drawing. Good shops soak the part and the gauge to the same temperature before final inspection.
In-process probing helps here. Instead of cutting a batch and inspecting at the end, the machine measures a datum or a bore after the finishing pass and offsets the next part. This keeps a run centered rather than drifting to one side of the tolerance band.
For GreatLight, inspection covers raw material check, in-process monitoring and final inspection, with 100% inspection before shipment and reports on request. That is the loop that turns a machine's capability into a shipped part that matches the drawing.
- 1Probe accessCheck that the stylus can reach the feature before setting tolerance.
- 2Thermal soakLet part and gauge settle to the same temperature.
- 3In-process offsetsCorrect drift during the run, not after.
When CNC Machining Is Not the Accurate Answer
CNC machining is a subtractive process. It removes material with a cutter, so it cannot make a part with zero draft on a deep rib, and it cannot match the per-part cost of die casting or injection molding at high volume. Accuracy per part is high; cost per part drops only within the range where the machine time is short.
For a simple bracket at 50,000 units a year, die casting plus a light machining pass on the critical bores is usually cheaper and just as accurate where it matters. For a complex housing at 200 units, CNC is the right call because the tooling cost of the other process would not amortize.
Some features are better made by another process and finished by CNC. A laser-cut sheet metal panel with a machined boss, or a 3D-printed prototype that gets its bearing bore reamed, often beats a fully machined part on both cost and lead time. Mixing processes is normal engineering, not a compromise.
The practical rule: use CNC when the geometry is complex, the volume is low to medium, and the tolerance is tight on a limited number of features. Use casting, molding or printing when the geometry is simple, the volume is high, and the tolerance is loose.
- 1CNC fitsPrototypes, low to medium volume, tight tolerance on key features.
- 2Cast or mold fitsHigh volume, simple geometry, loose tolerance on most faces.
- 3Hybrid fitsForm first, then machine only the critical surfaces.
Three-Axis vs Five-Axis vs Turned Parts
Pick the process by geometry, not by habit.
| Feature | Three-axis | Five-axis | Mill-turn |
|---|---|---|---|
| Prismatic block, open pockets | First choice | Overkill | Not suited |
| Compound angled face | Needs extra fixtures | One setup | Rarely used |
| Deep undercut | Not reachable | Reachable | Not reachable |
| Cylindrical part with cross holes | Two setups | One setup | One setup |
| Tolerance on position | ±0.02–0.05 mm | ±0.005–0.01 mm | ±0.005–0.01 mm |
| Setup count for complex part | 3 to 5 | 1 to 2 | 1 |
| Best batch size | 1 to 10,000+ | 1 to 5,000 | 100 to 50,000 |
The Verdict
If the part has compound angles, undercuts, or a tight position tolerance across several faces, use five-axis CNC machining. If it is a simple prismatic part with one or two tight features, three-axis machining with a good inspection plan is the cheaper and equally accurate route.
Questions Engineers Ask
What tolerance can CNC machining actually hold?
On a stable setup with aluminium or brass, ±0.005 mm is achievable on a limited number of critical features. On stainless or titanium, ±0.01 mm is a more realistic call without adding a finishing operation.
A blanket tolerance across every face is harder and costs more. Put the tight number only where the function needs it.
How does five-axis machining improve accuracy if the machine is the same?
It removes setups. Each refixture adds a datum shift, often 0.01–0.03 mm. Cutting a compound angle in one setup instead of three removes that stack-up.
The rotary axes also let the tool stay normal to a contoured surface, which keeps cutting force even and reduces deflection on thin sections.
Why does my deep pocket measure small in the middle?
Tool deflection. A long end mill bends away from the wall under cutting force, so the middle of a deep pocket bells inward. The effect grows quickly with the length-to-diameter ratio.
Reduce the depth-to-diameter ratio, use a stiffer tool, or take a light spring pass at the end. A rough pass that leaves 0.3 mm for finishing also helps.
Should I call out a surface finish for every face?
No. Call out Ra 0.8–1.6 μm on sealing faces, bearing fits and sliding surfaces. Leave the rest as-machined at Ra 1.6–3.2 μm.
A fine finish on a non-functional face adds machine time and cost without improving the part.
How does temperature affect the measurement of a large part?
Aluminium grows about 23 μm per meter per degree Celsius. Over a 1,000 mm part, a 5 °C difference between machining and inspection is about 0.11 mm, which is bigger than many tolerances.
Let the part soak at inspection temperature before the final check, and use the same reference temperature for the drawing and the report.
When is CNC machining the wrong choice for an accurate part?
At high volume with simple geometry. Die casting, injection molding or stamping will hit the same tolerance on the critical features at a much lower part cost.
A better plan is often hybrid: form the part with the cheaper process, then machine only the bores, faces or threads that need the tight tolerance.
Send the Drawing, Get an Accuracy Check
We review the drawing for features that cannot be machined or measured as called out, and return a quotation with free DFM analysis within 12 hours. No minimum order quantity, from one prototype to 10,000+ part runs.
12-hour quote100% inspectionNDA on request±0.005 mm
More From GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
