What standard tolerances can I expect from a professional CNC milling parts factory?

The short answer

The default is a standard, not a number

When a drawing does not put a tolerance on a dimension, the shop still has to make a decision, and ISO 2768 is the decision. Part one of the standard covers linear and angular dimensions in four classes, fine, medium, coarse and very coarse, and part two covers straightness, flatness, perpendicularity and symmetry in classes H, K and L. The block that appears on most CNC drawings is ISO 2768-mK, medium linear tolerance with K geometric tolerance, and it represents the natural economic capability of a modern machining centre rather than a compromise.

The size dependence is the point that surprises many buyers. A medium-class tolerance is 0.1 mm on a 10 mm feature and 0.5 mm on a 300 mm feature, because the same absolute error on a long dimension is a much smaller fraction of it. That is also why demanding a blanket plus or minus 0.05 mm across a 250 mm part is expensive: it forces multiple finish passes, thermal stabilisation and full CMM verification on dimensions that may not matter at all.

Three tolerance tiers and what each costs

Above the standard classes sits a set of named machining tiers, and it is worth separating them from the ISO block because they describe what a machine and a process can hold rather than what a drawing inherits. Standard machining holds roughly 0.1 to 0.2 mm on a general feature. Precision machining, on a calibrated machine with a dedicated finishing pass, holds 0.025 to 0.05 mm and is what a bearing bore or a sealing face usually needs. Tight tolerance machining reaches 0.005 to 0.01 mm and needs thermal stabilisation, in-process touch probing and full CMM verification. Ultra precision below that is a different industry, served by diamond turning or jig grinding in a climate-controlled room.

Cost does not rise linearly across those tiers. As a rule of thumb, specifying one class tighter than the part needs adds 30 to 50 percent to the unit price, because the shop has to slow the cut, add passes and add inspection. The same logic explains the title-block contradiction that costs buyers money: a drawing that states ISO 2768-mK but also carries a note demanding plus or minus 0.05 mm on every dimension forces the tighter reading, and estimators commonly add a 30 to 45 percent buffer to the price to protect against incoming inspection. One clear general-tolerance rule and specific callouts on the features that matter is cheaper and clearer than a blanket tight number.

Geometric tolerances are a separate standard

Dimensional tolerance says how big a feature may be; geometric tolerance says how straight, flat or square it must be. ISO 2768-2 covers this with classes H, K and L, and the numbers are small: flatness for a feature under 10 mm is 0.02, 0.05 and 0.10 mm across the three classes, rising to 0.10, 0.20 and 0.40 mm for a feature from 30 to 100 mm, and perpendicularity is 0.2, 0.4 and 0.6 mm up to 100 mm of the shorter side. On a machined part the geometric callout is often the one that decides whether the part assembles, because two faces can both be within their size tolerance and still not meet.

One geometric convention is worth a note because it changes what a shop can hold without changing the function. A hole position written as plus or minus coordinates creates a square tolerance zone, while the same requirement written as a true position with a diameter creates a round one. Because the diagonal of the square is longer than its side, converting to a cylindrical zone increases the allowable area by about 57 percent, giving the machinist real margin without loosening the fit. That is a design edit that costs nothing and buys process capability.

Surface finish is quoted in Ra, and it multiplies cost

Finish and tolerance are separate requirements that are frequently confused. Surface finish is given as Ra, an average roughness in micrometres, and it is set by feed rate, tool condition and the number of passes rather than by the machine's positioning accuracy. Standard milling leaves Ra 3.2 micrometres, which suits most non-functional faces. A dedicated finishing pass reaches Ra 1.6; reaching Ra 0.8 usually needs grinding or high-speed milling with a specific tool; and Ra 0.4 needs a secondary grinding or lapping operation.

The cost lesson here is about scope. A part might need Ra 0.8 on a sealing surface and nothing better than Ra 3.2 anywhere else, and the economical route is general machining for the bulk of the part with a local finishing pass confined to the sealing area. Specifying the finer finish across every face is one of the more avoidable cost mistakes in this category, because each step down the Ra ladder requires slower cutting, more passes or a different process entirely.

What drives a shop above or below its brochure figure

• Machine positioning is the ceiling. A well-maintained three-axis vertical machining centre holds roughly 0.0127 to 0.0254 mm across its travel with repeatability near 0.005 mm; five-axis and high-speed machines do better on the same part, but only if the fixture is equally good.
• Aluminium moves three times as much as steel. Under the same cutting force an aluminium feature deflects about three times as far, and its thermal expansion coefficient, 23.1 parts per million per kelvin, is more than double that of carbon steel, so thin walls and long parts need control that a brochure figure ignores.
• Every re-clamp adds error. A part machined in three setups carries the tolerance of three fixtures, which is why five-axis work often holds a tighter feature-to-feature tolerance than the individual machine accuracy suggests.
• Inspection decides the honest number. A tolerance is only real if it is measured; ask for a first-article CMM report and confirm which features were checked, not just that the report exists.
• General tolerances do not cover fits or threads. ISO 2768 does not set a shaft fit, a thread class or a feature-specific control, so those still need an explicit callout.
• A blanket tight note is a cost, not a benefit. Tightening a non-functional dimension buys nothing and slows the cut.

How to write a drawing that gets the tolerance you need

Put one general-tolerance block in the title area, normally ISO 2768-mK, add explicit callouts only on the features whose function depends on them, mark which dimensions are functional and which are reference, and state the finish per surface rather than per part. Then send the STEP model, the drawing, the material and the annual quantity. That set lets an engineer tell you which features can be milled in one setup and which will need a controlled process. See CNC machining for the capability, surface finishing for the finishes below Ra 0.8 and aluminium die casting where a cast body plus a light machining pass is the cheaper route at volume.