Tolerances and surface finish: how to specify a machined part correctly

Tolerances and surface finish: well specifying a part means finding the right balance between the intended function and what the manufacturing process can realistically achieve. An overly tight tolerance or an unnecessarily fine surface finish drives costs up in a non-linear way; a specification that is too loose leads to assembly failures and scrap. This guide covers dimensional tolerances, geometric tolerances, and surface finish, linking each concept to common machining processes and reference standards.

Why part specification determines manufacturability

A definition drawing communicates two fundamental pieces of information to the shop floor: the nominal geometry and the permissible deviations. If those deviations are not clearly expressed, every party involved — design engineering, process engineering, the operator — may interpret them differently. The result: non-conformances, costly scrap, and extended lead times.

Specification also has a direct bearing on the choice of production method. A part where every dimension carries an IT6 tolerance (a very tight tolerance band under ISO 286-1) will often require an additional finishing operation — grinding or honing — where an IT9 tolerance could have been met straight off the lathe or milling machine. Understanding the link between specification and process means designing parts that are both functional and economically viable to produce.

Dimensional tolerances: ISO grades, tolerance bands, and fits

Standard ISO 286-1 defines a system of fits and tolerances for cylindrical features (shafts and bores) and, by extension, for linear dimensions. Two concepts are inseparable:

• The tolerance grade (IT) — from IT01 (extreme precision) to IT18 (wide latitude) — sets the width of the permissible band for a given dimension. An IT6 on a 50 mm diameter corresponds to a band of around ten micrometers; an IT9 on that same diameter is approximately four times wider.
• The tolerance position (lowercase letters for shafts, uppercase for bores) determines whether the band results in clearance, interference, or uncertainty relative to the nominal size. An H7/g6 fit designates an H7 bore and a g6 shaft, producing the functional clearance typical of sliding guides.

For non-cylindrical parts or general dimensions, it is common practice to specify a general tolerance per ISO 2768 (grades f, m, c, v), avoiding the need to annotate every dimension. Functional dimensions, however — those governing an assembly or a critical clearance — must always be specified individually.

A practical example: a spindle shaft must fit into its bearing housing. The functional dimensioning requires the shaft diameter to be explicitly stated with its fit (e.g., ⌀40 h6), rather than relying on a general tolerance that would leave too much latitude.

Geometric tolerances: form, orientation, location, and runout

A part can meet its nominal dimensions and still be unusable if its geometry is defective. Geometric tolerances (or GD&T, Geometric Dimensioning & Tolerancing) — standardized under ISO 1101 — complement dimensional tolerances by controlling the form, orientation, and location of geometric features.

Four families are distinguished:

• Form: straightness, flatness, circularity, cylindricity. These tolerances require no datum; they characterize a feature in its own right.
• Orientation: parallelism, perpendicularity, angularity. These are always expressed relative to a datum.
• Location: position, coaxiality, symmetry. These control the situation of a feature relative to one or more datums.
• Runout: circular runout and total runout. Particularly useful for rotating parts, they combine form and location.

On the drawing, each geometric tolerance is read from a rectangular feature control frame divided into compartments: characteristic symbol, tolerance value, datum reference(s). A flat mounting surface specified with a flatness of 0.02 mm means that all points on that surface must lie between two parallel planes 0.02 mm apart. If the frame is incomplete — a missing datum reference on an orientation tolerance, a datum not physically established on the part — the operator has no physical anchor from which to measure conformance.

Surface finish and roughness: Ra, Rz, and drawing symbols

Surface finish describes the geometric texture of a surface after machining. Two parameters are commonly specified:

• Ra (arithmetical mean roughness): the average value of the deviations of the real profile from the mean line, over an evaluation length. This is the most universally used parameter.
• Rz (mean height of the five largest irregularities): more sensitive to isolated peaks and valleys; relevant for surfaces subject to fatigue loading or sealing requirements.

Standard ISO 1302 governs the indication of surface finish on technical drawings. The basic symbol is a triangle supplemented with additional indications: Ra (or Rz) value, lay direction, and process if required. An Ra value of 1.6 µm shown in the triangle means that the roughness must not exceed 1.6 µm.

On a drawing, when the same roughness applies to the majority of surfaces, it is noted in the title block (with the qualifier "unless otherwise specified") to keep the drawing uncluttered.

Reading and writing a definition drawing that conforms to standards

A complete definition drawing includes:

1. The views and sections needed for an unambiguous definition of the geometry.
2. Dimensional tolerancing with fits or general tolerances.
3. Feature control frames with their datum references.
4. Surface finish symbols per ISO 1302.
5. The title block (material, surface treatment, applicable standard, revision level).

Two drafting errors occur frequently. The first: placing a perpendicularity tolerance without defining a datum — the operator does not know which surface to measure from. The second: applying a fine roughness (Ra 0.8 µm) uniformly to all surfaces of a part, without distinguishing functional from non-functional areas, needlessly multiplying finishing passes.

To standardize the approach between the design office and the shop floor, it is useful to build a library of standard blocks (common fits, recurring surface finish symbols) and to train both parties to read ISO 1101 in the same way. That is often where the real source of interpretation discrepancies lies.

Choosing the right tolerance level for the machining process

Each process has a tolerance and roughness range achievable under normal production conditions. Specifying outside that range forces the shop to resort to additional operations — or to reject parts as non-conforming. The following table gives representative order-of-magnitude values:

Two important observations follow from this table.

First, the economic impact is non-linear. Moving from IT9 to IT7 often means an additional pass or tighter setup; moving from IT7 to IT5 may require switching to a different process entirely (grinding after turning), with the associated logistical cost. Equally, a surface finish of Ra 0.8 µm demands cutting conditions and tooling that are fundamentally different from those for Ra 3.2 µm.

Second, process capability (Cp, Cpk indices) must be taken into account. An IT6 grade is achievable by grinding, but the process must show sufficient capability for parts produced in series to remain within the tolerance band. Specifying a tolerance whose band is narrower than the natural variation of the process will inevitably lead to scrap.

Precision engineering shops — some located in established industrial areas with strong machining traditions — have mastered fine finishing processes (grinding, honing) that allow tight grades to be achieved in series production. Engaging with the subcontractor early in the design phase makes it possible to align specifications with the equipment actually available.

Common specification errors and their consequences on the shop floor

Several errors recur systematically when auditing definition drawings:

Over-specifying as a precaution

Applying a tight tolerance or a fine surface finish "to be safe" is a common but costly practice. It extends cycle times, ties up more expensive resources, and — if the process capability is not sufficient — generates scrap. The rule is to specify at the level that is just necessary for the function.

Under-specifying functional surfaces

The opposite error is leaving a general tolerance on a surface that governs a critical assembly: a bearing seat, a sealing land, a guide contact surface. The result is an assembly failure discovered after delivery.

Omitting geometric datum references

A feature control frame without a datum on an orientation or location tolerance is unusable for inspection. The operator will measure as best they can, and results will be inconsistent from one inspection to the next.

Mixing standards systems

Some drawings mix ISO notation with ASME Y14.5 notation (the American GD&T standard). The symbols are similar but not identical, and the interpretation rules differ. One system must be chosen and adhered to throughout, with the choice stated in the title block.

Overlooking surface treatments

Heat treatment, a coating (hard chrome, nitriding) or anodizing all modify final dimensions. If the tolerance is specified before treatment, the part may be out of tolerance afterward. It must be explicitly stated whether dimensions apply before or after treatment.