Tolerance guide

How Precise Are CNC Machines?

Short answer: a modern machining center holds ±0.005 mm on a well-planned part, and ±0.001 mm only under conditions worth understanding. This guide shows how to define the tolerance your part actually needs, which machine and setup can hold it, and how to check the result instead of trusting a spec sheet.

Get Instant Quote Talk to an Engineer

±0.005 mm standardRa 0.8–1.6 μm finish4,000 mm max size100% inspection

How precise are CNC machines – 5-axis machining center cutting a metal part

On this page

Key takeaways

One number is not enoughAccuracy is what the machine reaches; repeatability is what it holds across a batch. Buyers need the second one.

±0.005 mm is the working floorThat is our standard callout for milled and turned metal parts inside stable thermal conditions.

±0.001 mm needs special handlingIt is possible on small features, but only with temperature control, light cuts and slow feed rates.

The part decides, not the machineLong thin walls, deep pockets and soft plastics move after the cut. Those are process problems.

Measure before you promiseEvery claim in this article is verified by inspection reports, not by a machine brochure.

Definitions

What precision actually means on a CNC machine

When an engineer asks how precise are CNC machines, the useful answer separates three numbers. Accuracy is the gap between the commanded position and the real position of the tool tip. Repeatability is how tightly the machine returns to the same point over hundreds of cycles. Resolution is the smallest step the control can command, and it is usually far smaller than either of the other two. A machine can resolve 0.1 μm and still cut 0.02 mm off target if the ballscrew is warm.

Tolerance is a third thing again. It is the band printed on your drawing, and it belongs to the part, not the machine. A drawing callout of ±0.005 mm on a 50 mm aluminum bracket is routine work. The same callout on a 900 mm thin-wall housing is a different project: it needs roughing, a stress-relief pause, a finishing pass with light depths of cut, and a controlled room. Same machine, different plan, different risk.

So the honest answer to “how precise are CNC machines” is a range, not a figure. General milling and turning hold ±0.05 mm easily. Our standard envelope is ±0.005 mm (±0.0002 in) for metals on features we can reach in one or two setups. Below that, accuracy stops being a machine property and becomes a metrology and thermal-management exercise.

1
AccuracyCommanded position versus actual tool tip position.
2
RepeatabilitySpread of results across a batch at the same nominal target.
3
ResolutionSmallest control increment; the least useful of the three.
4
ToleranceThe band on your drawing; a part requirement, not a machine spec.

Process physics

Seven factors that move the number

Thermal growth is the largest single error source on a running machine. Steel expands about 11 μm per meter per °C. A spindle that warms 5 °C during a long roughing cycle shifts the tool tip, and the finishing pass then cuts a part that no longer matches the probing done at 8 a.m. Shops handle this by warm-up cycles, coolant temperature control, and by scheduling tight-tolerance finishing early rather than after four hours of heavy cutting.

Tool condition is next. A sharp carbide end mill cuts with predictable radial force. A worn one rubs, pushes the workpiece, and leaves both a size error and a poor finish. We track tool life by material and by feature: aluminum runs long, 17-4PH and Inconel do not. When a job calls for ±0.005 mm on a deep pocket, changing the tool before the last pass costs less than scrapping the part.

Workholding and material behavior decide the rest. Aluminum 6061 moves when you remove 70 percent of its cross-section, because internal stress releases as material leaves. Titanium and stainless work-harden if the feed is too light, so a cautious programmer can make the surface harder than the cutter. Plastics such as POM and PEEK expand with heat and spring back after the tool passes, so the finished bore measures smaller than the cut.

Fixturing errors hide until final inspection. A vise clamped on a thin floor bows the part; after unclamping it springs back and the flatness callout fails. Vacuum plates, soft jaws machined to the part profile, and sacrificial tabs all reduce this. On a 4,000 mm part, we plan support points before we plan toolpaths, because deflection over that length is measured in tenths of a millimeter, not microns.

Programming choices set the ceiling for everything else. Trochoidal paths, constant chip load, and a separate finishing pass with 0.2–0.3 mm radial engagement all protect the final dimension. Ramping into a pocket instead of plunging avoids tool deflection at the entry. A single roughing pass that removes 6 mm of radial stock will not hold ±0.02 mm on the wall, let alone ±0.005 mm.

Environmental vibration matters more than most buyers expect. A surface grinder next door, a forklift route, or an unbalanced load on a lathe all show up in the Ra reading. Machines on isolated pads in a temperature-controlled bay hold their numbers through a night shift. Machines in an open bay do not, and no amount of probing fixes that.

Finally, metrology limits the claim. If the shop measures with a caliper, the real uncertainty is around ±0.02 mm. A coordinate measuring machine in a controlled room, or a micrometer with a known reference, is what turns a tolerance into a verified number. Ask what instrument produced the report before you accept it.

1
Thermal driftWarm-up cycles and coolant temperature control; finish tight features early.
2
Tool wearReplace before the finishing pass on hard alloys.
3
Material stressRough, pause, then finish thin-wall parts.
4
MetrologyA caliper cannot verify a ±0.005 mm callout.

Machine classes

How machine type changes the achievable tolerance

Three-axis vertical mills are the workhorse for flat plates, brackets and housings open on one side. They reach the part from above only, so every face you need must be reachable in one orientation, or the part goes back for a second setup. Each additional setup adds roughly 0.01–0.02 mm of stack-up from re-clamping, which is why a ±0.005 mm callout across four faces usually pushes the job to a different machine class.

Four-axis mills add a rotary table, typically Ø400 mm, so the part indexes around one horizontal axis. This is the right choice for shafts with cross-drilled holes, cylindrical parts with milled flats, and any job where you would otherwise need three or four manual setups. Angular position between indexed features gets much tighter because the part never leaves the fixture.

Simultaneous five-axis centers cut with the tool tilted, so a single continuous pass can follow a curved surface or reach under a flange. For precision work the gain is not speed, it is setup count. A part machined in one five-axis setup avoids the re-clamping error entirely, and geometry that would need electrodes on a three-axis machine can be milled directly.

Mill-turn centers combine turning and milling in one spindle, which suits parts like valve bodies and sensor housings with a turned bore and milled side ports. Concentricity between the bore and the port pattern stays tight because the part is never re-chucked. Where a job needs both a Ø0.02 mm bore tolerance and a bolt circle, this is usually the cheapest route to the drawing.

None of this replaces process planning. A five-axis machine cutting a poorly supported thin wall will still fail inspection. The machine class only removes setup error; it does not remove thermal error, tool deflection or material movement.

1
3-axisOne orientation; best for flat and open geometry.
2
4-axisAdds Ø400 mm rotary indexing; fewer setups on shafts.
3
5-axisOne-setup access to five faces and undercuts.
4
Mill-turnTurned bore plus milled features without re-chucking.

Part design

Features that break a tight tolerance

Some geometry simply cannot hold ±0.005 mm, no matter which machine cuts it. A wall 0.8 mm thick and 60 mm tall will deflect under cutting force and then spring back. It is machinable, but the achievable tolerance is closer to ±0.03 mm, and the honest move is to say so before the quote rather than after inspection.

Deep pockets with a small corner radius are a second case. A Ø3 mm end mill reaching 30 mm deep has a length-to-diameter ratio of 10:1, which means it bends. The practical fix is to open the corner radius to at least 1.2 times the cutter diameter, or accept a larger tolerance at the floor of the pocket.

Holes with tight position and tight diameter at the same time are a third. If a Ø6 mm hole carries both an H7 fit and a ±0.01 mm position callout, drilling and reaming may not be enough. Boring in a second operation, or interpolating with a smaller cutter and finishing with a single spring pass, holds both.

Threads are often over-specified. A class 3 thread is not needed for a fastener that sits in a clearance hole. Class 2H is standard, cuts faster, and reduces the risk of a gauge failure. Reserve tight thread classes for parts that see vibration or repeated assembly.

Surfaces that must seal or slide need a finish callout, not just a size callout. A Ra 0.2–0.8 μm sealing face is a separate operation after the dimensional cut. If the drawing shows only a diameter and no Ra, the machined finish will be Ra 1.6–3.2 μm, which may leak under pressure.

1
Thin wallsUnder 2 mm, expect ±0.02 mm or looser.
2
Deep pocketsKeep corner radius at 1.2 × cutter diameter.
3
Small holesBore or spring-pass when diameter and position are both tight.
4
Sealing facesSpecify Ra separately from size.

Workflow

How to hold precision on a real job

Follow this order. Skipping a step is how parts fail inspection.

1
1. Read the drawing for function, not just numbersSeparate the dimensions that must mate with something from the ones that are informative. A ±0.01 mm callout on a clearance hole wastes money; a ±0.02 mm callout on a bearing seat is a risk. Send the drawing for DFM review before quoting, and ask which tolerances can be opened.
2
2. Fix the datum scheme firstChoose three datums that a single setup can reach, and use them consistently from raw stock through final inspection. If the datum is on a face that only appears in operation three, the whole tolerance stack becomes guesswork.
3
3. Match the machine class to the setup countOne setup: 3-axis. Two to four sides: 4-axis or 5-axis. Turned bore plus milled ports: mill-turn. Every extra setup adds roughly 0.01–0.02 mm of position error from re-clamping.
4
4. Plan the roughing and finishing splitLeave 0.3–0.5 mm radial stock for finishing on aluminum, 0.2–0.3 mm on stainless and titanium. Cut finishing at higher spindle speed, lower feed per tooth, and a constant engagement of 5–10 percent of cutter diameter.
5
5. Manage heat before the finish passRun the spindle warm-up cycle, confirm coolant temperature is stable, and probe the part again immediately before finishing. On long cycles, finish the tight features in the first two hours of the shift.
6
6. Control thin walls and stress releaseRough both sides of a thin wall symmetrically, then pause. For aluminum parts with heavy stock removal, a stress-relief step or a rough-and-requalify sequence keeps the wall from bowing after unclamping.
7
7. Inspect with the right instrumentUse a CMM in a controlled room for ±0.005 mm work, a micrometer or bore gauge for diameters, and a profilometer for Ra. Record the temperature at inspection, because a 3 °C difference explains a 0.003 mm shift on a 100 mm steel part.
8
8. Freeze the process after approvalOnce first article passes, lock the program, tool list, fixture and inspection method. A tool change from a different supplier can move the finish by one Ra band even when the size stays inside tolerance.

Capability matrix

Tolerance and finish by process and feature

Figures are our standard production envelope, not a laboratory best case.

Feature or process	Typical tolerance	Typical finish	When to use it
3-axis milling, flat plate	±0.02 mm	Ra 1.6–3.2 μm	Brackets, covers, open housings
4-axis milling, indexed	±0.01 mm	Ra 1.6 μm	Shafts, cross-drilled parts
5-axis, one setup	±0.005 mm	Ra 0.8–1.6 μm	Complex geometry, five faces
CNC turning, Ø under 100 mm	±0.005 mm	Ra 0.8–1.6 μm	Bores, pins, bushings
Fine finish pass	±0.005 mm	Ra 0.2–0.8 μm	Sealing faces, sliding surfaces
Thin wall under 2 mm	±0.02 mm	Ra 1.6 μm	Lightweight housings, heat sinks
Large part up to 4,000 mm	±0.05 mm	Ra 3.2 μm	Frames, rails, long beams
Plastic, POM or PEEK	±0.05 mm	Ra 1.6–3.2 μm	Insulators, low-load parts

Set the tolerance your part needs, then verify it

±0.005 mm is achievable across milling, turning and five-axis work, but only when the drawing, the setup plan and the inspection method agree. Send the drawing and we will tell you which callouts are costing money and which ones are genuinely tight.

Get Instant Quote Talk to an Engineer

FAQs

Questions engineers ask about CNC precision

What tolerance can a CNC machine hold on a normal production part?

For milled and turned metal parts, ±0.005 mm (±0.0002 in) is a realistic production tolerance when the features are reachable and the part is not thin-walled. Many parts do not need it; ±0.02 mm covers most brackets and housings and costs less.

Tighter than ±0.005 mm is possible on small diameters and flat faces with temperature control, light finishing cuts and a CMM in a controlled room. It is a special process, not a default.

Does a 5-axis machine always cut more accurately than a 3-axis machine?

No. The five-axis machine wins on setup count, which removes re-clamping error, and on access to undercut geometry. On a simple flat plate, a well-maintained 3-axis mill is just as accurate and faster to program.

Choose five-axis when the part needs four or five faces machined, or when a compound angle would otherwise require a custom fixture.

How does temperature affect the parts you machine?

Steel moves about 11 μm per meter per °C. A 100 mm steel part measured 3 °C warmer than the reference reads about 0.003 mm larger. That is most of a ±0.005 mm tolerance band.

We run spindle warm-up cycles, control coolant temperature, and finish tight features early in the shift. Inspection reports include the measurement temperature when a customer asks for it.

Can you measure ±0.005 mm on the shop floor?

Not with a caliper. Caliper uncertainty is roughly ±0.02 mm, so it cannot confirm a ±0.005 mm callout. We use a CMM in a controlled room, micrometers, bore gauges and a profilometer for surface finish.

Every shipment goes through 100 percent inspection, with raw material checks, in-process monitoring and final inspection. Reports are available on request.

Which materials are hardest to hold to a tight tolerance?

Titanium, Inconel and 17-4PH work-harden and push back on the cutter, so tool wear moves the size quickly. Plastics such as POM and PEEK expand with cutting heat and shrink after, so the finished bore measures undersize.

Aluminum 6061 is the easiest to hold, but heavy stock removal releases internal stress and the part can bow after unclamping. Rough, pause, then finish.

How do I write a drawing that gets an accurate quote?

Put the tight tolerances only on the dimensions that matter, name the datums, and state the surface finish for any face that seals or slides. Add the material condition and the quantity range.

A drawing like that gets a quotation and a free DFM analysis within 12 hours. Production can start within 24 hours, and typical parts ship in 3–5 days.