Machining tolerances: what to specify and what to avoid

A tolerance is a cost signal

A tolerance tells the supplier how much of the process capability to spend on a feature. A loose tolerance can be met with a standard cut and a general inspection. A tight tolerance needs a finishing pass, a stable machine, temperature control, a specific gauge and often a slower cycle.

The problem is that a drawing often carries tolerances that were copied from a previous part or added because a dimension looked important. The supplier cannot tell which calls came from a calculation and which came from caution, so the safe response is to price every call as if it were critical. The part becomes expensive without becoming better.

The reverse is worse. A feature that needs a tight tolerance but carries a general one will pass inspection and fail in assembly. The aim is a drawing where every tight call has a reason and every other dimension sits in the general tolerance.

Let the general tolerance do the work

ISO 2768-1 defines general tolerances in four classes: fine, medium, coarse and very coarse. A title block note such as ISO 2768-m applies to every dimension without an individual tolerance, so the drawing does not need a number on every line.

The class should match the process. Fine is unusual for a general note on a machined part, because it forces a level of control across every feature. Medium is a common default for machined metal. Coarse is appropriate for cast or flame-cut surfaces and for non-functional clearance.

ISO 2768-2 does the same for geometrical tolerances, with classes H, K and L for form and orientation. If the drawing has no geometric controls at all, the general class still applies when it is called in the title block. That is often enough for a bracket and not enough for a bearing seat.

Realistic bands by process

The bands below are typical for a capable shop on a rigid machine, in a temperature-controlled area, with a proven process. They are illustrative. The real limit is the supplier's measured capability, and a good supplier will say when a call is outside it.

The cost curve is not linear

Opening a tolerance is often free. Closing one is not. The first step from a general tolerance to a routine machined tolerance may cost nothing, because the process already holds it. The next step, from routine to precision, usually adds a finishing pass and a slower cycle. The step after that adds a different machine, a controlled environment or a specialist measurement.

The practical consequence is that a tolerance should be chosen at the edge of what the function needs, not at the edge of what the machine can do. A bore that only needs to clear a shaft does not need a precision fit. A bore that locates a bearing does, and the cost is justified.

There is also an inspection cost. A tolerance that needs a CMM or a custom gauge adds time to every lot, not just the first article. If the feature can be checked with a calliper, the inspection cost stays low. If it needs a gauge that has to be made, that cost lands on the programme.

Where geometric controls earn their place

A size tolerance controls a dimension, not a relationship. Two bores can each be within their diameter tolerance and still be too far apart, or not parallel, or not square to the mounting face. That is what geometric controls are for.

Use position for a hole pattern that has to assemble, with a projected zone if a long fastener passes through. Use perpendicularity for a face that seats against another. Use flatness for a sealing face. Use profile when a contoured surface has to follow a model within a band.

Keep the set small and tie it to the datums. Three or four well-chosen controls on a machined part are usually enough. A drawing covered in symbols with no datum strategy is harder to inspect than a drawing with simple dimensions, because the inspector has to guess which control dominates.

Calls to avoid

Some tolerance calls cause cost without adding control. These are the ones that come up most often in drawing reviews.

• A tight tolerance on a dimension that is not measured and not used, which adds cost and inspection time for nothing.
• A tolerance on a reference dimension, which is a contradiction and confuses the inspection plan.
• An angle tolerance in degrees on a short feature, where the linear error at the end of the feature is what matters.
• A surface finish call on a face that is painted, covered or never touched.
• A concentricity call where a position or a runout control would describe the function better and be easier to inspect.
• A stack of tolerances that adds up to more than the assembly clearance, which is a design error rather than a machining one.
• A general note such as 'machine to drawing' with no general tolerance class, which leaves every dimension undefined.

Do the stack before the drawing is released

A tolerance stack answers a simple question: if every dimension sits at its worst case, does the assembly still work? For a machined part in an assembly, the stack usually runs from a locating datum through the part to the feature that mates with the next component.

The worst-case method adds the tolerances arithmetically and gives a safe answer. The statistical method assumes a distribution and gives a tighter, more realistic answer, but it needs process data and a clear assumption about the distribution. For a small stack, worst case is usually enough and it is easier to defend.

Do the stack with the intended process in mind. A turned part holds its diameters from one centreline, so a stack along the axis is tighter than a stack across two setups. A milled part holds its hole pattern in one setup, so the pattern is tight but the relationship to a face machined later is not. The process tells you where the error lives.

A short review routine

Before release, read the drawing once as a machinist and once as an inspector. The machinist asks how many setups the part needs and which feature is hardest to reach. The inspector asks how each tight call will be measured and whether the gauge exists.

Then check three things. Every tight tolerance has a function. Every functional feature has a control that describes its relationship, not only its size. And the general tolerance class in the title block is appropriate for the process.

If a call survives all three, it belongs on the drawing. If it does not, it is a candidate for the general tolerance or for removal. That review usually takes less time than a single round of rework.