CNC Machining Tolerances: What ±0.005 mm Really Means

The short answer

A tolerance defines the permissible deviation from a nominal dimension. When you write ±0.005 mm on a print, you are asking the machinist to hold the finished feature within a five-micron window. That is a capability limit, not a default setting. In our facility in Dongguan, China, we operate over 50 CNC machines capable of holding machining tolerances to ±0.005 mm, but we only target that band when the assembly demands it. Applying your tightest tolerance to every dimension forces the shop to treat the entire part as critical, driving up cycle time and scrap rates for no functional benefit. Reserve the tightest callouts strictly for features that govern fit, sealing, or motion.

Where ±0.005 mm comes from

Holding a five-micron window is not just about buying an expensive machine. It requires controlling five interacting variables simultaneously:

• Machine rigidity and repeatability: the spindle bearings, ballscrews, and guideways must resist deflection under cutting loads and return to the exact same coordinate cycle after cycle.
• Tool wear and geometry: a fresh end mill cuts differently from one that has run for two hours; tool life management must match the tolerance requirement.
• Thermal stability: friction from cutting and ambient temperature shifts expand both the workpiece and the machine structure by microns per degree.
• Workholding pressure: clamping force strong enough to prevent vibration can distort thin-walled features, releasing that distortion only after the clamps are removed.
• Metrology resolution: you cannot control what you cannot measure, so the inspection instrument must have significantly finer resolution than the tolerance itself.

General tolerance vs critical callouts

A well-drawn print relies on a general tolerance block — typically referencing ISO 2768 or ASME Y14.5 — to cover non-critical dimensions such as overall length or clearance holes. Only the features that interface with other components receive individual, tighter callouts. If every dimension on your drawing carries a ±0.005 mm note, the machinist must slow down feed rates, change tools more frequently, and inspect every single feature rather than sampling. Tightening every dimension on a drawing raises manufacturing cost without improving assembly performance. Separate your functional requirements from your general geometry to keep the project economical.

A cost ladder

The relationship between tolerance and cost is non-linear. Moving from ±0.05 mm to ±0.01 mm might double the machining time; moving from ±0.01 mm to ±0.005 mm can double it again. The table below illustrates relative process steps and cost direction. These are engineering guidelines, not a quotation.

Tolerance band	Typical process approach	Relative cost direction
±0.1 mm	Standard roughing and finishing passes on conventional CNC mills or lathes	Baseline
±0.05 mm	Controlled finishing pass with sharp tooling; standard inspection	Slightly higher
±0.02 mm	Dedicated finishing tools, stable thermal environment, frequent in-process checks	Moderate increase
±0.01 mm	Precision boring or fine milling, strict setup protocols, full feature inspection	Significant increase
±0.005 mm	Multi-step finishing, climate control, dedicated fixturing, advanced metrology	Steep increase

For context on what our shop floor handles daily, review our full capabilities. We also achieve surface grinding to ±0.002 mm when flatness or parallelism demands it, which sits outside standard milling.

How tolerance interacts with surface finish and plating

Dimensional tolerance does not exist in isolation. Surface roughness removes material from the peaks of a machined surface, effectively shifting the mean diameter. We routinely achieve surface roughness down to Ra 0.4 µm, but requesting a mirror finish on a bore held to ±0.005 mm means the polishing process must stay entirely within that five-micron envelope. Electroplating and anodizing add thickness uniformly. If a turned shaft is machined to the upper limit of its tolerance and then receives a 10 µm nickel plate, the final assembled size will be out of spec. Always calculate the post-treatment dimension, not just the bare metal dimension, when defining your tolerance stack-up.

How tolerances are measured

The measurement tool must be matched to the tolerance band. A digital caliper is suitable for ±0.1 mm work but lacks the repeatability for anything tighter. Micrometers and height gauges handle the ±0.05 mm to ±0.02 mm range reliably. For ±0.01 mm and below, optical or tactile systems become necessary. Our quality department uses Mitutoyo inspection equipment, including height gauges, vision measuring systems (VMS), and coordinate measuring machines (CMM). A widely accepted rule of thumb in precision manufacturing is that measurement uncertainty should consume no more than one-fifth of the total tolerance band. If your tolerance is ±0.005 mm (a 0.010 mm total zone), your gauge uncertainty must be roughly 0.002 mm or less. Otherwise, you cannot confidently distinguish a good part from a bad one.

How to specify tolerances on a drawing

Clean documentation prevents costly misinterpretations. Start by establishing clear datums; a tolerance without a datum reference frame is ambiguous. Apply Geometric Dimensioning and Tolerancing (GD&T) symbols — such as position, flatness, or concentricity — only where they control a specific functional relationship. Avoid redundant dimensioning. If you define a hole location with basic dimensions and a position tolerance, do not also apply a plus-minus coordinate tolerance to the same feature. Ensure your CAD model and your 2D PDF revision match exactly before sending them to the machine shop. If you need guidance on packaging your design data, our article on what files you need for a CNC quote covers the essentials.

When a looser tolerance is the right answer

Loosening a tolerance is not a concession; it is often the correct engineering call. A clearance hole, a cover recess, a cable channel, or a non-mating edge carries no functional load, and holding it to ±0.01 mm buys nothing except cycle time. The practical test is simple: ask what the feature touches, and what happens if it is 0.05 mm off. If the answer is "nothing", the dimension belongs in the general tolerance block.

The same logic applies to surface finish. A Ra 0.8 µm finish on a bracket face doubles polishing time for a surface nobody inspects, while the same money spent holding one sealing face to ±0.005 mm prevents a leak. Precision is a budget: spend it on the features that decide whether the assembly works.

Tolerance checklist

Before releasing a drawing for production, verify these points:

• Apply a general tolerance block to all non-critical geometry.
• Reserve tight callouts (±0.01 mm or finer) exclusively for mating or sealing features.
• Account for surface treatments and plating thickness in your final dimensional stack-up.
• Define a clear datum reference frame using GD&T rather than relying solely on plus-minus limits.
• Eliminate dual dimensioning or conflicting notes on the same feature.
• Confirm that your specified tolerance is measurable with available inspection equipment.