Tolerances: What They Cost and Which Ones to Specify

By CNC Machining Vietnam·Published September 21, 2026·Editorial standards

Tolerance is the dimension on a drawing that decides the price, and it is the one most often copied from a template. A part quoted with everything held tight can cost several times the same part with three critical features called out and a sensible general note. This is what those numbers actually buy.

What a tolerance is costing you

Tightening a tolerance adds cost in four separate places, which is why the effect compounds:

1. Finishing passes. Removing the last few hundredths accurately means slow, light cuts. That is machine time.
2. Tool wear management. As a cutter wears, dimensions drift. A tight tolerance means changing tools more often or compensating more frequently.
3. Inspection. Tight features have to be measured, often on a CMM, often on every piece rather than a sample.
4. Scrap and rework. A narrower band means more parts fall outside it. Somebody pays for those.

Loosen a tolerance and all four improve together. That is why it is the single highest leverage change on a drawing.

What shops hold without special effort

These are typical ranges, not promises. The shop quoting your part confirms what it holds on your geometry, in your material, at your size.

Feature	Typical comfortable band	Notes
General linear dimensions	Around plus or minus 0.1 mm	The usual general note on a machined part
Fitted features, milled	Around plus or minus 0.05 mm	Achievable routinely on most machines
Bores, reamed	Around plus or minus 0.02 mm	A standard reamer does this repeatably
Tight fitted features	Plus or minus 0.01 mm and finer	Costs more, needs temperature control and CMM verification
Flatness on a machined face	Depends on part size and section	Thin parts distort, so size matters more than the number
Surface finish, as machined	Ra 1.6 to 3.2 micrometres	Finer values need extra finishing passes

Larger parts are harder. A tolerance that is routine across 50 mm is difficult across 500 mm, because thermal expansion, fixturing and machine geometry all scale with length. Always state the tolerance against the feature rather than as a blanket rule across the whole part.

Why a blanket general note is dangerous

“All dimensions plus or minus 0.02 mm unless otherwise stated” is a common note and an expensive one. It tells the shop that every edge, every chamfer and every non functional dimension is critical.

Two things happen. The price goes up across the board. And because the shop cannot tell which features actually matter, it spreads its attention evenly, which means the features that do matter get no more care than the ones that do not.

The better pattern:

• A relaxed general note that covers everything ordinary
• A small number of explicitly toleranced features, each with the datum it is measured from
• A short note saying which of those are functionally critical

Three critical dimensions marked clearly will be held better than thirty dimensions held at the same level.

Fits, and why they communicate better than numbers

For mating features, a standard fit designation carries more information than a raw tolerance. Writing 12H7 for a bore tells the shop the nominal size, the tolerance band and, importantly, the intent: that a shaft is going in there.

The three families in ordinary use:

• Clearance fit. The parts always assemble with a gap. Used for shafts that rotate or slide, and for bolt clearance.
• Transition fit. The parts may be slightly tight or slightly loose. Used for locating features that are assembled and disassembled.
• Interference fit. The parts must be pressed or heated to assemble. Used for bearings and bushings that must not move.

If you are specifying a bore for a bearing, name the fit. A shop that sees H7 knows to ream it and knows to measure it with a bore gauge rather than callipers.

Geometric tolerance, in one paragraph

Linear tolerances control size. Geometric tolerances control form, orientation and position: flatness, perpendicularity, concentricity, true position. They matter when the relationship between features matters more than any single dimension.

The one that saves the most money in practice is true position on a hole pattern. A pattern held to true position with a bonus tolerance is easier and cheaper to hold than the same pattern controlled by tight plus or minus dimensions between every hole, and it describes what you actually need, which is that the bolts go through.

Tolerance and inspection are the same decision

A tolerance that cannot be measured is not being held, it is being hoped for. Before specifying a band, ask whether the shop has equipment that can verify it and whether you have equipment that can verify it on arrival.

If the shop’s tightest measuring capability is coarser than your tightest tolerance, the part cannot be proven even if it is correct. That mismatch is worth finding during vetting rather than during a dispute.

It also decides what to ask for in documentation. A first article inspection on the critical features is worth far more than a full report on everything.

Temperature, which nobody mentions

Metrology standards assume 20 degrees Celsius. A part measured in a workshop at 32 degrees and measured again in a cool inspection room will not give the same numbers, and aluminium moves roughly twice as much as steel for the same temperature change.

On general tolerances this is noise. At plus or minus 0.01 mm across a long dimension it is not. If your part has tolerances at that level, ask where and at what temperature the shop measures, and expect a real answer.

How to mark up a drawing before you send it

1. Go through every toleranced dimension and ask what breaks if it moves by twice as much.
2. Relax everything where the answer is nothing.
3. For the survivors, state the datum each one is measured from.
4. Replace tight linear dimensions between holes with true position where the requirement is assembly.
5. Use standard fit designations for anything that mates.
6. Set the general note at the loosest level the part tolerates.
7. Note which features you want measured and reported.

That pass typically takes an hour and is worth more than any negotiation on price. The rest of the levers are in the design changes guide.

When the drawing is marked up, send it here and up to three shops in Vietnam will quote it on what actually matters.

Frequently asked questions

Keep reading

• Writing Thread Callouts That a Machine Shop Cannot Misread
• Swiss-Type Turning: When a Small Lathe Part Needs a Sliding-Headstock Machine