Guide
Machining tolerances: what to put on your drawing.
Which tolerance each feature needs, what a tighter one does to the price, and what applies when your drawing says nothing.
What a tolerance is, and what “standard” means
A tolerance is how far a dimension may stray and still be accepted: 25 mm ±0.1 means anything from 24.9 to 25.1. “Standard tolerance” is used for three different things, which is why two suppliers can quote the same part at different numbers.
A shop default
What the workshop applies to a dimension that has no tolerance. Ours is typically ±0.1 mm or better.
An ISO class
A table by size, such as ISO 2768-m: ±0.1 mm up to 6 mm, ±0.2 mm up to 30 mm.
A capability
The best a process can hold on a feature. It is the reason a tighter number costs more.
When the drawing is silent
What applies when your drawing says nothing
A tolerance can come from three places. The first one that exists wins.
- 01
The tolerance on the dimension itself
A value written next to a dimension always wins. What you tighten or loosen there is what we quote and inspect.
- 02
The general-tolerance note in the title block
A line such as “General tolerances ISO 2768-mK” covers every dimension that has no tolerance of its own. It is the shortest way to say it once for the whole drawing.
- 03
The shop default
With neither, the workshop applies its own: typically ±0.1 mm or better, in our case. A drawing with no tolerance and no note leaves the number to the supplier.
The 3D model does not carry tolerances
A STEP file holds geometry and nothing else. Tolerances, threads and surface finish live on the 2D drawing, so a quote made from the model alone is priced at the default. If the model and the drawing disagree, we stop and ask you before anything is made; keeping them consistent is up to you.
General tolerances: ISO 2768-mK
Dimensions with their own tolerance: as shown
Ø12 H7, bearing seat: Ra 0.8
Material 6061-T6. Clear anodize; dimensions apply after finishing
An example, not a template. Only the bearing seat is tight; everything else follows the general note, so only that feature is priced as tight.
ISO 2768
General tolerances: ISO 2768 in one table
The permissible deviation, in mm, by nominal size and class. The default reference for machined and sheet-metal parts.
| Size range, mm | f · fine | m · medium | c · coarse | v · very coarse |
|---|---|---|---|---|
| 0.5–3 | ±0.05 | ±0.1 | ±0.2 | – |
| >3–6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| >6–30 | ±0.1 | ±0.2 | ±0.5 | ±1 |
| >30–120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| >120–400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| >400–1000 | ±0.3 | ±0.8 | ±2 | ±4 |
| >1000–2000 | ±0.5 | ±1.2 | ±3 | ±6 |
| >2000–4000 | – | ±2 | ±4 | ±8 |
- Below 0.5 mm the deviation is written next to the dimension.
- ISO 2768-mK reads as class m for linear and angular dimensions (part 1) and class K for form and position (part 2).
- Part 2 (classes H, K, L) has been withdrawn and replaced by ISO 22081:2021; part 1 dates from 1989 and a revision is in preparation. Drawings still cite “mK”, so it works, but a feature whose form or position matters is better given its own geometric tolerance than left to a general class.
- ISO 2768 is a table of general tolerances, not a certificate: nobody is “ISO 2768 certified”.
By feature
Which tolerance goes on which feature
Tighten what the part does and leave the rest to the general note.
Finishing changes a dimension
Anodizing and plating add material to the surface, and powder coat adds a layer. Say on the drawing whether a dimension applies before or after finishing, and call out threads and tight bores as masked or as finished.
| Feature | What to specify | Why |
|---|---|---|
| Bore for a bearing or a pressed bushing | A fit on the hole and on the shaft, e.g. H7 with p6 | The fit is what holds the part. A general ±0.1 mm cannot give it. |
| Dowel pin hole | H7 on the hole and a position tolerance on the pair | What matters is where the two holes are, more than their diameter. |
| Sliding or rotating fit | H7/g6 for a close fit, H8/f7 for a free one | A clearance fit is always loose; the grade sets how much. |
| Seal groove | Width and depth from the seal supplier’s table, and a surface roughness | The seal sets the number, not the part. |
| Thread | Size, class (6H internal, 6g external) and depth | The thread standard already holds the diameter. Do not tolerance it again. |
| Face that mates with another | Flatness on that face, e.g. 0.05 mm | A size tolerance alone does not limit form. |
| Outer envelope, cosmetic faces | Nothing: the general note | Every extra tolerance is something to set up and to inspect. |
Price
Why a tighter tolerance costs more
It is not the number on the drawing. It is what it takes to hold it.
What we do with it
We do not price a tolerance for the whole part. Mark the dimension on the 2D drawing: we review it, we hold it and we price only that feature. A tighter tolerance usually means more process control and inspection, and a higher price on that feature.
Slower cutting
A tight feature is finished with a light pass at a lower feed, and sometimes in a second operation such as reaming or grinding.
More setups and fixturing
Features that have to line up with each other are cut in one setup, or measured again between setups.
Inspection
A ±0.1 mm dimension is checked with a caliper. A much tighter one needs a gauge or a CMM, one feature at a time.
Scrap and tool wear
The closer to the limit, the more parts fall outside it and the more often the tool has to be checked.
ISO 286
Fits and IT grades
An IT grade is the width of the tolerance zone for a given size. A fit pairs a hole with a shaft.
Read H7/g6 like this: the capital letter is the hole, the lowercase letter the shaft, the number the IT grade, and the letter the position of the zone. The tighter the grade, the more the operation changes (reaming, boring, grinding), and the price follows the operation.
| Size range, mm | IT5 (µm) | IT6 (µm) | IT7 (µm) | IT8 (µm) | IT9 (µm) | IT10 (µm) | IT11 (µm) | IT12 (µm) |
|---|---|---|---|---|---|---|---|---|
| >3–6 | 5 | 8 | 12 | 18 | 30 | 48 | 75 | 120 |
| >6–10 | 6 | 9 | 15 | 22 | 36 | 58 | 90 | 150 |
| >10–18 | 8 | 11 | 18 | 27 | 43 | 70 | 110 | 180 |
| >18–30 | 9 | 13 | 21 | 33 | 52 | 84 | 130 | 210 |
| >30–50 | 11 | 16 | 25 | 39 | 62 | 100 | 160 | 250 |
| >50–80 | 13 | 19 | 30 | 46 | 74 | 120 | 190 | 300 |
| >80–120 | 15 | 22 | 35 | 54 | 87 | 140 | 220 | 350 |
| >120–180 | 18 | 25 | 40 | 63 | 100 | 160 | 250 | 400 |
H7/g6
Clearance
The shaft always fits loosely in the hole. For parts that slide or turn: guides, pivots, free-moving pins.
H7/k6
Transition
A slight clearance or a slight interference. It locates a part accurately and can still be taken apart.
H7/p6
Interference
The shaft is always larger than the hole. It is pressed in and held by the fit: bushings, pressed pins.
By process
What each process holds, and the standard behind it
Tolerance means something different in each process. These are the defaults we apply when the drawing says nothing, and the standard that governs the part.
These are defaults for a dimension with no tolerance of its own; a tolerance on the drawing overrides them. Welded structures fall under ISO 13920.
| Process | Default we apply | Governing standard |
|---|---|---|
| CNC machining | Typically ±0.1 mm or better | ISO 2768-1 |
| Sheet metal, cut features | ±0.2 mm | ISO 2768-1 |
| Sheet metal, bend angle | ±1° | ISO 2768-1 |
| Injection molding | ±0.25 mm | ISO 20457 |
| 3D printing: FDM | ±0.5 %, minimum ±0.5 mm | – |
| 3D printing: SLS, MJF, SLA | ±0.3 %, minimum ±0.3 mm | – |
| Die and sand casting | Ask with the file | ISO 8062-3 |
Tool
Look up a tolerance for your size.
A general tolerance from ISO 2768-1 and an IT grade from ISO 286. It is what the standard says, not a quote.
General tolerance, ISO 2768-1
±0.2 mm
Size over 6 mm, up to 30 mm
Tolerance zone, ISO 286 · IT7
21 µm (0.021 mm) wide
Size over 18 mm, up to 30 mm
For other sizes, fits with a specific shaft and hole deviation, or anything else the tables do not say, send the drawing.
What to send
What you send, and what you get back.
The 3D model and the PDF drawing are enough.
Your 3D model (STEP) and the 2D PDF drawing
The model gives the geometry; the drawing carries what the model cannot say: tolerances, threads, surface finish. Mark the dimensions that need to be tight and add the general-tolerance note; everything else follows it.
A price per part, in 24–48 hours
With the unit price and the lead time of every part, finishing included.
If a tolerance can’t be held, the change it needs
We tell you before anything is made, and requote it.
Questions
Questions about tolerances
What engineers and buyers ask before they draw the note.
What tolerance applies if my drawing doesn’t specify one?
The general-tolerance note in the title block, if the drawing has one (for example ISO 2768-mK). If it has none, the workshop default, which for us is typically ±0.1 mm or better. A tolerance written next to a dimension always overrides both. A drawing with no tolerance and no note leaves the number to the supplier, so one line is worth adding.
What tolerance can CNC machining hold?
Typically ±0.1 mm or better is our default, and it covers most features without adding cost. A tighter dimension is marked on the 2D drawing: we review it, hold it and price only that feature. For fits, ISO 286 grades IT6 to IT8 are the usual choice.
Do I need a 2D drawing if I upload a STEP file?
Yes, for anything the model cannot say: tolerances, threads, surface finish. A STEP file holds geometry only, so a quote made from the model alone is priced at the default tolerance. If the model and the drawing disagree, we stop and ask you before anything is made.
Which ISO 2768 class should I choose, m or f?
The loosest the part can work with. Class m is ±0.1 mm up to 6 mm and ±0.3 mm from 30 to 120 mm; class f is half of that up to 120 mm. If one feature needs more, give that feature its own tolerance instead of tightening the whole drawing.
Is ISO 2768-2 still valid?
No. ISO 2768-2 (classes H, K and L for form and position) was withdrawn and replaced by ISO 22081:2021. Many drawings still cite “mK”; for a feature where form or position matters, give it its own geometric tolerance. ISO 2768-1, for linear and angular dimensions, is still in use and is being revised.
Why does a tighter tolerance cost more?
Because holding it takes slower cutting, sometimes a second operation, more care with setups and more inspection, and more parts fall outside the limit. It is the feature that carries the cost, which is why we price only the dimensions you mark as tight and not the whole part.
What tolerance should I use for a press fit in aluminum?
A common choice is H7 on the hole with p6 on the shaft for a light interference fit, and k6 where the part must still be taken apart. Aluminum expands more with temperature than steel and is softer, so give the working temperature and the mating material when you send the drawing.
Do tolerances apply before or after anodizing?
Say it on the drawing. Anodizing adds a thin layer to the surface, so a dimension that has to be met after finishing is machined with that in mind, and one that applies before finishing is inspected before. Without a note, we ask you.
Are tolerances different for sheet metal, molding and 3D printing?
Yes: each process has its own default and its own standard. For sheet metal we apply ±0.2 mm on cut features and ±1° on bends, for injection molding ±0.25 mm, and for 3D printing a percentage of the size with a minimum, by technology. The table above has them.
Read next
Still have a question?
Send your part and ask an engineer.
Your parts protected by an NDA before you upload them.