Engineering Tolerances & Fits: Hole-Basis Systems, Tolerance Grades and Drawing Callouts

If you have ever watched a shaft refuse to enter a hole that both parts swear is the right size, you have met the gap between a drawing dimension and a real manufactured part. No fabrication process — not a lathe, not a 3D printer, not a laser cutter — produces exactly 25.000 mm. Every process produces 25.000 mm plus or minus something. Tolerances are how you tell the machinist (or your future self at the workbench) how much "plus or minus" you can live with, and fits are how you describe what should happen when two such imperfect parts meet: slide freely, sit snugly, or grip permanently.

Get this right and your screw jack load-testing rig assembles with hand pressure and runs smoothly. Get it wrong and you are filing parts at 2 AM the night before the demo — or worse, discovering that your Geneva mechanism demo rig binds solid because the drive pin and the slot were both made "exactly to size" and neither is.

This guide explains the ISO 286 tolerance system from zero: what H7/g6 actually means, how to read and write tolerance callouts on drawings, how to pick a fit for the job, and how to check what you got with the measuring tools a student can actually afford.

The vocabulary: say it right or nobody understands the drawing

Six terms carry the whole system. Learn them precisely, because every formula and every table below assumes them.

• Nominal (basic) size — the size you write on the drawing, e.g. Ø25. It is a label, not a promise.
• Upper deviation / lower deviation — how far above or below the nominal the part is allowed to go. For a shaft specified Ø25 g6, the deviations are −0.007 mm and −0.020 mm (looked up in the ISO tables — more on that below).
• Maximum / minimum limit — nominal plus the deviations. That Ø25 g6 shaft must measure between 24.980 mm and 24.993 mm. Anything outside is scrap or rework.
• Tolerance — the width of the allowed band: maximum limit minus minimum limit. For that shaft: 24.993 − 24.980 = 0.013 mm, i.e. 13 microns. Tolerance is always a positive number; it has no sign.
• Tolerance zone — the same idea drawn as a band around the nominal line. Fit diagrams draw the hole's zone and the shaft's zone relative to a common zero line (the nominal size).
• Fit — the relationship between two mating parts' tolerance zones: whether the shaft is always smaller than the hole (clearance), always bigger (interference), or the zones overlap (transition).

The one sentence to carry into the workshop: a dimension on a drawing is not a target, it is the centre of an allowed band — and the band's width is a cost decision, not a decoration.

Why tolerance is a cost decision, not a precision contest

There is a standing relationship in manufacturing: each time you halve the tolerance, the cost roughly doubles to triples, because the process has to move from a hacksaw to a lathe to a grinder to a lapping machine. The chart below is illustrative rather than exact, but the direction is universal and every workshop quote you ever get will follow it.

Tolerance band	Typical process that achieves it	Relative cost
±0.5 mm	Hacksaw, rough cutting, 3D print (as-printed)	1×
±0.1 mm	Milling, turning, tuned 3D print	~2×
±0.05 mm	Careful turning/milling, reamed holes	~4×
±0.02 mm	Grinding, honing	~8×
±0.005 mm and tighter	Lapping, precision grinding, metrology lab	15× and up

The student lesson: specify the loosest tolerance that still lets the mechanism work. A bracket hole that only passes a bolt needs ±0.2 mm, not ±0.02 mm. The machinist will charge you — in money, time, or goodwill — for every unnecessary zero after the decimal point. When CNC drilling a PCB with GRBL, hole position matters far more than hole diameter; spend your tolerance budget where the function lives.

Reading the code: what H7, g6, and k6 actually mean

The ISO 286 designation has two parts: a letter and a number.

• The letter is the fundamental deviation — where the tolerance zone sits relative to the nominal (zero) line. Capital letters (H, K, P) are for holes (internal features); lowercase (g, k, p) are for shafts (external features).
• The number is the tolerance grade (IT grade) — how wide the zone is. Smaller number = tighter tolerance. IT7 is tighter than IT11.

So Ø25 H7/g6 reads as: a 25 mm nominal hole with an H-positioned, grade-7 zone, mating with a 25 mm nominal shaft with a g-positioned, grade-6 zone.

Three letters do most of the everyday work:

• H (hole) — the most common hole position. Its lower deviation is exactly zero: an H hole is never smaller than nominal, only larger. This is the foundation of the hole-basis system.
• h (shaft) — the mirror image: upper deviation exactly zero, so an h shaft is never larger than nominal. Common for general shafts.
• g (shaft) — sits slightly below the zero line, guaranteeing clearance against an H hole. The classic "slides freely" shaft.
• k (shaft) — sits astride the zero line, overlapping a small amount with an H hole: the classic transition fit, sometimes clearance, sometimes slight interference.
• p (shaft) — sits entirely above the zero line: guaranteed interference against an H hole. Press-fit territory.

The full alphabet runs A–ZC for holes and a–zc for shafts, with js/Js straddling the line symmetrically, but in student fabrication you will live almost entirely in the H/h/g/k/m/n/p neighbourhood.

Hole-basis vs shaft-basis: why H comes first

Two conventions exist for pairing zones:

• Hole-basis system — the hole is fixed at H (its common, easy-to-make position), and you pick the shaft letter to get the fit you want: H7/g6 (clearance), H7/k6 (transition), H7/p6 (interference). This is the default in industry and in this guide, because standard reamers and drills naturally produce H-range holes — you vary the shaft, which is easy to turn to any size on a lathe.
• Shaft-basis system — the shaft is fixed at h, and the hole letter varies (G7/h6, K7/h6, P7/h6). Used when you buy a standard shaft (cold-drawn bar, linear rail shafting) and cannot easily resize it, so you bore the hole to suit.

Practical rule: unless you are building around a bought shaft you cannot modify, use the hole-basis system. Your machinist's reamer set already speaks H.

Tolerance grades: how tight is IT7?

The IT grade sets the zone width for a given size range. The table below gives the standard tolerance values in microns (thousandths of a millimetre) for common size ranges — these are the ISO 286 numbers your machinist looks up, reproduced here so you can do fit math without the handbook.

IT grade	Ø3–6 mm	Ø6–10 mm	Ø10–18 mm	Ø18–30 mm	Ø30–50 mm	Typical use
IT6	8 µm	9 µm	11 µm	13 µm	16 µm	Precision fits: bearing seats, gauge work
IT7	12 µm	15 µm	18 µm	21 µm	25 µm	The workhorse: general precision fits
IT8	18 µm	22 µm	27 µm	33 µm	39 µm	General machining, close-running fits
IT9	30 µm	36 µm	43 µm	52 µm	62 µm	Light press fits, general parts
IT10	48 µm	58 µm	70 µm	84 µm	100 µm	Clearance fits, non-critical
IT11	75 µm	90 µm	110 µm	130 µm	160 µm	Rough machining, press work
IT12	120 µm	150 µm	180 µm	210 µm	250 µm	Coarse: flame-cut, rough cast

Notice two things: the same grade gets wider as the part gets bigger (holding 13 µm on a 25 mm shaft is ordinary lathe work; holding 13 µm on a 250 mm shaft is a different business), and IT7/IT8 covers nearly all student precision needs. If your drawing says IT5 on a college-lathe part, the machinist will quietly re-quote you.

Worked example: decoding Ø25 H7/g6 completely

Let us do the full limit arithmetic for the most common student running fit, a 25 mm shaft in a 25 mm hole. Size range Ø18–30 mm: IT7 = 21 µm, IT6 = 13 µm.

Hole Ø25 H7: H means lower deviation = 0. Tolerance width = IT7 = 21 µm, so upper deviation = +21 µm.

• Minimum hole = 25.000 mm, maximum hole = 25.021 mm.

Shaft Ø25 g6: the fundamental deviation for g in this size range is −7 µm (upper deviation), and the zone extends downward by IT6 = 13 µm, so lower deviation = −20 µm.

• Maximum shaft = 24.993 mm, minimum shaft = 24.980 mm.

The fit:

• Maximum clearance = largest hole − smallest shaft = 25.021 − 24.980 = 0.041 mm.
• Minimum clearance = smallest hole − largest shaft = 25.000 − 24.993 = 0.007 mm.

Because the minimum clearance is positive, this is a guaranteed clearance fit: the shaft always slides in the hole, with between 7 and 41 microns of play. That is the feel of a well-made sliding joint — smooth, no rattle, no binding. This is the fit you want for the lead screw nut in a screw jack load-testing rig or any shaft that must rotate or slide in its housing.

The three fit families and when to use each

Every fit is one of three kinds. The table below is the selection chart to keep open while you design — it covers the hole-basis fits that handle roughly 95% of student mechanisms.

Fit	Type	Character	Use it for
H11/c11	Clearance (loose)	Large guaranteed play	Pivots, linkages, agricultural/loose machinery feel — parts made on basic equipment
H9/d9	Clearance (free running)	Generous play	Shafts in plain bearings where you want zero risk of binding
H8/f7	Clearance (close running)	Small, reliable play	General rotating shafts, pulleys on shafts, gearbox shafts
H7/g6	Clearance (sliding)	Minimal play, always slides	Precision slides, lead screws, instrument shafts
H7/h6	Clearance (locational)	Near-zero clearance	Parts that must locate precisely but still assemble by hand — dowel pins, jig bushes
H7/k6	Transition	May clear or grip slightly	Keyed pulleys, gears on shafts — locates well, usually assembles by hand
H7/n6	Transition (tighter)	Usually slight interference	Bearing inner rings on shafts (the standard bearing-seat fit)
H7/p6	Interference (light press)	Always grips	Bushings pressed into housings, permanent light press
H7/s6	Interference (medium press)	Firm grip	Couplings, press-fit inserts that must never move
H7/u6	Interference (heavy press)	Very firm grip	Heavy-duty press fits — needs a press or thermal assembly

Two fits deserve special attention because students meet them constantly:

H7/k6 (transition) — the "locating" fit. The zones just overlap: the largest k6 shaft is a hair bigger than the smallest H7 hole. In practice, with normal manufacturing variation, most assemblies slide together with light hand pressure and a few need a tap with a mallet. Use it where a gear or pulley must sit exactly on a shaft without wobble but you still want to disassemble it. If you add a keyway, this fit plus the key is the standard way to mount transmission elements.

H7/p6 (interference) — the light press fit. The smallest p6 shaft is bigger than the largest H7 hole, so assembly always needs force (arbor press) or thermal tricks: heat the housing or chill the shaft. The parts then grip by friction alone. Use it for bronze bushings pressed into a housing or a bearing outer ring seated in its bore — places where movement would be a failure, not a feature.

Never design an interference fit you plan to assemble with a hammer and a prayer. Press fits need controlled force along the axis — a vice with soft jaws at minimum, an arbor press ideally. Hammering a press fit cocks the part, galls the surfaces, and gives you a joint that is both damaged and loose.

Choosing the fit: a decision sequence

Work through these questions in order for every mating pair on your drawing:

1. Must it move? (rotate or slide) → clearance fit. How freely? Loose pivot → H11/c11; smooth precision slide → H7/g6.
2. Must it locate precisely but come apart? → transition fit. Dowel pin → H7/h6 or H7/k6.
3. Must it never move? → interference fit. Light duty → H7/p6; permanent and loaded → H7/s6.
4. Is one part a bought standard? → check what the standard expects. Deep-groove ball bearings expect a k6 or m6 shaft and an H7 housing as the starting point (bearing makers publish full fit tables — ask your supplier for the catalogue page). Linear ball bushings on ground shafting usually want the shaft-basis approach.
5. Can your process hold it? → a transition fit is meaningless if both parts are 3D-printed at ±0.2 mm; the zones overlap by kilometres. Match the fit ambition to the process capability (see the process table above).

Measuring what you made: match the tool to the tolerance

A tolerance you cannot measure is a wish. The measuring hierarchy, with honest resolution limits:

• Steel rule — ±0.5 mm if you are careful. Fine for stock cutting, useless for fits.
• Vernier caliper (150 mm, 0.02 mm least count) — the student workhorse. Realistically trustworthy to about ±0.05 mm in student hands. Adequate for IT9 and looser, marginal for IT8.
• Outside micrometer (0–25 mm, 0.01 mm least count) — trustworthy to about ±0.01 mm with good technique (consistent ratchet pressure, clean anvils, zero-checked). This is the tool for IT6–IT8 shafts.
• Bore gauge / inside micrometer / telescopic gauges — holes are harder than shafts. Telescopic gauges plus an outside micrometer transfer the measurement; a proper bore gauge reads directly. Budget for learning time: bore measurement is a skill, not just a tool.
• Go / no-go gauges — for production-style checking: the "go" end must enter, the "no-go" end must not. You can make simple plug gauges on the lathe for your own critical holes.

The rule of thumb from metrology practice: your measuring instrument should resolve about one-tenth of the tolerance you are checking. Checking a 21 µm (IT7) tolerance with a 20 µm-least-count caliper is not inspection, it is optimism. And always measure at 20°C-ish room temperature if you are chasing microns — a 25 mm steel part grows about 0.3 µm per °C, which sounds tiny until your "IT6" measurement was taken on a part fresh off a warm lathe.

3D printing vs machining: separate tolerance worlds

Student projects increasingly mix printed and machined parts, and the two live in different tolerance universes:

• FDM 3D printing (PLA/PETG, 0.2 mm layers): expect ±0.15 to ±0.3 mm on a well-tuned printer, worse across large spans. Holes print undersized (typically 0.2–0.4 mm under nominal for small bores) because of extrusion width and shrinkage — always drill or ream printed holes that matter, or design them oversized and finish them.
• Resin (MSLA) printing: ±0.05 to ±0.1 mm is achievable — good enough for light press fits of small inserts (heat-set threaded inserts are the standard trick).
• Laser-cut acrylic/plywood: ±0.1 to ±0.2 mm, with taper on the cut edge (kerf is wider at the entry side). Design slots, not tight holes, for adjustability.

Practical approach for a hybrid build like a CNC PCB drilling machine: machine or ream the features that define motion (bearing bores, shaft seats), print the features that define shape (covers, brackets, cable guides). Never ask a printed bore to be a bearing seat without post-machining — and if you must, print it 0.5 mm undersize and ream to H7.

Tolerance stacking: why assemblies drift

Parts do not add up at nominal — they add up at their limits. Two ways to estimate the stack:

Worst-case (arithmetic) stacking adds the tolerances directly. Three plates, each 10 ±0.1 mm, stacked: total = 30 ±0.3 mm. Guaranteed but pessimistic — it assumes every part lands at its worst limit simultaneously, which almost never happens.

Statistical (RSS) stacking assumes normal variation and adds the squares: total tolerance = √(0.1² + 0.1² + 0.1²) ≈ ±0.17 mm. More realistic for batches of parts, but it is a probability statement, not a guarantee — roughly 0.3% of assemblies can still exceed it if the process is truly normal.

For one-off student builds, worst-case is the honest method: you are making one of each part, and "statistically it should fit" is cold comfort at midnight. Design the stack so the worst case still assembles — or add one adjustable element (a slotted hole, a shim pack, a threaded adjuster) that absorbs the variation. Every experienced designer hides one "fudge" feature per assembly; the skill is hiding it where it does not compromise function.

Writing tolerances on a drawing (so the machinist gets it right)

On a dimension, write the fit directly: Ø25 H7 for the hole, Ø25 g6 for the shaft. In the title block, add a general tolerance note for everything not explicitly toleranced — the ISO 2768 medium class note ("ISO 2768-mK") is the standard shorthand: it assigns ±0.1–0.3 mm-class tolerances by size range to all unmarked dimensions, so your drawing is fully defined without cluttering every dimension.

If you model in Fusion 360, the companion CAD-to-prototype guide walks through taking a model to a physical part; when you export the 2D drawing from it, annotate the critical fits (bearing bores, shaft seats, sliding interfaces) with their ISO designations and let the general-tolerance note cover the rest.

Three drawing habits that prevent workshop arguments:

1. Dimension the feature the function needs. A hole that locates a bearing gets its diameter toleranced; a hole that just passes a bolt gets a loose limit or nothing.
2. Never tolerance the same feature twice (e.g. an overall length plus every segment) — the drawing becomes over-constrained and contradictory. Chain-dimension only where the stack allows it.
3. Add surface finish notes where motion happens (e.g. "Ra 1.6" on a sliding shaft). A dimensionally perfect shaft with a rough-turned finish will still gall and seize — tolerance without finish control is half a specification.

Inspection checklist before assembly day

• Every mating pair on the drawing has an explicit fit designation (H7/g6 etc.), not just a nominal size.
• All other dimensions fall under the title-block general tolerance note.
• You own (or can borrow) a measuring tool with ~1/10 the resolution of your tightest tolerance.
• Bearing seats are specified to bearing-fit practice (k6/m6 shaft, H7 housing — or the bearing maker's table), not guessed.
• Printed parts that mate with machined parts have post-machining allowance or clearance designed in.
• The tolerance stack has been checked worst-case, with one adjustable feature per critical assembly.
• Press-fit parts have a chamfered lead-in and an assembly method (press/vice/thermal) decided in advance.

Common tolerance mistakes, diagnosed

Symptom	Likely cause	Fix
Shaft will not enter hole though both "measure right"	Both made to nominal with no clearance designed in; measurement error ate the margin	Redesign as H7/g6 or similar; open the hole by the needed clearance
Sliding joint binds after working initially	Transition fit chosen where clearance was needed; thermal expansion or a burr closed the gap	Switch to a true clearance fit; deburr and check finish
Press-fit bushing spins in the housing	Clearance or transition fit used where interference was needed	Re-specify as H7/p6; check the housing bore was actually round
Parts fit individually but the assembly is skewed	Tolerance stack not checked; errors accumulated across the chain	Worst-case stack analysis; add a slotted/adjustable feature
Machinist quotes an absurd price or lead time	Unnecessarily tight tolerances (IT6 where IT11 would do) on non-critical features	Loosen everything non-functional; keep tight tolerances only on mating features
3D-printed bearing bore is loose/sloppy	Printed bore oversize and out-of-round; no finishing allowance	Print undersize and ream to H7, or design a machined insert
Dowel pins fall out / will not go in	Hole not reamed to the pin's specified fit (pins are usually m6)	Ream dowel holes to H7 and use the specified pin tolerance

Putting it together

Tolerances and fits are a language for negotiating between the ideal geometry in your CAD model and the imperfect geometry your processes produce. Learn to read H7/g6 the way you read a sentence, match the fit to the function, measure with a tool worthy of the tolerance, and check the stack before you cut metal. Do that, and assembly day becomes the satisfying part of the project — the part where everything slides, seats, and spins exactly as drawn. For the measurement and debugging side of getting physical builds right, the test-and-debug guide covers the systematic approach that catches fit problems before they become demo-day problems.