Most CNC machine shops quote a standard machining tolerance of ±0.1 mm (about ±0.004 in) for milling and turning, and that is accurate enough for the majority of non-mating part features. Tighter control - down to ±0.02 mm or better on selected features - is achievable but costs more in setups, inspection, and scrap risk. The right approach is to apply general tolerances to most dimensions (ISO 2768 is the standard that defines them) and call out tight tolerances only where parts actually fit, seal, or align. This guide explains the standard values, how ISO 2768 grades work, what limits achievable precision, and where spending more on tolerance genuinely pays off.
What Is a CNC Machining Tolerance?
A machining tolerance is the total permissible variation in a part dimension. Because no cutting process produces identical parts twice, every dimension on a drawing needs an acceptable range. A dimension specified as 25 ±0.1 mm may legally measure anywhere from 24.9 to 25.1 mm; the part is either inside that band or it is scrap.
Two families of tolerances matter in CNC work. Dimensional tolerances control size - a length, diameter, or hole position. Geometric tolerances (defined by the GD&T system, ASME Y14.5 or ISO GPS standards) control form and orientation: flatness, perpendicularity, concentricity, and similar characteristics. The two are related but not interchangeable - a pin can be exactly the right diameter and still be bent, which is why critical mating features often need both a size tolerance and a geometric callout.
Tolerances are also written in two directions. A bilateral tolerance such as ±0.1 mm allows variation both larger and smaller. A unilateral tolerance such as +0.05/−0 mm allows variation in only one direction, which is common for press-fit features where a part must never exceed a maximum size.
Standard CNC Machining Tolerances: Typical Industry Values
Machine shops group tolerance capability into practical bands. The exact numbers vary by shop, machine condition, material, and part geometry, but the following table reflects widely used industry practice for CNC milling and turning of metals.
| Tolerance band | Typical range | What it is used for |
|---|---|---|
| Standard (general) | ±0.1–0.2 mm | Housings, brackets, cosmetic surfaces, non-mating features - the default for most dimensions |
| Precision | ±0.02–0.05 mm | Bearing seats, dowel holes, mating faces, parts that must assemble without rework |
| High precision | ±0.01–0.02 mm | Press fits, spindle and shaft seats, precision gears, gauge and fixture features |
| Ultra precision (selected features only) | Better than ±0.01 mm | Optics mounts, metrology hardware - rare, expensive, and only justified when measurement capability exists downstream |
Two practical rules follow from this table. First, a drawing that leaves dimensions undefined is not tolerance-free - it inherits the shop's standard tolerance, which is why general standards such as ISO 2768 exist. Second, precision is not uniform across a part: a well-clamped aluminum bracket can hold ±0.02 mm on a bore while the same setup struggles to hold ±0.1 mm across a long, thin section that deflects or moves with temperature.
ISO 2768 Tolerance Classes Explained
ISO 2768 is the international standard for general (undefined) tolerances. Instead of tolerancing every dimension on a drawing, the designer adds a single note - for example ISO 2768-mK - and every unmarked linear dimension inherits a permissible deviation based on its nominal size. The four linear classes, from tightest to loosest, are f (fine), m (middle), c (coarse), and v (very coarse).
| Nominal size range (mm) | f (fine) | m (middle) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5–3 | ±0.05 | ±0.1 | ±0.2 | ±0.5 |
| 3–6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| 6–30 | ±0.1 | ±0.2 | ±0.5 | ±1 |
| 30–120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| 120–400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| 400–1000 | ±0.3 | ±0.8 | ±2 | ±4 |
| 1000–2000 | ±0.5 | ±1.2 | ±3 | ±6 |
The letter after the dash covers geometric general tolerances (flatness, perpendicularity, symmetry and so on) in classes H, K, and L - so ISO 2768-mK combines middle linear tolerances with medium geometric tolerances, a very common default for machined general engineering parts. One caution: ISO 2768 applies to dimensions that have no individual tolerance on the drawing. Any dimension you do mark always overrides the general note.
What Limits Achievable Tolerance in CNC Machining?
- Material behavior. Aluminum machines dimensionally stable and cool; stainless steel and titanium generate more heat and tool wear; engineering plastics creep and move with temperature, so a dimension measured at the machine can drift after the part cools - plastics generally cannot hold metal-grade tolerances.
- Part size and stiffness. Variation grows with size. Holding ±0.02 mm across a 30 mm boss is routine work; holding it across a 600 mm face fights machine geometry and thermal drift.
- Feature geometry. Deep pockets, thin walls, and long unsupported spans deflect under cutting forces. Small internal features limit how the part can be measured as much as how it can be cut.
- Workholding and setups. Every additional orientation of the part introduces an alignment error between features. Features machined in one setup hold much tighter relative positions than features tied together across two setups.
- Post-processing. Anodizing adds a ceramic layer that changes dimensions by a few microns; plating adds more. Parts that must stay exact after finishing are either machined to pre-finish sizes or finished with a final cut after treatment.
When Tight Tolerances Are Worth the Cost
Tightening a tolerance is not a linear cost increase - it changes the whole production recipe. Below roughly ±0.05 mm, shops slow down finishing passes, add measurement steps between operations, raise scrap allowances, and may dedicate specific machines or cutters to the job. For prototype quantities the added cost per part is noticeable; for production quantities it compounds across every unit.
That cost is justified exactly where function demands it. Bearing seats, press-fit pins, dowel locations, sealing surfaces, and alignment features between mating parts all need real precision - under-tolerancing them produces assemblies that need hand-fitting or fail outright. Over-tolerancing everything else is pure waste: a cosmetic housing face or a clearance slot gains nothing from ±0.01 mm, and the budget spent there is unavailable for the features that matter. For a deeper look at controlling spend, see our guide on how to optimize CNC machining costs, and our breakdown of choosing between aluminum alloys where material choice also affects achievable precision.
How to Specify Tolerances on Your Drawings
- Add a general tolerance note - for example ISO 2768-mK - and let ordinary dimensions inherit it. This keeps drawings readable and matches how shops plan normal machining.
- Call out tight tolerances only on functional features: fits, seats, seals, and alignment-critical positions. A drawing with three critical dimensions gets more engineering attention than one where every dimension is critical.
- Use GD&T for geometric requirements. If a face must be flat or two bores must be concentric for the assembly to work, say so with a flatness or position callout rather than hoping size tolerances imply it.
- State the measurement reference. Tolerances assume a defined datum and temperature; noting critical features and how they will be inspected prevents disputes later.
- Match tolerances to inspection reality. A tolerance is only as good as the metrology behind it - specify what the part will actually be checked with, and confirm your supplier has that capability before relying on it.
Frequently Asked Questions
What is a standard tolerance for CNC machining?
Most shops apply a standard tolerance around ±0.1 mm for CNC milling and turning when a drawing does not specify otherwise, with metals holding this comfortably. If your drawing carries an ISO 2768 note, the class letter sets the value - for example, class m gives ±0.1 mm for dimensions between 0.5 and 6 mm, widening as parts get larger.
What does ISO 2768-mK mean on a drawing?
It combines two general tolerance settings: m (middle) governs permissible deviations for unmarked linear dimensions, and K governs general geometric tolerances such as flatness and perpendicularity. Any dimension with its own stated tolerance overrides the general note.
What is the tightest tolerance CNC machining can hold?
There is no single ceiling - it depends on the machine, part geometry, material, temperature control, and available metrology. Selected features on rigid, small-to-medium metal parts can be held to ±0.01 mm or tighter by precision-focused shops, while plastics, large parts, and multi-setup features realistically hold looser bands. The practical question is not the extreme limit but whether a feature genuinely needs that level and can be verified with suitable measurement equipment.
How much more do tight tolerances cost?
Cost rises disproportionately below about ±0.05 mm: slower cutting, in-process inspection, higher scrap allowances, and sometimes dedicated tooling or post-process grinding. The exact premium depends on the feature and quantity, so the efficient approach is to tolerance tightly only where parts fit, seal, or align, and leave the rest at standard or ISO 2768 defaults.
Do 3-axis and 5-axis machines hold different tolerances?
Not inherently for a single feature - a dimension's tolerance depends more on material, geometry, and setup than on how many axes moved. Five-axis machining reduces the number of setups for complex parts, which improves the relative position between features machined in one clamping and removes re-clamping error. For a full comparison, see our article on what makes 5-axis CNC machining stand out.
Get Tolerances Right Before You Order
Clear, functional tolerancing is the cheapest way to avoid rework, and our engineers routinely review drawings and flag where a tolerance looks over- or under-specified before quoting. Send your 3D files and drawings through our custom CNC machining services page or request a custom machining quote directly - we will confirm achievable tolerances per feature and quote accordingly, with surface finishing options coordinated so tolerances hold after treatment.
Related: custom CNC machining services | how to optimize CNC machining costs | choosing between aluminum alloys | surface finishing services | what makes 5-axis CNC machining stand out | request a custom machining quote
