Tolerances in CNC machining: how they work and which ones to specify
The general tolerance we apply if you say nothing, how tight it can go, what it costs and how to specify a fit without making the whole part more expensive.
If you do not specify any tolerance, a machined part is manufactured with the general ISO 2768-f tolerance for metals and ISO 2768-m for plastics: on a dimension of 25 mm it is ±0.1 mm, the thickness of two sheets of paper. This is sufficient for nine out of ten parts. The tenth, the one with a shaft that fits into a bearing or a pin that goes into a hole, needs a specific tolerance on a specific dimension. And only there.
In this guide we explain how tolerances work in custom CNC machining: what is applied by default, how far you can refine, why a tight tolerance increases the part cost, and how to specify an H7 or g6 fit on the drawing so it comes out right the first time.
A tolerance is the margin of error you accept. The smaller it is, the slower the machining and the more it is measured. Request the tight tolerance only on dimensions where one part fits with another; for the rest, the general tolerance is already very fine.
What is a dimensional tolerance?
No machine produces an exact dimension: a 25 mm shaft comes out as 24.98 or 25.03 depending on the tool, temperature, and wear. The tolerance is the interval within which the dimension is considered acceptable. It is written in two ways:
- With limits: 25 ±0.05, or 25 +0.02/−0.01. This is the clearest way for individual dimensions.
- With an ISO 286 class: 25 H7, 25 g6. A letter indicates the position of the interval relative to the nominal dimension (H starts at zero and goes up; g stays below) and a number, the IT grade, which is the width of the interval. A 25 H7 ranges from 25.000 to 25.021 mm: a 21-micron margin.
The lower the IT number, the narrower the interval: IT11 is 130 µm for Ø25, IT7 is 21 µm, and IT6 is 13 µm. The ISO 286 tolerance calculator gives you the limits for any dimension and class without opening the standard.
What tolerance is applied if I do not specify anything?
The ISO 2768-1 standard defines general tolerances by dimension ranges. At Proto&Go! we apply class f (fine) for metals and class m (medium) for plastics, which move more with temperature and humidity:
| Nominal dimension (mm) | Class f · fine (metals) | Class m · medium (plastics) |
|---|---|---|
| 0,5 a 3 | ±0,05 | ±0,1 |
| more than 3 to 6 | ±0,05 | ±0,1 |
| more than 6 to 30 | ±0,1 | ±0,2 |
| more than 30 to 120 | ±0,15 | ±0,3 |
| more than 120 to 400 | ±0,2 | ±0,5 |
| more than 400 to 1.000 | ±0,3 | ±0,8 |
This covers housings, brackets, plates, fixtures, functional prototypes and the vast majority of parts that don't mate with another through a fit. The standard also sets general tolerances for angles, radii and chamfers, which are included.
How far can you refine in CNC machining?
For specific dimensions indicated on the drawing, we achieve IT7 in metals (21 µm in Ø25) and IT11 in plastics. On the lathe, outer diameters can even reach IT6, because the part rotates on its own axis and the tool only needs to maintain a distance. Precision holes are honed or reamed; below IT6 requires grinding, which is another process and another price.
Geometric tolerances (flatness, parallelism, perpendicularity, concentricity) are specified the same way and are achieved mainly by machining the related faces in the same setup. That is why a part with two faces perpendicular to within 0.02 mm comes out better from a 5-axis machining center, which machines them without unclamping.
Why does a tight tolerance increase the part cost?
Because it changes how that dimension is machined, not just how it is measured:
- Slower finishing passes, with less depth of cut and new tooling.
- In-machine and off-machine measurement: each IT7 dimension is checked with a micrometer or probe, part by part.
- Temperature control: aluminum expands 23 µm per meter and degree; a 200 mm part changes 5 µm between the machine and the measurement room.
- More rejection: a part out of a 20 µm tolerance is scrapped; out of 200 µm, almost never.
The result is that an IT7 dimension can double or triple the time for that operation. If there are two or three dimensions on a part, it barely affects the total price; if the whole part is ±0.02, the price skyrockets without the part functioning better. It is the same criterion we apply in how to reduce the cost of a machined part.
Fits: how to choose H7, h6, g6 and company
A fit is the relationship between a hole and a shaft that are assembled. The standard system is the hole-basis system: the hole is always made H7 and the shaft class is chosen based on what is required:
| Fit (H7 hole) | Shaft | Result | Example |
|---|---|---|---|
| Clearance | g6, f7 | Rotates or slides with small clearance | Shaft in a bushing, sliding guide |
| Fine sliding | h6 | Fits by hand, with no appreciable clearance | Centering pin, guide column |
| Slightly forced | k6, m6 | Fits with a hammer, it comes apart | Bearing on a shaft |
| Press fit | p6, s6 | Pressed into a press, it does not come apart | Bushing in a housing |
The shaft-hole fit calculator shows the resulting clearance or interference for any combination. And a tip that avoids many problems: set the tight tolerance on the easiest part to machine. A turned shaft to h6 is routine; a deep blind hole to H6, not.
Tolerances and finishes: the detail that is forgotten
Finishes add or remove material: anodizing adds 2.5 to 12.5 µm to each face (one diameter, double), zinc plating adds 5 to 15 µm, and RAL painting adds 40 to 100 µm. It does not matter for a dimension with general tolerances; for an H7 with a 21 µm margin, it could be the entire margin. If the dimension must be met after finishing, state it in the drawing and it will be machined corrected, or the area will be masked. You have the thicknesses for each finish in surface finishes for CNC machining.
And in 3D printing, sheet metal, and vacuum casting?
Each process has its precision. MJF 3D printing works with ±0.3 mm up to 100 mm and ±0.3% above; in sheet metal, the cut contour and the bent part have different precisions; in vacuum casting, the tolerance depends on the resin shrinkage and the geometry. If you are unsure which process meets the tolerance you need, the guide to tolerances by manufacturing process compares them in a table.
How to indicate tolerances in the order
- Upload the STEP. The 3D model carries the nominal geometry, but not the tolerances or the threads.
- Add a PDF assigned to the part with only the functional dimensions: fits, threads, distances between drilled holes that mount with another part.
- Write the tolerance as limits (±0.02) or as class (25 H7). Both are valid.
- If a dimension must be met after finishing, indicate it.
- Do not set a finer general tolerance in the box "just in case": it makes the whole part more expensive. ISO 2768-f is already fine.
The engineer reviewing the order checks that each tolerance is achievable with the material and the process, and if any is not or is not needed, they will tell you before manufacturing. Parts are available from 8 working days and each dimension with tolerance is verified before shipping.
Frequently asked questions about machining tolerances
What tolerance does a machined part have if I don't specify any?
General tolerances ISO 2768-f apply to metals and ISO 2768-m to plastics. For a 25 mm dimension in metal, this means ±0.1 mm, sufficient for most functional parts, housings, supports, and prototypes.
What is the tightest tolerance that can be requested for CNC machining?
For specific dimensions indicated on the drawing, IT7 in metals (21 microns on a 25 mm diameter) and IT11 in plastics. Turned diameters allow IT6. Below that, grinding is required, which is another process.
What does 25 H7 mean?
It is a 25 mm nominal hole with H7 tolerance: it can measure between 25.000 and 25.021 mm. The letter H indicates that the range starts at the nominal dimension and goes upwards; the 7 is the IT grade, which sets the width of the range, 21 microns in this case.
Why does a tighter tolerance increase the part cost?
It requires slower finishing passes, measuring each part dimension by dimension, and rejecting more units. An IT7 dimension can double the time of that operation. Reserving it for functional dimensions keeps the price low without losing function.
