What tolerance does a dimension carry when the drawing gives it none? Enter the nominal size, the feature type and the class from the title block (for example ISO 2768-mK). You get the permissible deviation and the limits, how the other classes compare at that size, the geometric tolerances for class H, K or L, and the loosest class that would meet a tolerance you need.
Engineering estimate, not a quote. Always check the edition of the standard named on your drawing; an individual tolerance on the drawing overrides the general one.
A drawing cannot sensibly put a tolerance on every dimension, so most drawings carry a general tolerance note in the title block, such as "ISO 2768-mK". That note gives every dimension and feature without its own tolerance a default one, taken from two tables. ISO 2768-1 covers sizes: linear dimensions, external radii and chamfer heights (called broken edges), and angles. ISO 2768-2 covers geometry: straightness, flatness, perpendicularity, symmetry and circular run-out. The first letter of the callout picks the size class and the second letter picks the geometry class.
Step 1: find the size range. The tables group nominal sizes into ranges written as "over A up to B", so a boundary value belongs to the lower range: 30 mm is in "over 6 up to 30", not in "over 30 up to 120". Below 0.5 mm the standard gives no general tolerance; the deviation must be written on the drawing. The tables are in millimetres, so an inch dimension is converted first (× 25.4).
Step 2: read the deviation for the class. Linear and broken-edge deviations are symmetric (±). Some cells are empty: class v has no value up to 3 mm and class f has none over 2000 mm, because those combinations are not sensible. An empty cell means the dimension needs an explicit tolerance.
Step 3: apply it. The limits are the nominal minus and plus the deviation, and the total band is twice the deviation.
Angles are different. The angular deviation depends on the length of the shorter side of the angle, because a short side cannot be measured or held to the same angle as a long one. The deviation is in degrees and minutes. To see what it means on the part, multiply the side length by the tangent of the deviation: that is how far the end of the side may sit from its nominal position.
Geometry. ISO 2768-2 values for straightness and flatness depend on the length of the line or surface; perpendicularity uses the shorter of the two features; symmetry uses the longer feature; circular run-out is a single value per class. These are the zones that apply when the drawing shows no geometric tolerance on that feature.
| Class | 0.5–3 | >3–6 | >6–30 | >30–120 | >120–400 | >400–1000 | >1000–2000 | >2000–4000 |
|---|---|---|---|---|---|---|---|---|
| f fine | ±0.05 | ±0.05 | ±0.1 | ±0.15 | ±0.2 | ±0.3 | ±0.5 | – |
| m medium | ±0.1 | ±0.1 | ±0.2 | ±0.3 | ±0.5 | ±0.8 | ±1.2 | ±2 |
| c coarse | ±0.2 | ±0.3 | ±0.5 | ±0.8 | ±1.2 | ±2 | ±3 | ±4 |
| v very coarse | – | ±0.5 | ±1 | ±1.5 | ±2.5 | ±4 | ±6 | ±8 |
| Class | Edge 0.5–3 | Edge >3–6 | Edge >6 | Angle, shorter side ≤10 | >10–50 | >50–120 | >120–400 | >400 |
|---|---|---|---|---|---|---|---|---|
| f fine | ±0.2 | ±0.5 | ±1 | ±1° | ±0°30′ | ±0°20′ | ±0°10′ | ±0°5′ |
| m medium | ±0.2 | ±0.5 | ±1 | ±1° | ±0°30′ | ±0°20′ | ±0°10′ | ±0°5′ |
| c coarse | ±0.4 | ±1 | ±2 | ±1°30′ | ±1° | ±0°30′ | ±0°15′ | ±0°10′ |
| v very coarse | ±0.4 | ±1 | ±2 | ±3° | ±2° | ±1° | ±0°30′ | ±0°20′ |
| Tolerance | Length range | H | K | L |
|---|---|---|---|---|
| Straightness and flatness | ≤10 | 0.02 | 0.05 | 0.1 |
| >10–30 | 0.05 | 0.1 | 0.2 | |
| >30–100 | 0.1 | 0.2 | 0.4 | |
| >100–300 | 0.2 | 0.4 | 0.8 | |
| >300–1000 | 0.3 | 0.6 | 1.2 | |
| >1000–3000 | 0.4 | 0.8 | 1.6 | |
| Perpendicularity (shorter side) | ≤100 | 0.2 | 0.4 | 0.6 |
| >100–300 | 0.3 | 0.6 | 1 | |
| >300–1000 | 0.4 | 0.8 | 1.5 | |
| >1000–3000 | 0.5 | 1 | 2 | |
| Symmetry (longer feature) | ≤100 | 0.5 | 0.6 | 0.6 |
| >100–300 | 0.5 | 0.6 | 1 | |
| >300–1000 | 0.5 | 0.8 | 1.5 | |
| >1000–3000 | 0.5 | 1 | 2 | |
| Circular run-out | any | 0.1 | 0.2 | 0.5 |
A machined aluminium L-bracket is drawn with "Untoleranced dimensions: ISO 2768-mK" in the title block. The base is 85 mm long, the upright is 40 mm tall, the corner is a 90° angle, and the end of the base has a 2 mm chamfer. None of these has its own tolerance. One feature, the 85 mm length, has to locate in a slot and the designer wants to know whether ±0.2 mm is covered.
Two results are worth noticing. First, the medium class gives the 85 mm length ±0.3 mm, so a designer who assumed "general tolerance is about ±0.1" would be wrong by a factor of three at this size; the deviation grows with size. Second, the 90° corner looks loose at ±30′, and on a 40 mm leg it is: ±0.35 mm at the tip, a band 0.70 mm wide. Do not compare that with "0.4" as if it were ±0.4. An ISO 2768-2 perpendicularity value is the full width of the zone (two parallel planes 0.4 mm apart, roughly ±0.2 mm), so on this corner the class K perpendicularity is the tighter of the two controls and is the one an inspector will usually find binding. The angular table matters most for angles other than 90°, where no general perpendicularity applies. Switching the whole drawing to class f to rescue one dimension would tighten every other feature too; the right fix is an explicit tolerance on the 85 mm length. Press Load the worked example to reproduce the length, geometry and class-recommender lines, then switch the feature type to see the chamfer and the angle.
The general tolerance exists so that the drawing only has to talk about what matters. The trick is deciding what matters. A feature that locates, seals, fits or carries a datum should almost never be left to the general note: the stack-up that proves the assembly works needs a known tolerance, and ISO 2768-1 itself says a part outside the general tolerance need not be rejected if it still functions, which is not the protection you want on a critical feature. Everything else, from cosmetic edges to clearance holes with plenty of room, is what the general note is for.
ISO 2768-1 states its own scope: parts produced by metal removal and parts formed from sheet metal. It is common to see "ISO 2768-m" on an injection molded part drawing anyway, usually copied from a machined-part template, and it causes two opposite problems. On small molded features the medium class can be tighter than the process holds once shrinkage variation is added, especially on dimensions across the parting line or affected by a slide. On large flat molded parts, ISO 2768-2 flatness values such as 0.4 mm over 100–300 mm (class K) are often unrealistic in any resin prone to warp. Molded plastics have their own standard, ISO 20457, which sets tolerance groups by resin family and by whether a dimension is fixed by a single mold half or crosses the parting line, and many molders work from the SPI/PIA commercial and fine tables. Castings use ISO 8062-3 casting tolerance grades. For 3D printed prototypes, the general note is a reasonable reference for a machined-equivalent part but says nothing about what a given printer holds. If a drawing for a formed part does use ISO 2768, review each untoleranced feature against what the process can hold before the tool is cut.
| Method | Use it when | Limit |
|---|---|---|
| ISO 2768-1 / -2 general tolerances (this page) | Non-critical features of machined or sheet metal parts on drawings that call ISO 2768 | Not for functional features; scope excludes molded and cast parts |
| Explicit ± tolerance or ISO 286 fit | Features that fit, locate or seal; shafts and holes (e.g. H7/g6) | Must be sized from function, usually by a stack-up |
| GD&T per ASME Y14.5 or ISO 1101 | Position, profile and orientation of functional features relative to datums | Needs a datum scheme and trained inspection |
| ISO 20457 or SPI/PIA tables | Injection molded plastic parts | Values depend on resin and on whether the dimension crosses the parting line |
| ISO 8062-3 casting grades | Sand, die and investment castings | Grade depends on casting process and size |
| Title-block block tolerances (e.g. X.X ±0.1, X.XX ±0.05) | Older and inch drawings that tie tolerance to decimal places | Not size-dependent; easily misread when CAD exports extra decimals |
Deviation values are from ISO 2768-1:1989, General tolerances, Part 1: Tolerances for linear and angular dimensions without individual tolerance indications, tables 1 (linear dimensions), 2 (external radii and chamfer heights) and 3 (angular dimensions), and ISO 2768-2:1989, General tolerances, Part 2: Geometrical tolerances for features without individual tolerance indications, tables for straightness and flatness, perpendicularity, symmetry and circular run-out. The rule that a part outside the general tolerance is not automatically rejected if function is unimpaired is from ISO 2768-1. ISO 20457 (molded plastic parts), ISO 8062-3 (castings) and ISO 22081 (general geometrical specifications) are named for scope only. The linear equivalent of an angular deviation, L·tan(Δθ), and the class recommender are this page's own calculations, not part of the standard.
An 85 mm linear dimension falls in the ISO 2768-1 range over 30 up to 120 mm. The permissible deviation is ±0.15 mm for class f (fine), ±0.3 mm for class m (medium), ±0.8 mm for class c (coarse) and ±1.5 mm for class v (very coarse). On a drawing marked ISO 2768-mK, an untoleranced 85 mm dimension may therefore measure anywhere from 84.7 to 85.3 mm, a total band of 0.6 mm.
ISO 2768-mK in the title block means that every dimension and feature without its own tolerance takes the general tolerances of ISO 2768-1 class m (medium) for linear and angular dimensions and ISO 2768-2 class K for geometrical tolerances such as straightness, flatness, perpendicularity, symmetry and circular run-out. The first letter (f, m, c or v) is the size class from part 1; the second letter (H, K or L) is the geometry class from part 2. An added E, as in ISO 2768-mK-E, applies the envelope requirement to all single features of size.
ISO 2768-1 gives ± deviations by nominal size range in millimetres. 0.5 to 3: f 0.05, m 0.1, c 0.2, v not specified. Over 3 to 6: f 0.05, m 0.1, c 0.3, v 0.5. Over 6 to 30: f 0.1, m 0.2, c 0.5, v 1. Over 30 to 120: f 0.15, m 0.3, c 0.8, v 1.5. Over 120 to 400: f 0.2, m 0.5, c 1.2, v 2.5. Over 400 to 1000: f 0.3, m 0.8, c 2, v 4. Over 1000 to 2000: f 0.5, m 1.2, c 3, v 6. Over 2000 to 4000: f not specified, m 2, c 4, v 8. Below 0.5 mm the deviation must be written next to the dimension.
ISO 2768-1 angular tolerances depend on the length of the shorter side of the angle, not on the angle itself. For class m (and f) the deviation is ±1° up to 10 mm, ±30′ over 10 to 50 mm, ±20′ over 50 to 120 mm, ±10′ over 120 to 400 mm and ±5′ over 400 mm. Class c is 1°30′, 1°, 30′, 15′ and 10′; class v is 3°, 2°, 1°, 30′ and 20′. A 90° corner with a 40 mm shorter side in class m is 90° ± 30′, which moves the end of that side by 40 × tan(0.5°) = 0.35 mm.
ISO 2768-1 has a separate table for broken edges: external radii and chamfer heights. For classes f and m the deviation is ±0.2 mm for 0.5 to 3 mm, ±0.5 mm over 3 to 6 mm and ±1 mm over 6 mm. For classes c and v it is ±0.4, ±1 and ±2 mm. A 2 mm chamfer on an ISO 2768-m drawing may therefore be 1.8 to 2.2 mm.
ISO 2768-1 is written for parts made by metal removal and parts formed from sheet metal. It is often seen on plastic part drawings, but it does not reflect how molded dimensions behave: shrinkage, wall thickness, resin and whether the dimension crosses the parting line all change what is achievable. For molded plastics, ISO 20457 (which replaced DIN 16742) gives tolerance groups by resin and dimension type, and the SPI/PIA commercial and fine tables are common in practice. For castings, ISO 8062-3 applies. Apply ISO 2768 to molded parts only after checking each value against what the process can hold.
Not automatically. ISO 2768-1 states that general tolerances describe customary workshop accuracy and that a workpiece exceeding them should not lead to automatic rejection if its ability to function is not impaired. That is a reason to put an explicit tolerance on every dimension that matters to fit or function: a general tolerance is a default for non-critical features, not a guarantee for critical ones.
Class m (medium) is the usual default for machined and fabricated metal parts and is within normal machine-shop capability. Class f (fine) roughly halves the deviations and is used for precision machined parts where most features matter. Class c (coarse) suits rough machining, weldments and large fabrications, and class v (very coarse) suits heavy fabrication and flame-cut work. Choose the loosest class that every non-critical feature can accept, then tolerance the critical features individually rather than tightening the whole drawing.
Not sure which general tolerance class belongs on your drawing, or whether a molded or cast part can hold it? Ask our AI assistant. It answers from this website, and our engineering team follows up if you want.
AI assistant. Answers can be wrong; nothing it says is a quote or a promise.
This lookup gives an engineering estimate. Our engineering team reviews drawings for which features need explicit tolerances, which general class suits the process, and where a molded or cast part needs its own tolerance standard, while each change is still a drawing edit and not a tool modification.
Book a 30-min call Send a drawing or sample