Engineering & PLMFree referencePDF, Excel, Word exportDiscrete Manufacturing

ISO 2768-2 General Geometrical Tolerances Table (H, K, L)

Part 2 of ISO 2768 gives default geometrical tolerances for features that carry no individual geometric control. Look up the class named in your drawing note, find the length range, and read the tolerance zone width.

Download:

Characteristic	Class	Length range (mm)	Tolerance zone (mm)
Straightness and flatness	H	up to 10	0.02
Straightness and flatness	H	over 10 up to 30	0.05
Straightness and flatness	H	over 30 up to 100	0.1
Straightness and flatness	H	over 100 up to 300	0.2
Straightness and flatness	H	over 300 up to 1000	0.3
Straightness and flatness	H	over 1000 up to 3000	0.4
Straightness and flatness	K	up to 10	0.05
Straightness and flatness	K	over 10 up to 30	0.1
Straightness and flatness	K	over 30 up to 100	0.2
Straightness and flatness	K	over 100 up to 300	0.4
Straightness and flatness	K	over 300 up to 1000	0.6
Straightness and flatness	K	over 1000 up to 3000	0.8
Straightness and flatness	L	up to 10	0.1
Straightness and flatness	L	over 10 up to 30	0.2
Straightness and flatness	L	over 30 up to 100	0.4
Straightness and flatness	L	over 100 up to 300	0.8
Straightness and flatness	L	over 300 up to 1000	1.2
Straightness and flatness	L	over 1000 up to 3000	1.6
Perpendicularity	H	up to 100	0.2
Perpendicularity	H	over 100 up to 300	0.3
Perpendicularity	H	over 300 up to 1000	0.4
Perpendicularity	H	over 1000 up to 3000	0.5
Perpendicularity	K	up to 100	0.4
Perpendicularity	K	over 100 up to 300	0.6
Perpendicularity	K	over 300 up to 1000	0.8
Perpendicularity	K	over 1000 up to 3000	1
Perpendicularity	L	up to 100	0.6
Perpendicularity	L	over 100 up to 300	1
Perpendicularity	L	over 300 up to 1000	1.5
Perpendicularity	L	over 1000 up to 3000	2
Symmetry	H	all ranges	0.5
Symmetry	K	up to 100	0.6
Symmetry	K	over 100 up to 300	0.6
Symmetry	K	over 300 up to 1000	0.8
Symmetry	K	over 1000 up to 3000	1
Symmetry	L	up to 100	0.6
Symmetry	L	over 100 up to 300	1
Symmetry	L	over 300 up to 1000	1.5
Symmetry	L	over 1000 up to 3000	2
Circular run-out	H	all ranges	0.1
Circular run-out	K	all ranges	0.2
Circular run-out	L	all ranges	0.5

Straightness and flatness use the longer side of the surface (or the length of the line element). Perpendicularity uses the shorter leg of the angle. Verify against the current edition of ISO 2768-2 before relying on a value for acceptance.

Tie drawing tolerances to ERP inspection plans

Optional: a short review of how inspection characteristics could be generated from drawing data in your ERP.

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

How to use the table

Pick the characteristic you are inspecting, then the class from the second letter of the drawing note (ISO 2768-mH uses class H). For flatness and straightness, measure the length of the longer side of the surface. For perpendicularity, use the shorter of the two features forming the angle, and treat the longer one as the datum. The value is the full width of the tolerance zone, not a plus-minus figure, so a 0.2 mm value means a 0.2 mm wide zone.

Filter by characteristic to see all three classes together
Remember that the value is a zone width, not a deviation each side
Export to Excel to attach to an inspection plan

Defaults that are easy to misread

Part 2 does not define general tolerances for profile, position, coaxiality or angularity. Coaxiality may be taken as equal to the run-out default, but only where the standard says so. The general rules also state that each geometrical tolerance applies independently, and that size limits do not by default control form unless the envelope requirement is called out on the drawing.

Worked example

A 250 mm long plate has the note ISO 2768-mK. Flatness defaults to class K in the 100 to 300 mm band, which is 0.4 mm. A 60 mm tall boss, perpendicular to the plate and sitting in the up to 100 mm band, is controlled to 0.4 mm. An inspector with a surface plate and indicator can verify both quickly. If the sealing face must be flatter, that surface needs its own flatness callout, since the default will not protect it.

Common mistakes

Teams often assume the default geometrical tolerance is tighter than the size tolerance, but a class K flatness on a short part can be looser than the size band. Others cite only part 1 and forget the second letter. When critical datums are involved, general tolerances are not a substitute for a datum reference frame, and ERP quality plans should carry explicit characteristics for anything functional.

Frequently Asked Questions

What do H, K and L mean in ISO 2768?

They are the three geometrical tolerance classes in part 2, from tightest to loosest: H, K, L. They are written as the second letter in a note such as ISO 2768-mK, where the first letter is the linear class from part 1.

Does the default flatness apply to every surface?

It applies to any surface without an individual flatness or form control, unless the drawing says otherwise. Mating or sealing faces should carry explicit callouts, because a default sized for general workshop accuracy may be too loose for function.

Is the value a plus or minus tolerance?

No. Geometrical tolerances define the width of a zone in which the feature must lie. A 0.4 mm flatness value means the whole surface must fit between two parallel planes 0.4 mm apart.

Is there a default for position or profile?

No, ISO 2768-2 does not give general values for position or profile of a surface. Where those matter, they have to be specified on the drawing with a feature control frame and a datum reference frame.

Netray can help you attach default and explicit tolerances to inspection plans in your ERP, so planners and inspectors see the same numbers as the drawing.

Talk to an Expert Explore More Free Tools

Related Tools

Engineering & PLM

More Engineering & PLM tools

See all

Back to All Tools