A machining tolerance is the total variation a drawing allows from a specified dimension. It is written as a plus-or-minus value, a pair of limits, a fit class or a geometric callout. No process holds zero variation, and every step tighter adds operations, inspection time and scrap risk. The skill is putting tight limits only where the part needs them. See what we can make in our CNC machining capabilities, but remember that the number on the drawing decides what the part costs.
Standard machining tolerances: chart in mm and inches
When a drawing has no tolerance on a dimension, the shop falls back on a general tolerance. The figure most often quoted for CNC machining is ±0.005 in (±0.13 mm). Drawings that cite ISO 2768 use the table below instead.
ISO 2768-1 general tolerances for linear dimensions (± mm, inch in brackets)
| Nominal size (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5 to 3 | 0.05 (0.002 in) | 0.1 (0.004 in) | 0.2 (0.008 in) | n/a |
| over 3 to 6 | 0.05 (0.002 in) | 0.1 (0.004 in) | 0.3 (0.012 in) | 0.5 (0.020 in) |
| over 6 to 30 | 0.1 (0.004 in) | 0.2 (0.008 in) | 0.5 (0.020 in) | 1 (0.039 in) |
| over 30 to 120 | 0.15 (0.006 in) | 0.3 (0.012 in) | 0.8 (0.031 in) | 1.5 (0.059 in) |
| over 120 to 400 | 0.2 (0.008 in) | 0.5 (0.020 in) | 1.2 (0.047 in) | 2.5 (0.098 in) |
General tolerances are a floor for features nobody has toleranced on purpose. Anything that mates, seals or locates another part needs its own tolerance on the drawing.
Divine Precision’s published figures for CNC machining tolerances on turned parts and aluminum milled parts sit well inside those general limits. They apply per drawing and are confirmed at quote.
| Feature | Divine Precision | Inch equivalent |
|---|---|---|
| Turned diameter | ±0.01 mm | ±0.0004 in |
| Ground diameter | ±0.005 mm | ±0.0002 in |
| Surface finish, standard | Ra 1.6 µm | about 63 µin |
| Surface finish, on request | Ra 0.4 µm | about 16 µin |
The four types of tolerances
- Limit: the two allowed extremes are written out, for example 24.99 / 25.01.
- Unilateral: all variation goes one way, for example 25.00 +0.00 / −0.02.
- Bilateral: equal variation on both sides, for example 25.00 ±0.01.
- Geometric (GD&T): controls form, orientation, location and runout rather than size alone.
Use bilateral tolerances for general features and unilateral tolerances for fits, where one limit must not be crossed. Geometric tolerances apply when the relationship between features matters more than any single size.
ISO 2768 and h6/H7 fits explained
ISO 2768
ISO 2768 sets general tolerances for untoleranced dimensions. Part 1 covers linear and angular dimensions in four classes: fine (f), medium (m), coarse (c) and very coarse (v). Part 2 covers geometric tolerances in three classes: H, K and L. The callout goes in the title block, for example “ISO 2768-mK”, meaning medium for linear sizes and K for geometry. It then applies to every dimension without its own tolerance.
h6 vs H7
H7 and h6 come from the ISO 286 fit system. The capital letter marks a hole and the lowercase letter marks a shaft. The number is the IT grade, which sets the width of the tolerance band. Both are quoted against the nominal size.
For a 25 mm nominal size:
- H7 hole: +0.021 / 0 mm
- h6 shaft: 0 / −0.013 mm
The largest shaft (25.000) never exceeds the smallest hole (25.000). The assembly has between 0 and 0.034 mm of clearance, which is a close sliding (locational clearance) fit. The bands widen with nominal size, so the same letters give different numbers at 10 mm or 60 mm.
GD&T: the symbols you’ll meet on a drawing
In the US, geometric tolerancing follows ASME Y14.5, and ISO drawings use the equivalent ISO GPS standards. Check which edition a drawing cites: concentricity and symmetry were dropped in the 2018 edition of ASME Y14.5, and position or profile is used in their place. Machining tolerance symbols fall into five groups:
- Form: flatness, straightness, circularity, cylindricity. These control the shape of one feature.
- Orientation: perpendicularity, parallelism, angularity. These control tilt against a datum.
- Location: position, plus concentricity and symmetry on drawings made to older editions. These control where a feature sits.
- Runout: circular and total runout. These control wobble of a turned surface about an axis.
- Profile: line and surface profile. These control a contour, such as a curved face.
Each symbol sits in a frame with a tolerance value and, usually, datum letters. Use GD&T when how features relate to each other matters more than their individual sizes. A hole position held by true position from a datum scheme is a clearer instruction than a stack of ± dimensions.
Is ±0.005″ tight? What tighter tolerances cost
No. ±0.005 in (±0.13 mm) is the standard CNC tolerance. Tight starts around ±0.001 in (0.025 mm) and below. Four things drive the cost as limits close in:
- Extra operations: a feature that a lathe or mill cannot hold reliably moves to grinding or another finishing step.
- Slower cycles and more inspection: lighter cuts, extra measuring passes and more frequent gauge checks.
- Material and temperature behavior: parts move with clamping force, heat and residual stress, and some materials hold size better than others.
- Scrap risk: a narrower band rejects more parts, and that risk is priced into the quote.
The table shows how process choice moves cost. The figures are indicative values from general machining practice, not Divine Precision quotes, and the multipliers are relative to standard milling.
| Process | Typical achievable tolerance | Relative cost |
|---|---|---|
| Milling, standard | ±0.13 mm (±0.005 in) | 1× (baseline) |
| Turning, tightened | ±0.025 mm (±0.001 in) | about 2× |
| Grinding | ±0.005 mm (±0.0002 in) | about 3–5× or more |
Inspection is what makes a tolerance real. A first-article inspection on a CMM confirms the dimensions before the batch starts, and lots are then checked against the drawing, with the scope of the 100% check confirmed per drawing at quote. A first-article inspection report shows what that record contains, and the quality assurance overview explains how inspection fits the rest of production.
Surface finish limits tolerance too. A bore toleranced to a few microns cannot sit on a surface rougher than the tolerance band, so pair tight dimensions with a stated Ra value.
How to specify the right tolerance
- Start with a general tolerance in the title block, such as ISO 2768-m, so every untoleranced dimension has a defined limit.
- Tighten only functional features: fits, bearing seats, sealing surfaces and locating bores.
- Pick the datum scheme first, then apply GD&T against it.
- Pair every tight dimension with a surface finish, so the tolerance and the finish do not conflict.
- Send a STEP or IGES model with a 2D drawing carrying the GD&T, so the toleranced features are unambiguous.
Once several toleranced features sit in one assembly, their limits add up. Reading a tolerance stack before it reaches the shop floor shows how that accumulation works.
Not sure which tolerance your drawing needs? Send the file and we’ll review it for tolerance and manufacturability before you commit to a number.
FAQ
Is .005 a tight tolerance?
No. ±0.005 in (±0.13 mm) is the commonly cited standard CNC tolerance. Tight usually means ±0.001 in (0.025 mm) or less, and it costs more.
What are the four types of tolerances?
Limit, unilateral, bilateral and geometric (GD&T). The first three control size. Geometric tolerances control form, orientation, location and runout.
What is the ISO standard for machining tolerances?
ISO 2768 is the general-tolerance standard. Part 1 covers linear and angular sizes in classes f, m, c and v, and part 2 covers geometric tolerances in classes H, K and L. Fits between holes and shafts follow ISO 286.
What is h6 and H7 tolerance?
H7 is a hole tolerance and h6 is a shaft tolerance, both from the ISO 286 fit system. Paired, they give a close sliding fit. At 25 mm nominal, the hole is +0.021/0 mm and the shaft is 0/−0.013 mm.
What are standard CNC machining tolerances in mm?
About ±0.13 mm (±0.005 in) when a drawing carries no callout. Under ISO 2768-m, the general tolerance is ±0.2 mm for sizes over 6 to 30 mm.
What do the tolerance symbols on a drawing mean?
A ± sign marks a bilateral tolerance. GD&T symbols control a feature’s form, orientation, location or runout against a datum frame.
What’s the tightest tolerance CNC machining can hold?
It depends on the feature, material and process. Divine Precision lists ±0.005 mm on ground diameters and ±0.01 mm on turned diameters, confirmed per drawing at quote.
Do tighter tolerances cost more?
Yes. They add operations, inspection time and scrap risk. Apply them only to functional features and leave the rest on the general tolerance. To see how a number on your drawing affects the quote, request a quote.
