Current standards for tolerances of non-tolerated linear and angular dimensions

• 1
  What non-tolerated linear and angular dimensions actually cover
• 2
  How ISO 2768 splits linear and angular limits
• 3
  Straightness, flatness and the second part of the standard
• 4
  What the machinist does with a general tolerance callout
• 5
  When a general tolerance is the wrong tool
• 6
  ISO 2768-m linear and angular limits at a glance

A machined part leaves the shop with a drawing. Most dimensions on that drawing carry an explicit tolerance, but the rest do not. Those untoleranced dimensions are not free. They fall under a general tolerance rule that the drawing invokes in its title block or notes. The phrase non-tolerated linear and angular dimensions describes exactly that body of rules: the default limits for any dimension the designer did not individually tolerance.

The idea is old and practical. Writing a tolerance on every dimension of a large weldment or a cover plate adds clutter, not control. Instead the drawing states one general tolerance class, and every untoleranced dimension inherits the limit deviation for its size band. The machinist reads the title block once and knows the target for the whole sheet.

Two families of dimensions matter here. Linear dimensions cover lengths, widths, step heights, slot depths, radii, chamfer lengths and center distances. Angular dimensions cover angles between faces, between an inclined face and a datum, and the included angle of a countersink or a dovetail. Both are handled by the same general standard, but with different size bands and different deviation values.

One boundary is worth stating up front. A general tolerance is a manufacturing default, not a design intent. If a dimension affects fit, function, sealing or assembly, it needs its own tolerance. General tolerances exist for the dimensions that genuinely do not matter much. Treating them as a substitute for real tolerance analysis is where most arguments between design and the shop start.

ISO 2768-1 covers linear and angular dimensions without individual tolerance indications. It defines four classes, usually marked as f (fine), m (medium), c (coarse) and v (very coarse). The class is written in the title block, for example 'General tolerances ISO 2768-m'. Once that line is present, every untoleranced dimension on the sheet uses the table values for class m.

The linear table is built from size bands. For class m, a dimension from 0.5 mm up to 6 mm carries ±0.1 mm. From 6 mm to 30 mm it is ±0.2 mm. From 30 mm to 120 mm it is ±0.3 mm, from 120 mm to 400 mm it is ±0.5 mm, and from 400 mm to 1,000 mm it is ±0.8 mm. Larger bands open up to ±1.2 mm and ±2 mm. The deviation grows with size because the same process holds a tighter percentage on a short feature than on a long one.

The angular table is separate and uses shorter side lengths. For class m, a side up to 10 mm carries ±1°, up to 50 mm ±0°30′, up to 120 mm ±0°20′, up to 400 mm ±0°10′, and above 400 mm ±0°5′. The logic is geometric: a small angular error multiplied by a long side becomes a large linear error, so the allowed angle tightens as the side gets longer.

Class f is roughly half the class m values and suits a shop that holds tight control anyway. Class c is about twice class m and class v is about four times, used for heavy weldments and rough castings. Choosing a class is a cost decision. A drawing marked 2768-f tells the shop to slow down on every single untoleranced feature, and that shows up in the quote.

ISO 2768-1 handles size. ISO 2768-2 handles form and position for features that carry no individual geometric tolerance. It defines three classes: H, K and L. Class H is the tightest, K is the middle, and L is the loosest. The class is written next to the general tolerance note, for example 'ISO 2768-mK'.

The 2768-2 tables cover straightness and flatness of a surface, perpendicularity of a surface, symmetry, and circular run-out. Each value scales with the nominal length of the feature. A flat surface 100 mm long under class K has a flatness allowance on the order of 0.1 mm, while the same surface under class L allows roughly twice that.

This matters on parts that bolt to another part. A housing face that is flat within 0.1 mm may rock on a mating casting, and the gap closes when the bolts are tightened. If the drawing relies on a general form tolerance, that rocking is permitted. If the designer needs a seated joint, a flatness callout with its own value is the honest way to say so.

One common gap: ISO 2768-2 does not cover cylindricity, coaxiality or position of holes in the general class. Those need explicit geometric tolerances. A hole pattern with no position tolerance is controlled only by the linear general tolerance on the center distances, which is usually far looser than the clearance the fastener needs.

The first thing we look at on a new drawing is the title block. If it says ISO 2768-mK, we build the process plan around the class m linear bands and the K form bands. A dimension of 250 mm on that sheet is a ±0.5 mm target, and there is no reason to chase ±0.05 mm on it.

The second thing we look at is which dimensions carry their own tolerance. Those are the ones that drive setup, tool choice and inspection. On a 5-axis part, a ±0.005 mm bore may need a separate finishing pass and a temperature-stable check, while the untoleranced pocket depth around it is machined to the general band in the same cycle.

Third, we check for conflict. It happens more often than people expect. A dimension can be untoleranced on the sheet and still be fully constrained by a tighter callout elsewhere, for example the position of a bore that also sets a center distance. In that case the tighter requirement wins, and the general tolerance is irrelevant.

Fourth, material behaviour enters. An aluminium 6061 bracket holds a general band easily. A long thin 316L shaft or a magnesium AZ31B housing moves after machining as internal stress releases, and an untoleranced length can drift outside the band overnight. When that risk is real, we flag it in the DFM note rather than shipping and hoping.

A general tolerance is a default, and defaults fail in predictable places. The first is any dimension that sets a fit. A bearing bore, a dowel hole, a seal groove or a shaft journal needs a real tolerance and often a fit designation. Leaving them untoleranced and trusting the general band is how assemblies end up with press fits that slip or clearance fits that bind.

The second is any dimension that stacks. If three untoleranced lengths in a chain each carry ±0.3 mm, the stack can move 0.9 mm in the worst case. That may be fine for a cover, and unacceptable for a linkage. The general tolerance does not know it is part of a stack, so the designer has to do that arithmetic.

The third is thin walls and long slender features. A 0.8 mm wall on a PEEK part deflects under cutting force, and the resulting thickness varies more than the general band allows. The same applies to a 3 mm wide fin on a heat sink or a long unsupported rib. These are process limits, not table limits.

The fourth is surface texture. The general tolerance standard says nothing about finish. An untoleranced face can be Ra 1.6–3.2 μm as machined, or Ra 0.8–1.6 μm if the drawing asks for it, or Ra 0.2–0.8 μm after fine finishing. If a sealing face needs a specific roughness, it must be called out. No general note covers it.