+91 97253 36833info@cnc-shopfloor.com Exporting Anywhere in the WorldWe deal under NDA
Home About Services Industries Gallery Capabilities FAQ Blog Contact Request a quote
Home / Blog / CNC Machining Tolerances Explained: A Guide for Buyers
Insights · 18 Nov 2026

CNC Machining Tolerances Explained: A Practical Guide for Buyers

A tolerance tells the machinist how far a dimension is allowed to vary from the number on the drawing. Get tolerances right and parts fit first time at a fair price. Get them wrong and you either receive parts that do not assemble, or pay for precision that the part never needed.

This guide explains how tolerances work on a CNC drawing, what the common notations such as ISO 2768-m, H7/g6 and GD&T actually mean, and how to specify them so your supplier can quote accurately and deliver parts that work.

What a tolerance actually means

No machine can make a dimension that is perfectly exact. A tolerance defines the range that is acceptable. For a hole marked Ø20 ±0.05, any diameter from 19.95 mm to 20.05 mm passes inspection. Tolerances can be written in a few ways:

  • Bilateral: 20 ±0.05, the same amount above and below the nominal size.
  • Unilateral: 20 +0.02/0, variation allowed in one direction only. This is common for holes and shafts that must fit together.
  • Limit dimensions: 20.00 / 20.02, the minimum and maximum written out directly.
  • Fit codes: Ø20 H7, a standard tolerance band from ISO 286, explained below.

The tolerance decides how a feature is machined and how it is checked. That is why it has such a large effect on cost.

Standard vs tight tolerances

The table below gives a rough idea of what different tolerance bands mean on the shop floor. The exact limits depend on the size of the feature, the material and the machine, so treat it as a guide rather than a rule.

Tolerance bandWhat it means in practiceTypical use
±0.1 to ±0.3 mmStandard machining. No special effort needed.Outside dimensions, clearance holes, non-mating features
±0.05 mmRoutine on a well-maintained CNC machine with careful setup.Mating faces, hole positions in assemblies
±0.01 to ±0.025 mmPrecision work. Slower finishing passes, stable temperature and closer inspection.Bearing seats, dowel holes, sliding fits
Tighter than ±0.01 mmOften needs grinding, honing or lapping after machining.Gauges, hydraulic spools, high-precision bores

Every step down the table adds machining time and inspection effort. Our article on what drives CNC machining cost explains why over-tight tolerances are one of the most common hidden cost drivers.

General tolerances: ISO 2768 in one table

Most drawings do not put a tolerance on every single dimension. Instead, the title block carries a note such as "General tolerances ISO 2768-mK". Every dimension without its own tolerance then follows that standard.

The first letter sets the class for linear dimensions: f (fine), m (medium), c (coarse) or v (very coarse). Medium is the usual choice for machined parts.

Nominal size (mm)f (fine)m (medium)c (coarse)v (very coarse)
0.5 to 3±0.05±0.1±0.2–
over 3 to 6±0.05±0.1±0.3±0.5
over 6 to 30±0.1±0.2±0.5±1.0
over 30 to 120±0.15±0.3±0.8±1.5
over 120 to 400±0.2±0.5±1.2±2.5
over 400 to 1000±0.3±0.8±2.0±4.0
over 1000 to 2000±0.5±1.2±3.0±6.0

The second letter (H, K or L, from ISO 2768-2) sets general limits for geometry such as straightness, flatness and perpendicularity. If a drawing has no general tolerance note at all, the supplier has to guess, and two shops may guess differently. Always include one.

Fits for holes and shafts (ISO 286)

When a pin, shaft or bearing has to go into a hole, the relationship between the two sizes matters more than either size alone. ISO 286 defines standard tolerance bands for this, written as a letter and a number. A capital letter is used for holes and a small letter for shafts. For example, a Ø10 H7 hole may measure anywhere from 10.000 mm to 10.015 mm.

Common hole-and-shaft combinations are:

  • H7/g6, sliding fit: a small clearance so the parts move freely but accurately, for example a locating pin that must slide.
  • H7/h6, locational clearance fit: parts assemble by hand with almost no play.
  • H7/k6, transition fit: may be a slight clearance or a slight interference. Used for accurate location of hubs and gears.
  • H7/p6, press fit: an interference fit, assembled with a press. Used for bushes and dowels that must not move.

Using fit codes rather than inventing your own ± values tells any trained machinist exactly what you need, and it lets the shop use standard reamers and gauges.

Geometric tolerances (GD&T): when ± is not enough

A ± tolerance controls size, but not shape, orientation or location. A hole can be the right diameter but in the wrong place, or a face can be the right thickness but not flat. Geometric dimensioning and tolerancing (GD&T, defined in ISO 1101 and ASME Y14.5) covers these cases:

  • Position controls where holes and features sit relative to datum surfaces. It is the best way to make sure a bolt pattern lines up with its mating part.
  • Flatness matters for sealing faces and mounting surfaces.
  • Perpendicularity and parallelism control how faces and bores relate to each other.
  • Runout and concentricity matter for rotating parts such as shafts and pulleys.

GD&T works from datums, usually labelled A, B and C. These are the reference surfaces that the part is located on, both in the machine and during inspection. Choosing datums that match how the part is assembled gives the most useful result.

Watch out for tolerance stack-up

When dimensions are chained one after another, their tolerances add up. Four holes dimensioned from each other at ±0.1 mm each can leave the last hole up to ±0.4 mm away from where you expect it relative to the first edge.

The fix is to dimension critical features from a single datum (baseline dimensioning), or to use a position tolerance. This keeps the error on each feature independent of the others.

Surface finish goes hand in hand

Tolerance and surface finish are linked. A tight tolerance on a rough surface makes little sense, because the roughness itself can use up part of the tolerance. Surface roughness is usually given as Ra in micrometres (µm):

  • Ra 3.2 µm: a standard as-machined finish, fine for most functional parts.
  • Ra 1.6 µm: a finer machined finish for mating and visible surfaces.
  • Ra 0.8 µm: for sliding surfaces, seals and bearing seats. Needs careful finishing passes.
  • Ra 0.4 µm and finer: usually needs grinding, honing or polishing.

What affects the tolerance a shop can hold

  • Material. Aluminium and brass machine predictably. Plastics expand with heat and some absorb moisture, so tight tolerances on plastic parts are harder to hold and may change after delivery. Stainless steel work-hardens and needs care.
  • Part geometry. Thin walls, long slender shafts and deep bores deflect under cutting forces, which makes tight tolerances more difficult.
  • Feature size. The same tolerance is easier to hold on a 10 mm feature than on a 500 mm one.
  • Coatings. Anodizing, plating and powder coating add thickness. Typical anodizing grows the part surface by roughly half of the coating thickness. State whether tolerances apply before or after finishing, and mark critical bores and threads for masking. Our guide to surface finishes covers each coating in more detail.
  • Heat treatment. Hardening can distort a part. Features with tight tolerances are often finish-machined or ground after heat treatment.

How tolerances are checked

A tolerance is only useful if it can be measured. Typical inspection tools include calipers and micrometers for general sizes, bore gauges and pin gauges for holes, thread gauges for threads, height gauges for step heights and a CMM (coordinate measuring machine) for hole positions and GD&T. If you need an inspection report or a first article inspection (FAI) on critical dimensions, ask for it in your RFQ so it is included in the quote.

Checklist: tolerancing your next drawing

  • Add a general tolerance note, for example ISO 2768-mK.
  • Put tight tolerances only on features that really need them, such as fits, sealing faces and locating features.
  • Use standard fit codes (H7/g6, H7/p6 and so on) for holes and shafts.
  • Use datums and position tolerances for hole patterns that must line up with a mating part.
  • Dimension critical features from a common datum to avoid stack-up.
  • Specify surface finish where it matters, and say whether tolerances apply before or after coating.
  • Mark the critical dimensions you want reported on inspection.
  • Send a 3D model with the 2D drawing. Our guide on which CAD files to send for a CNC quote explains why.

Conclusion

Good tolerancing is about precision where it matters and sensible general tolerances everywhere else. A clear general tolerance note, standard fits for holes and shafts, and GD&T for critical locations give your supplier everything needed to quote accurately and make parts that assemble first time. If you are unsure whether a tolerance is too tight, send us the drawing. Our CNC machining services team reviews tolerances as part of every quote and points out where a change could save cost, all under NDA. Request a quote.

FAQ

What is the standard tolerance for CNC machining?
When a drawing gives no other tolerance, many shops work to ISO 2768-m (medium). That is ±0.1 mm for features up to 6 mm, ±0.2 mm from 6 to 30 mm and ±0.3 mm from 30 to 120 mm. Tighter tolerances are possible but should be called out only on features that need them.
What does ISO 2768-mK mean on a drawing?
It sets the general tolerances for every dimension that has no tolerance of its own. The m means the medium class for linear and angular dimensions (ISO 2768-1), and the K sets the class for geometric tolerances such as flatness, straightness and perpendicularity (ISO 2768-2).
Do tighter tolerances always cost more?
In general, yes. Tighter tolerances need slower finishing passes, more careful setups and more inspection. Below about ±0.01 mm, parts often need extra operations such as grinding or honing, which adds cost and lead time.

Have a part to make? Let's talk.

Request a quote