Engineering & PLMFree referencePDF, Excel, Word exportDiscrete Manufacturing

ISO 2768-1 General Tolerances Table (Classes f, m, c, v)

ISO 2768-1 gives default tolerances for linear and angular dimensions that carry no individual tolerance on the drawing. A single note, such as ISO 2768-m, then covers every untoleranced size, which keeps drawings readable and tells the shop what accuracy is expected.

Download:

Feature	Nominal size range	f (fine)	m (medium)	c (coarse)	v (very coarse)
Linear (mm)	0.5 up to 3	+/-0.05	+/-0.1	+/-0.2	-
Linear (mm)	over 3 up to 6	+/-0.05	+/-0.1	+/-0.3	+/-0.5
Linear (mm)	over 6 up to 30	+/-0.1	+/-0.2	+/-0.5	+/-1.0
Linear (mm)	over 30 up to 120	+/-0.15	+/-0.3	+/-0.8	+/-1.5
Linear (mm)	over 120 up to 400	+/-0.2	+/-0.5	+/-1.2	+/-2.5
Linear (mm)	over 400 up to 1000	+/-0.3	+/-0.8	+/-2.0	+/-4.0
Linear (mm)	over 1000 up to 2000	+/-0.5	+/-1.2	+/-3.0	+/-6.0
Linear (mm)	over 2000 up to 4000	-	+/-2.0	+/-4.0	+/-8.0
External radii and chamfer heights (mm)	0.5 up to 3	+/-0.2	+/-0.2	+/-0.4	+/-0.4
External radii and chamfer heights (mm)	over 3 up to 6	+/-0.5	+/-0.5	+/-1.0	+/-1.0
External radii and chamfer heights (mm)	over 6	+/-1.0	+/-1.0	+/-2.0	+/-2.0
Angular, by length of shorter leg (mm)	up to 10	+/-1 deg	+/-1 deg	+/-1 deg 30 min	+/-3 deg
Angular, by length of shorter leg (mm)	over 10 up to 50	+/-0 deg 30 min	+/-0 deg 30 min	+/-1 deg	+/-2 deg
Angular, by length of shorter leg (mm)	over 50 up to 120	+/-0 deg 20 min	+/-0 deg 20 min	+/-0 deg 30 min	+/-1 deg
Angular, by length of shorter leg (mm)	over 120 up to 400	+/-0 deg 10 min	+/-0 deg 10 min	+/-0 deg 15 min	+/-0 deg 30 min
Angular, by length of shorter leg (mm)	over 400	+/-0 deg 5 min	+/-0 deg 5 min	+/-0 deg 10 min	+/-0 deg 20 min

ISO 2768-1 applies to dimensions with no individual tolerance. Note it on the drawing as, for example, ISO 2768-m, or ISO 2768-mK when the geometric classes of part 2 are also invoked. Verify the values against the current standard before relying on them in a contract.

Default tolerance notes in your ERP records

Optional: we can review how drawing standards and tolerance classes are attached to your items and purchase orders.

Optional. The tool and every export work without this. No spam.

How to use the table

Pick the class named in your drawing title block, then find the row for the feature type and nominal size. A plain 50 mm milled dimension under class m is +/-0.3 mm. A 10 mm external corner radius under class m is +/-1.0 mm. Use the search box to narrow by feature. The table is for linear sizes, external radii and chamfer heights, and angles. Internal radii and chamfers follow the same limits only when you note that they are covered.

Choosing the class

Class f suits ground or precision work, m is the usual default for ordinary machined parts, c suits rough machining and fabrication, and v is for very coarse work such as flame cutting. Most shops hold medium comfortably on CNC equipment, so m is a safe default on machined parts. Use a tighter class only when the function demands it, because it increases inspection scope and cost. A looser class on a fabricated frame saves money without affecting function.

Machined housings and brackets: class m
Precision fixtures and gauges: class f, plus individual tolerances
Weldments and sheet metal frames: class c, or a separate fabrication standard

What the standard does not cover

General tolerances do not replace functional tolerances. Any dimension that affects fit, sealing or assembly should carry its own tolerance or a GD&T control. Part 2 of the standard adds default geometric tolerances for straightness, flatness, perpendicularity, symmetry and runout in classes H, K and L, which is where the K in ISO 2768-mK comes from. Also check whether your industry customer has its own default tolerance note, which then takes precedence.

Common mistakes

Common mistakes are leaving the note off entirely so no default applies, citing ISO 2768 without a class, assuming the default tolerance applies to reference or basic dimensions, and expecting the shop to hold a medium class on a 3 metre fabricated part. If a dimension in a purchase order matters for assembly, tolerance it explicitly rather than relying on the title block note.

Frequently Asked Questions

What does ISO 2768-mK mean?

It invokes medium class for linear and angular dimensions from part 1 and class K for geometric tolerances from part 2. Dimensions and features without their own tolerance then default to those limits, so the shop and inspector know the expected accuracy.

What is the ISO 2768 medium tolerance for 50 mm?

For a nominal size over 30 up to 120 mm, class m gives +/-0.3 mm. A 50 mm dimension with no stated tolerance can therefore range from 49.7 to 50.3 mm. Class f would be +/-0.15 mm and class c +/-0.8 mm.

Is ISO 2768 the same as DIN 7168?

ISO 2768 replaced the older German DIN 7168 general tolerances, and the class letters f, m, c and v correspond closely. Existing drawings that cite DIN 7168 are still seen, so check whether the values you need match the current ISO standard.

Does ISO 2768 apply to sheet metal?

It can, but most sheet metal shops work to their own capability tables or a dedicated standard because bending and forming are less accurate than machining. Class c or a specific fabrication note is more realistic than class m for formed features.

If you want default tolerance notes and drawing standards carried into your ERP purchase and quality records, we can help design the data model and checks.

Talk to an Expert Explore More Free Tools

Related Tools

Engineering & PLM

More Engineering & PLM tools

See all

Back to All Tools