The CNC tolerance chart every designer should have bookmarked.

Why this matters: tolerances are the silent cost driver.

On a typical CNC-machined part, the choice between ±0.1 mm and ±0.01 mm can change the price by a factor of 3–5. Not because the feature is harder to physically cut — but because of everything that surrounds it: more setup rigidity, finer tooling, in-process measurement, longer cycle times, and higher scrap rates.

Most engineers intuit this. The mistake we see most often is defaulting to tighter tolerances "just to be safe." A block of dimensions all toleranced at ±0.02 mm — when only two of them actually affect fit — quietly doubles the part cost. This guide gives you the reference tables to call out tight tolerances only where they matter.

ISO 2768 general tolerances — the starting point.

ISO 2768 (replacing older DIN 7168) specifies four classes of general tolerance for linear dimensions: fine (f), medium (m), coarse (c), and very coarse (v). Most CNC drawings are called out as ISO 2768-m or ISO 2768-mK. These are the default tolerances for any dimension not otherwise specified on the drawing.

Here is the full table for linear dimensions:

Every CNC shop can meet ISO 2768-m without thinking about it. 2768-f is where you start to pay attention — it's still routine, but parts will get inspected more carefully. The "K" suffix (as in 2768-mK) adds general geometric tolerances: flatness, straightness, symmetry, and runout.

How fobproto thinks about tolerances: three tiers.

Standards are good for drawing callouts, but for quoting we group everything into three tiers that roughly map to process capability and cost:

Linear dimensions — tolerance chart by tier and size.

Achievable on milled and turned parts in soft metals (aluminum, mild steel, brass):

For harder alloys (stainless, Inconel, titanium, tool steel), expect tolerances roughly 1.5× wider at the same tier — or, equivalently, a 30–50% cost premium to hold the softer-metal tolerance.

Hole diameters and hole-to-hole locations.

Holes are where tolerances get tight fast. ISO 286 defines H7/h6/g6 bore fits — here's what CNC can deliver without second-op reaming or boring:

Form and position — GD&T on CNC parts.

ASME Y14.5 geometric tolerances map cleanly onto CNC capabilities — but only if you specify datums correctly. Here are typical achievable values per 100 mm of feature size:

Surface roughness achievable by process.

What each CNC process can actually hold.

Different processes hit different tolerance ceilings. Know which process is cutting your feature before you specify the tolerance:

Five rules for tolerancing a CNC drawing.

ISO 2768 — the general-tolerance standard you should actually use

Most drawings don't need explicit tolerances on every dimension. ISO 2768 provides four tolerance classes (f, m, c, v for linear dimensions; H, K, L for geometric) that handle "general" tolerances across the whole drawing via a single block note.

Call out "ISO 2768-mK" in your drawing's title block and every unspecified dimension gets medium linear (m) + medium geometric (K) tolerances automatically. This is industry standard and every shop worldwide reads it correctly. Use explicit tolerances only on features that truly need tighter than medium — typically 3-8 features per drawing, not the 30-50 we often see.

IT grades — what they mean and what each costs

The ISO IT (International Tolerance) system defines 20 grades, from IT01 (tightest) to IT18 (loosest). In practice, CNC parts live between IT6 and IT13.

A key practical point: the cost of tightening tolerance is not uniform across grades. Going from IT12 to IT11 is a 20% cost bump. Going from IT9 to IT8 is a 2× cost bump. Going from IT7 to IT6 is a 2× bump. Every step down the grade ladder is more expensive than the previous step.

Process-specific tolerance capabilities

3-axis CNC milling

• Linear dimensions: ±0.05 mm standard, ±0.02 mm achievable with care
• Bore tolerance: ±0.025 mm (reamed), ±0.010 mm (bored)
• Flatness: 0.02 mm/100 mm routinely
• Parallelism: 0.03 mm/100 mm typical
• Position tolerance: ±0.05 mm between features on same setup; ±0.1 mm across setups

CNC turning

• Diameters: IT7 standard, IT6 achievable with Swiss machines or precision lathes
• Lengths: ±0.05 mm
• Concentricity: 0.01 mm (single-setup), 0.02-0.05 mm (chuck re-grip)
• Roundness: 0.005 mm on precision lathes

Wire EDM

• ±0.005 mm routinely
• ±0.002 mm with fine-wire setup
• Surface finish: Ra 0.8-1.6 μm as-cut, Ra 0.2 μm after finish pass
• Best for hardened materials or complex internal geometries

Grinding

• ±0.002-0.005 mm on precision surface grinders
• Ra 0.1-0.4 μm surface finish routine
• Required for IT5 and tighter on hardened materials

Material effects on achievable tolerance

Tolerance capability depends partly on material. Aluminum machines more predictably than stainless steel; stainless more predictably than titanium; all three more predictably than PEEK or UHMW.

For tighter-than-achievable specs on any material, the shop needs to add operations — grinding, honing, lapping, or post-machining heat treatment. Each operation roughly doubles the cost of that feature.

GD&T vs ±tolerance — when each makes sense

Linear tolerance (±0.05 mm on a dimension) and geometric tolerance (perpendicularity 0.02 mm to datum A) do different jobs. Most drawings need both:

• Use linear ± tolerance when: the feature is simple, the dimension is what matters, and function is well-defined by location. Examples: diameter of a shaft, length of a part, thickness of a plate.
• Use GD&T when: the relationship between features matters more than any single dimension. Examples: the axis of one bore must be parallel to the axis of another bore; a flat face must be perpendicular to the datum axis; a sealing surface must be flat within a tight limit regardless of where it sits in the drawing.

Over-using GD&T is a common source of cost inflation. If a part has 20 features and the drawing calls out position tolerance, perpendicularity, parallelism, and flatness on all 20, inspection time alone can exceed machining time. On the other hand, under-using GD&T — relying only on ± tolerances for a part with critical assembly relationships — can lead to parts that pass inspection but don't assemble correctly.

Five common tolerance mistakes we see on drawings

From our shop's QA team, the patterns that most often cause quote-to-rejection cycles:

Representative tolerance specs by industry

Different industries have unspoken norms for what tolerance is "normal" — drifting from these raises questions and often requires justification:

If you're specifying aerospace-level tolerances on an industrial-machinery application, you're overpaying. If you're specifying industrial-level tolerances on aerospace work, you'll have assembly problems. Matching tolerance expectations to industry norms is a cheap shortcut.

Measurement uncertainty — the ignored factor

A ±0.02mm tolerance only means something relative to the measurement method used to verify it. Common inspection tools and their realistic accuracy:

• Digital caliper: ±0.02-0.05 mm repeatable. Good for general checking, inadequate for verifying tight tolerances.
• Micrometer: ±0.005 mm on external dimensions. Good for shafts and straight features.
• Bore gauge / plug gauge: ±0.002-0.005 mm on internal diameters. Slow but accurate.
• CMM (coordinate measuring machine): ±0.003-0.01 mm depending on machine. The standard for complex geometry inspection.
• Optical comparator: ±0.01 mm on 2D features. Fast for profiles and contours.
• Laser scanner: ±0.05-0.2 mm. Fast whole-surface capture but less accurate than CMM.

A tolerance band needs to be about 4× larger than the measurement uncertainty for reliable inspection (the 4:1 rule). Spec'ing ±0.005 mm tolerance on a feature that can only be measured with a ±0.003 mm method creates a gray zone where parts might pass or fail based on measurement noise alone. Match your tolerance callouts to the practical measurement capability.

Common tolerance questions