How Tolerances Drive CNC Cost: The Tolerance You Do Not Need

The shape of the curve

It is tempting to think of tolerance cost as a straight line: tighten the tolerance by half and pay twice as much. That is not how it works.

The cost curve is flat at the loose end and then rises steeply. At the loose end, the tolerance is describing what the machine does anyway — a general tolerance block on a machined part costs nothing extra because the process achieves it without trying. In the middle, a comfortable tolerance adds a little care and perhaps a finishing pass. Towards the tight end, the curve turns sharply upwards, and the last increment of precision costs far more than the first.

The reason for the shape is that holding a tight tolerance requires a set of changes that each cost something, and they stack up as the tolerance tightens. A loose tolerance needs none of them. A moderate tolerance needs one or two. A tight tolerance needs all of them at once.

The tolerance tiers

Tolerance values are meaningless without a size to attach them to — ±0.01 mm on a 6 mm bore is a different proposition from ±0.01 mm on a 600 mm face — so this table is about tiers rather than absolutes.

Tier	Typical form	What it costs	What it forces
General block	ISO 2768-m on all unspecified dimensions	Nothing extra	Nothing — it is what the process naturally achieves
Comfortable	±0.1 mm on a metal part	Little	Ordinary care
Close	±0.05 mm	Moderate	A finishing pass, normal tool-wear attention
Precision	±0.01 mm	Significant	Lighter finishing cuts, slower feeds, tool-wear management, in-process measurement
Beyond precision	Tighter than ±0.01 mm	Reviewed per drawing	Rigid fixturing, temperature awareness, special tooling, higher scrap risk

Read the table as a shape rather than a set of numbers. The step from the general block to comfortable is small. The step from close to precision is large. The step beyond precision is a different conversation about the part rather than a different number on the drawing.

The same curve applies to CNC milling and CNC turning, and to every material — with the difference that harder and more abrasive grades reach the steep part of the curve sooner, because tool wear and deflection are worse to begin with. The grades we run, and how each behaves, are on the materials page.

What a tight tolerance actually forces

Six things, and all of them apply to every part in the batch.

Lighter finishing passes. To hit a tight dimension reliably, the last cut has to be small and the feed has to be controlled, which takes longer than a single decisive cut. The toolpath gets longer and the cycle time rises.

Slower feeds and speeds. Where the tolerance is near the limit, the parameters move away from maximum metal removal towards maximum control.

Tool-wear management. A worn cutter produces a different dimension from a fresh one. Where the tolerance is tight, the tool has to be changed more often, or the offset has to be adjusted between parts — which is time that does not appear in the cutting cycle.

More rigid fixturing. Deflection is proportional to cutting force and inversely related to rigidity. Holding a tight tolerance means reducing deflection, which means better workholding, sometimes a tailstock or a steady, and sometimes a different operation sequence.

Thermal awareness. Metal moves with temperature, and a tight tolerance is small enough that the part warming up during cutting can matter. On the tightest work the part is allowed to stabilise before the final measurement, and on some parts the temperature of the shop itself is part of the plan.

Measurement and scrap. A tight tolerance requires measuring, and measuring takes time. It also means that parts which miss the band are scrapped rather than reworked, which is a real cost that shows up across the batch rather than on the individual part.

Stack those six together and the steep part of the curve stops being surprising. None of them is dramatic on its own; together they change the whole character of the job. They are also the reason tolerance sits near the top of the list of cost drivers on a machined part — the full picture is set out in what actually drives the cost of a machined part.

Tolerance and geometry have to be read together

This is the part of the subject that a tolerance table cannot express, and it is where most of the practical judgement lives.

The same tolerance value can be easy or hard depending on the feature it sits on.

Feature	Same tolerance is…	Why
Short, thick, well-supported section	Easy	Rigid; little deflection; easy to reach
Thin wall	Difficult	Deflects under the cutter; may need lighter passes or support
Deep bore	Difficult	Long slender tool; deflection and taper; chip evacuation
Feature far from the datum	Difficult	Errors accumulate over the distance
Small hole	Difficult	Small tool, low rigidity, limited access
Large flat face	Difficult if flatness matters	Distortion from clamping and from material removal
External diameter on a turned part	Comparatively easy	Turning holds diameter naturally

A drawing that carries ±0.01 mm on a rigid external diameter and ±0.01 mm on a thin-wall internal feature is asking for two very different things, and they look identical on paper. The shop can see the difference; the drawing does not state it.

Distance from the datum compounds this. Every source of error — thermal expansion, machine geometry, setup error, tool deflection — scales with how far the feature is from the reference. A tolerance that is comfortable near the datum can be genuinely difficult at the far end of a long component. Where a tight tolerance sits far from its datum, saying so explicitly helps the shop plan the sequence to suit it.

The over-tolerancing problem

Most drawings do not have too few tolerances. They have too many tight ones, and they usually got there in one of four ways.

Copied from a previous drawing. A tolerance that was needed on one part is carried onto the next one, where the requirement may not exist.

Applied as a blanket. A note that says everything is ±0.02 mm, because it seemed tidy. Each of those is a per-part cost, and most of them are controlling nothing.

Tightened to be safe. A designer who is unsure whether a tolerance matters often tightens it, on the reasoning that tighter cannot hurt. It can: it is a permanent per-part cost in exchange for a requirement the function may not have.

Left over from a different process. A tolerance that was appropriate for a grinding operation may be unnecessary on a part that is milled, and one that was appropriate for a prototype may be excessive for production.

The antidote is a single question asked of each tight tolerance: what does this feature do? If the answer involves a fit, a seal, a location or an alignment, the tolerance is doing work. If the answer is that it does not mate with anything, or that it is a clearance hole, or that it is a surface nobody measures, the tolerance is costing money for nothing.

Tolerance should follow fit, not habit

The features that genuinely need tight tolerances form a short and predictable list:

• Bearing seats and bores where a bearing has to fit with a defined interference or clearance
• Spigots and mating diameters where two parts locate on each other
• Sealing faces and O-ring grooves where a seal has to work
• Locating pins, dowel holes and datum features that position other components
• Gear and spline features where the mesh depends on it
• Threads with a defined class, where the fit of the fastener depends on the pitch diameter
• Fits with a specified clearance or interference stated on the drawing

And the features that almost never need one:

• Clearance holes for fasteners
• Cosmetic faces and non-mating surfaces
• Internal cavities and pockets that hold nothing
• Undimensioned features left to the general block
• Any dimension whose function is simply “the part is this big”

The practical instruction that separates these two lists is to state which features are functional — and the numbers that go with them — and leave the rest to the general block. That single habit is worth more than any negotiation on the quotation, because it acts on every part in the batch rather than once.

Stack-up, and why tightening one dimension can be the wrong move

Where several toleranced dimensions contribute to the same assembly outcome, their tolerances accumulate. Five dimensions at ±0.05 mm produce a stack that can be several times that, and the assembly can fail even though every part is in tolerance.

The usual response is to tighten something, and the usual choice is the dimension the designer is most worried about. That is often the wrong one, for two reasons:

• Tightening a middle dimension in a stack reduces the total by its own contribution only, which may not be enough to fix the assembly.
• Loosening the dimensions that do not matter may free enough cost to tighten the one that does — or may solve the problem outright, because the tolerance was never the binding constraint.

The productive sequence is to identify which dimensions actually drive the fit, decide the total tolerance the assembly needs, and then allocate it across those dimensions rather than inheriting whatever each one happened to carry. That is an assembly-level calculation rather than a part-level one, and it belongs on the enquiry where the whole assembly is visible.

A geometric tolerance can be cheaper than a tight one

There is a route that often achieves the requirement for less money: describe what actually matters geometrically rather than controlling it indirectly through size.

A hole pattern controlled by tight positional dimensions forces each hole to be in the right place. The same pattern controlled by a position tolerance states the requirement directly and can allow the shop more freedom — and where the callout is at maximum material condition, a hole at the larger end of its size tolerance can be allowed additional positional tolerance, because the clearance it provides has grown.

The same principle applies to flatness, perpendicularity and concentricity. A face that has to seal needs a flatness callout, not necessarily a tight thickness. A bore that has to be perpendicular to a face needs a perpendicularity callout, not necessarily a tight length. In each case the geometric callout expresses the function, and the size tolerance is freed to be whatever the process achieves naturally.

This is not an argument for adding geometric tolerances everywhere — a callout that is not needed is a cost like any other. It is an argument for saying what the feature has to do, and letting the shop choose the least expensive way to control it. The drawing conventions and accepted formats are set out on the drawing requirements page.

What to put on the drawing

Instead of	Write
Blanket tolerance on everything	General block, plus tolerances only on the functional features
±0.01 mm on every dimension	±0.01 mm on the fits and locations; general block elsewhere
Tight tolerance, no context	Tight tolerance plus what the feature does — seat, seal, locate, align
Tight tolerance far from the datum	Say where the datum is and which features must relate to it
Tight size on a pattern	Consider a position tolerance, which may allow more freedom
Every dimension toleranced	State which features are functional and leave the rest

The single most valuable line on a drawing with tight tolerances is the one that says what those features are for. A shop that knows a bore is a bearing seat will plan the sequence, the tooling and the fixturing around holding it. A shop that sees a tight number on an unexplained feature will hold it, charge for it, and never know whether it needed holding.

Precision features are held to ±0.01 mm with ISO 2768-m as the general block, and anything tighter is reviewed against the drawing — see tolerances we hold. Send the drawing with the functional features identified and the quantity, and the quote comes back within 24 hours with DFM feedback, including a note where a tolerance is driving cost without controlling anything. Orders start at 50 pieces per style and material, samples from a single piece in 5–10 days, and every batch ships with a material certificate (MTR) tracing the grade to its mill heat plus pre-shipment photos.