What Tolerance Should You Specify on CNC Machined Parts — and What Does Tighter Tolerance Cost?

Flat illustration of a CNC machined metal bracket with a caliper measuring a bore and a drawing showing a tolerance callout.

Your drawing is ready, the model is finished, and now you have to decide what tolerance to put on each dimension. Put the tightest number everywhere and the quote comes back high — or the supplier quietly prices the risk in. Put a loose number on a sealing face and the parts do not fit.

For most features, use the ISO 2768 general tolerance in the title block and call out tighter limits only where fit, function, sealing, or alignment actually demands it. Every step tighter than the default adds process control and inspection — slower feeds, more setups, more measurement — so precision should be spent where the part earns it back.

This guide shows which default applies, when to tighten it, what tightening costs, and how to write the callout so a supplier can actually check it.

What a tolerance actually promises

A tolerance is not a promise that a dimension will be exact. It is the range of variation you accept — the amount a feature may differ from nominal and still work. Three distinctions decide how it is read:

  • Bilateral vs unilateral. A bilateral tolerance such as ±0.05 mm allows variation in both directions. A unilateral tolerance such as +0.00/−0.10 mm allows it in one direction only — useful for a bore that must never be undersize, or a shaft that must never be oversize.
  • General vs specific. A general tolerance in the title block (for example "ISO 2768-m") covers every dimension that has no tolerance of its own. A specific tolerance written next to one dimension overrides the general rule for that dimension only.
  • Size vs geometry. A size tolerance controls how big a feature is. A geometric tolerance (flatness, perpendicularity, position, runout) controls its shape and its relationship to other features — and a part can pass every size tolerance and still fail to assemble if the geometry is wrong.

A tolerance that cannot be measured is not a specification; it is a wish. Before writing any number, ask what instrument will check it — caliper, micrometer, pin gauge, thread gauge, or CMM — and whether the supplier has it. Our CNC machining guide covers the processes, materials, and cost drivers behind these choices; this article is the tolerance decision itself.

The ISO 2768-1 defaults: what applies when you write nothing

ISO 2768-1 defines default tolerances for linear and angular dimensions that have no tolerance of their own. It uses four classes — f (fine), m (medium), c (coarse), v (very coarse) — and you apply one by writing it in the title block, for example "ISO 2768-m". For most engineering work, the default is enough, and it saves documentation time and machining cost.

The table below shows the published defaults used by Protolabs Network for CNC machined parts — metals to ISO 2768-f (fine) and plastics to ISO 2768-m (medium) unless the drawing says otherwise. These are reference values from a published service standard, not Cavity Mold capability claims; confirm your own supplier’s defaults at quote. See the Hubs / Protolabs Network ISO 2768-1 guide.

Nominal size rangePlastics (ISO 2768-m)Metals (ISO 2768-f)
0.5 mm to 3 mm±0.1 mm±0.05 mm
Over 3 mm to 6 mm±0.1 mm±0.05 mm
Over 6 mm to 30 mm±0.2 mm±0.1 mm
Over 30 mm to 120 mm±0.3 mm±0.15 mm
Over 120 mm to 400 mm±0.5 mm±0.2 mm
Over 400 mm to 1,000 mm±0.8 mm±0.3 mm
Over 1,000 mm to 2,000 mm±1.2 mm±0.5 mm
Over 2,000 mm to 4,000 mm±2 mm—

Two things to notice. First, the tolerance grows with the size of the feature — a 300 mm length cannot be held to the same ±0.05 mm as a 3 mm bore, and a drawing that asks for it will be priced accordingly. Second, plastics get the looser class by default, because they are more sensitive to heat, moisture, and fixturing stress and can warp or creep after machining. If you need precision in a plastic part, choose a stable grade such as polycarbonate and specify the tolerance only where it matters.

If a dimension falls below 0.5 mm, no default applies — write the tolerance on the drawing explicitly.

When the default is not enough

Defaults cover most features. Call out a tighter, specific tolerance only when the function depends on it:

FeatureWhat to specifyHow it is checked
Press, slip, or interference fitsThe fit class or the explicit bilateral tolerance on both mating partsPin or plug gauges, micrometer, bore measurement
Sealing faces and boresTighter size tolerance plus a flatness or surface-finish requirementCMM or surface plate with indicator; roughness measurement
Bearing seats and shaftsExplicit diameter tolerance, plus roundness or cylindricity if rotation mattersMicrometer and roundness measurement; CMM
Alignment-critical featuresPosition or perpendicularity (GD&T) against a stated datum, not just tighter size tolerancesCMM against the datum reference frame
Mating to off-the-shelf partsThe tolerance the bought component’s data sheet requiresThe bought part’s own gauge or specification
ThreadsThe thread callout itself (for example M6 × 1, 6H/6g) — threads follow their own ISO standards, not ISO 2768Thread plug or ring gauges

The common mistake is to tighten every dimension instead of the one that matters. A bracket with twenty dimensions at ±0.01 mm costs far more than the same bracket with one bearing bore at ±0.01 mm and the rest at the ISO default — and the two brackets assemble identically. Use GD&T (geometric dimensioning and tolerancing) when the relationship between features matters more than the size of any one of them: a position tolerance on a bolt-hole pattern against a datum says more about assembly than a tight tolerance on each hole’s diameter.

What tighter tolerance costs

There is no general multiplier for the cost of precision — no verified source gives one, and any percentage quoted as a rule would be invented. What can be said, and what suppliers confirm, is where the cost comes from:

  • More process control. Tighter features need more careful setups, slower feeds, lighter cuts, and sometimes a second operation on a different machine. A bore that must hold ±0.01 mm is not the same job as a bore at ±0.1 mm.
  • More inspection. Each tight dimension is a measurement: a CMM program, a gauge, a first-article report, and the time to run it. Geometric tolerances down to about ±0.010 mm are achievable in CNC work, but only when they are clearly called out on the drawing and confirmed at quote — they are never free.
  • More scrap risk. The tighter the window, the more parts fall outside it. That risk is priced into the quote, or it appears later as rejected parts and rework.
  • Material and geometry limits. Thin walls, deep pockets, long tool reach, and large flat surfaces all fight tight tolerances. Plastics add heat and moisture movement on top. A tolerance that ignores the geometry is a tolerance the shop will either refuse or price defensively.

As a reference point for what "standard" means in CNC machining, Protolabs states a standard tolerance of ±0.005 in. (0.13 mm) for its machined parts and accepts GD&T tolerancing for deeper control. See Protolabs’ Definitive Guide to CNC Machining. Your supplier’s standard will differ — ask for it before you write the drawing, not after the quote arrives.

Milling or turning for tolerance-critical features

The process matters as much as the number. Milling and turning hold different kinds of accuracy best:

MillingTurning
Best forComplex geometry, pockets, slots, multi-face featuresCylindrical parts, shafts, bores, concentric features
Strength on tolerance-critical featuresPositional relationships across multiple faces, complex pocket depths, hole patternsDiameters, roundness, concentricity, perpendicularity to axis
Where it gets challengingDeep pockets (depth more than 3× width), thin walls, small features with long tool reach, large flat surfaces prone to chatterNon-round features, interrupted cuts, off-centre features, very long parts without tailstock support
Inspection advantageMulti-point CMM for three-dimensional relationshipsIn-process measurement of diameters during machining
Specify tighter tolerances forBolt-hole patterns, mating surfaces, press-fit pockets, critical wall thicknessesBearing journals, seal bores, press-fit diameters, threaded interfaces

The rule of thumb: for cylindrical tolerance-critical features such as shafts, bores, and bearings, turning usually achieves tighter tolerances more cost-effectively. For features that need positional accuracy across several surfaces or complex three-dimensional relationships, milling is the better choice.

Materials change what is realistic

Metals are more dimensionally stable and predictable during machining, which makes tighter tolerances practical and repeatable. Plastics are more sensitive to heat and moisture and can warp or creep after machining, so tight tolerances are less predictable and often more expensive. The Hubs guide applies ISO 2768-f to metals and ISO 2768-m to plastics for exactly this reason.

That does not mean plastic parts cannot be precise — it means the tolerance should be set with the material in mind. A ±0.02 mm bore in aluminium is a routine callout; the same bore in nylon, which absorbs moisture and moves with temperature, needs a conversation about the measuring conditions (temperature, humidity, time after machining) before it needs a tighter number.

Finish changes dimensions — state before or after

A finish is not only a surface. It changes the size of the feature it covers, and a tolerance that does not say whether it applies before or after finishing cannot be checked:

  • Removal finishes such as polishing and brushing take material away.
  • Build-up finishes such as powder coating, electroless nickel plating, and anodizing add thickness.
  • Abrasive finishes such as bead blasting mainly change texture, but can still matter on mating or sliding surfaces.

The standard as-machined finish is Ra 3.2 µm. For anything beyond that, write on the drawing whether the dimensions apply before or after the finish — for example "Ø20.00 ±0.02 mm after anodizing" — and include it in the tolerance stack for fit-critical features such as bores, shafts, and sealing faces. Our guide to specifying surface finish on CNC machined parts explains the Ra values and finishes themselves; this article is about what they do to your dimensions.

Drawing-callout checklist

Before the drawing goes out, run through these seven checks:

  1. ISO class in the title block — "ISO 2768-m" or "ISO 2768-f" so every unmarked dimension has a defined tolerance.
  2. Critical dimensions flagged — only the dimensions that affect fit, function, sealing, or alignment carry specific tolerances; the rest stay on the default.
  3. Datums stated — every GD&T callout references a datum, so the supplier and the inspector measure from the same origin.
  4. GD&T where the relationship matters — position, perpendicularity, or runout instead of tightening every size dimension.
  5. Threads called out — thread size, pitch, and class on the drawing; threads follow their own ISO standards.
  6. Pre- or post-finish stated — whether each tolerance applies before or after finishing, especially on fit-critical features.
  7. Inspection method agreed — which instrument checks each tight dimension (caliper, micrometer, gauge, CMM), and whether a first-article report is required.

A drawing that passes all seven can be quoted without a round of clarification questions — and the price that comes back is priced against the tolerances you actually need. Our quality control and inspection page describes the stage checkpoints — incoming material, first-off, in-process, and final — where this evidence is collected.

Frequently asked questions

Can I mix tolerance standards on the same part?
Yes. Use ISO 2768-1 as the general tolerance, then call out tighter tolerances for the critical dimensions. That keeps costs down by adding precision only where it is needed.

What if I need tolerances tighter than ISO 2768-f?
Put the detailed specification on the technical drawing and ask the supplier to review feasibility and pricing at quote. A tolerance below the default is a discussion, not a line item — the supplier needs to confirm the feature, the material, and the measurement method.

Should I tolerance every dimension tightly "just to be safe"?
No. Over-tolerancing is the most common way buyers pay for precision they do not need. Tighten the dimensions that affect fit, function, or sealing; leave the rest on the ISO default.

Send the drawing with the tolerances already decided

The fastest way to a comparable CNC quote is to send the drawing with the tolerance decisions already made: the ISO class in the title block, the critical dimensions flagged, and the finish and inspection requirements stated. Use our contact page and include the STEP file, the 2D drawing with the ISO 2768 class and flagged critical dimensions, the material, the quantities, the key tolerances, the finish per surface, and your target timing — and we will quote against those tolerances rather than assuming them.

Hey! I’m Jerry — a hands-on mold & CNC guy who’s spent years turning ideas into real, tangible products. From tight-tolerance molds to complex machining projects, I’ve seen (and solved) a bit of everything.

Beyond the tools and machines, I’m all about people: building trust, making things easier for clients, and finding smart solutions that work. I’ve worked with teams around the world, and I’m always excited to meet others who love creating and building as much as I do.

If you’re into manufacturing, product development, or just like a good behind-the-scenes look at how things get made — let’s connect!

Send Us Your Requirements

Let's review your mold project

Tell us what you’re building and we’ll help identify the right tooling path. Send your 2D drawing, 3D CAD file, resin, annual volume, tolerances, or target timeline when available.

Engineering-led reviewReply within one business dayConfidential project details

No obligation. We’ll review the information and reply with a practical next step. Prefer email? jerry@cavitymold.com.