The callout „ø30 H7” takes up a few characters on a drawing, yet it decides whether a bearing will seat in its housing, whether a dowel pin will locate a part the way the designer intended, and how much the machining will cost. Our article on tolerances in CNC machining covered the basics. Here we go one level deeper: what the most common tolerance zones actually mean, how many micrometres they are worth, and how to combine them into a fit.
How to read ø30 H7
The callout has three parts:
- ø30 — the nominal size,
- the letter — the position of the tolerance zone relative to the nominal size; a capital letter is always the hole, a small letter the shaft,
- the number — the IT grade, that is the width of the tolerance zone. The lower the number, the narrower the zone.
The letter H marks a hole whose lower deviation is zero — the hole can only come out larger than nominal. The letter h marks a shaft whose upper deviation is zero — the shaft can only come out smaller. That is why H and h are the starting point of most fits.
One thing to keep in mind: the width of the zone depends on the diameter. IT7 is 15 μm at ø8 and already 35 μm at ø100. „H7” is therefore not a single value but a rule you have to read from a table for your particular size.
Calculate it instead of looking it up. Rather than reading the deviations off the table below, you can have them straight away: ISO 286 fits and tolerances calculator — enter a diameter and a fit such as ø30 H7/g6 and get the deviations, the limit sizes and the clearance or interference. It runs in your browser and sends nothing to a server.
Deviation table for the most common tolerance zones
Deviations in micrometres (1 μm = 0.001 mm), to ISO 286:
| Nominal diameter | H7 (hole) | h6 (shaft) | g6 (shaft) | js9 | h9 (shaft) |
|---|---|---|---|---|---|
| over 6 up to 10 mm | +15 / 0 | 0 / −9 | −5 / −14 | ±18 | 0 / −36 |
| over 10 up to 18 mm | +18 / 0 | 0 / −11 | −6 / −17 | ±21.5 | 0 / −43 |
| over 18 up to 30 mm | +21 / 0 | 0 / −13 | −7 / −20 | ±26 | 0 / −52 |
| over 30 up to 50 mm | +25 / 0 | 0 / −16 | −9 / −25 | ±31 | 0 / −62 |
| over 50 up to 80 mm | +30 / 0 | 0 / −19 | −10 / −29 | ±37 | 0 / −74 |
| over 80 up to 120 mm | +35 / 0 | 0 / −22 | −12 / −34 | ±43.5 | 0 / −87 |
How to read it: a ø25 g6 shaft has to end up between 24.980 and 24.993 mm. A ø25 H7 hole — between 25.000 and 25.021 mm.
Have a drawing of your part? Send it for a quotation. Email the drawing to biuro@hardpower.pl or describe the part in the contact form — we will reply and ask for the drawing. HARDPOWER is a CNC machining company in Szczecin, Poland, certified to ISO 9001:2015 (PRS certificate no. NC-3170).
What the individual zones mean
H7 — the most widely used hole tolerance in machine building. Holes for dowel pins, bushings, bearing seats, guideways. Drilling alone will not produce it: an H7 hole comes from reaming, boring or finish milling.
h6 — a shaft that runs „from zero downwards”. Paired with H7 it gives a sliding fit with very little clearance: the parts go together by hand yet guide each other accurately. Typical for locating and interchangeable components.
g6 — a shaft shifted slightly below nominal. Paired with H7 there is always a small clearance left, so the parts can slide or rotate relative to each other. The classic fit for guideways, pins and moving parts that still need accurate guidance.
js9 — a symmetrical zone: half the tolerance above nominal, half below. Used where what matters is the position relative to nominal rather than the direction of the deviation — keyway widths, hole spacings, locating dimensions without an interference fit.
h9 — a wide shaft tolerance „downwards”. Found on drawn bars, on shafts under retaining rings and wherever a free fit is good enough. Distinctly cheaper to produce than h6.
Worked example: the ø30 H7/g6 fit
Hole ø30 H7: from 30.000 to 30.021 mm.
Shaft ø30 g6: from 29.980 to 29.993 mm.
- minimum clearance: 30.000 − 29.993 = 0.007 mm,
- maximum clearance: 30.021 − 29.980 = 0.041 mm.
Whichever parts from the batch happen to meet, the clearance will always fall between 7 and 41 μm. That is the whole point of a fit: the parts are interchangeable without hand fitting.
For comparison, H7/h6 at the same diameter gives a clearance from 0 to 0.034 mm — tighter, with the option of assembling the parts flush.
The hole-basis system
On the shop floor it is easier to produce an accurate shaft to any size than an accurate hole — holes are made with fixed-size tooling such as reamers and checked with plug gauges. This is why the hole-basis system is used almost everywhere: the hole is always H, and the character of the fit is set by the shaft tolerance (g6 — clearance, h6 — sliding, k6/n6 — transition, p6 and beyond — interference). If you are designing a part for CNC machining, sticking to this rule usually lowers the cost.
What a tighter grade costs
Every IT grade down narrows the tolerance zone by more than a third. For machining that means an extra finishing pass, slower parameters, more frequent inspection and a higher risk of scrap. In practice:
- grades IT9–IT11 are ordinary machining — no effect on price,
- IT7–IT8 call for a finishing operation and dimensional inspection,
- IT6 is already a critical dimension: stable temperature, every part measured or dense sampling across the batch,
- IT5 and tighter — after an individual review of the drawing; grinding often comes into play.
On the drawings that reach us, by far the most common zones are H for holes and h for shafts — H7, H8, h6, h7, h9 — alongside fits with g6 and dimensions in the js zone. Dimensions marked as critical we hold on turned and milled parts and confirm by measurement, and where the requirements are unusually tight we assess feasibility already at the quotation stage.
The conclusion for a designer is simple: specify a fit only where the parts actually work together. Leave the remaining dimensions to the general tolerance ISO 2768-m — which for sizes from 6 to 30 mm is ±0.2 mm, and from 30 to 120 mm ±0.3 mm.
How we verify fits
Fitted dimensions are measured on a Mitutoyo CRYSTA-APEX S9106 coordinate measuring machine with an accuracy of 0.5 μm, at a controlled temperature. That matters: a steel shaft of ø100 warmed by 5 °C grows by roughly 6 μm, which is a quarter of the h6 zone. On request we supply an inspection report with the batch. More on how we measure in our article on precision measurement and quality control and on our precise measurement page.
Frequently asked questions
What does the tolerance H7 mean?
It is a hole tolerance zone: the lower deviation is zero, the upper one depends on the diameter — for example +0.021 mm for ø18–30 mm.
What is the difference between h6 and g6?
Both apply to a shaft in IT grade 6. h6 starts at the nominal size and runs downwards; g6 is additionally offset from nominal (by 7 μm for ø18–30, for instance), so paired with an H7 hole it always leaves a clearance.
Which fit should I choose for a dowel pin?
Dowel pins are most often produced to m6. In an H7 hole this gives a transition fit — the pin sits firmly, yet the joint can still be taken apart. If one of the parts is to be removed often, its hole is made with slightly more clearance.
Can I put H7 on every hole just to be safe?
You can, but the part will be needlessly more expensive. Every H7 hole is an extra operation and an extra measurement. Fits are worth keeping for holes that genuinely mate with something.
Do you check the tolerances on a drawing before quoting?
Yes. If a callout is impossible to produce, self-contradictory or needlessly drives the cost up, we flag it with the quotation.
Have a drawing of your part? Send it for a quotation. Email the drawing to biuro@hardpower.pl or describe the part in the contact form — we will reply and ask for the drawing. HARDPOWER is a CNC machining company in Szczecin, Poland, certified to ISO 9001:2015 (PRS certificate no. NC-3170).
