What Is a Machining Tolerance Table【General Tolerance · Fits · IT Grades Explained】

A "tolerance" is the allowable variation of a dimension from the value stated on the drawing (the difference between the maximum and minimum permitted sizes). On the shop floor, whether you can hold a tolerance governs quality, inspection, and cost alike — too tight and machining cost soars, too loose and parts won't assemble. Choosing the right tolerance is the heart of both design and machining. This article covers terminology, general tolerances (JIS B 0405), fits, IT grades, accuracy by machining method, and how to read a drawing — with worked examples.

Basic tolerance terms

• Nominal (basic) size: the reference dimension stated on the drawing.
• Upper / lower deviation: the allowed amount on the plus and minus side of the nominal size.
• Maximum / minimum limit of size: the nominal size plus the upper/lower deviation.
• Tolerance: max limit − min limit = upper deviation − (lower deviation) = the width of allowed variation.
• Example: φ20 +0.02 / −0.01 → max 20.02, min 19.99, tolerance 0.03.

A tolerance is always a positive "width" with no direction. It's the deviations that carry direction.

Why tolerances exist (accuracy vs. cost)

Nothing can be machined perfectly; there is always variation. A tolerance is the agreement on "how much variation is still functionally OK."

As a rule, halving a tolerance sharply increases machining cost (extra operations, tighter inspection, higher scrap). So the practical rule is to tighten only the dimensions that affect function and roll everything else into the general tolerance. "Tighten it all to be safe" is the most wasteful pattern there is.

General tolerances (JIS B 0405-1991)

These deviations apply collectively to dimensions with no individual tolerance. The grade (f/m/c/v) is stated in the title block or a note as "JIS B 0405-m". The grades are f = fine, m = medium, c = coarse, v = very coarse — and medium (m) is by far the most common.

Permissible deviations for linear dimensions except chamfers (unit: mm, ±)

Nominal size range	f Fine	m Medium	c Coarse	v Very coarse
0.5 up to 3	0.05	0.1	0.2	−
Over 3 up to 6	0.05	0.1	0.3	0.5
Over 6 up to 30	0.1	0.2	0.5	1.0
Over 30 up to 120	0.15	0.3	0.8	1.5
Over 120 up to 400	0.2	0.5	1.2	2.5
Over 400 up to 1000	0.3	0.8	2.0	4.0
Over 1000 up to 2000	0.5	1.2	3.0	6.0
Over 2000 up to 4000	−	2.0	4.0	8.0

※ For nominal sizes below 0.5 mm, state the deviation individually next to that dimension.

Permissible deviations for chamfers (corner radii / chamfer heights) — unit: mm, ±

Nominal size range	f·m (fine, medium)	c·v (coarse, very coarse)
0.5 up to 3	0.2	0.4
Over 3 up to 6	0.5	1
Over 6	1	2

Permissible deviations for angular dimensions (by length of the shorter side)

Length range of the shorter side	f·m	c Coarse	v Very coarse
Up to 10	±1°	±1°30′	±3°
Over 10 up to 50	±30′	±1°	±2°
Over 50 up to 120	±20′	±30′	±1°
Over 120 up to 400	±10′	±15′	±30′
Over 400	±5′	±10′	±20′

Fits (hole and shaft combinations)

The size difference between hole and shaft decides whether you get clearance or interference.

Type	State	Use
Clearance fit	Always has clearance	Shafts that rotate/slide smoothly
Transition fit	May be clearance or interference	Location, light press
Interference fit	Always has interference	Fixing, press-fit, anti-rotation

• Hole basis (H): fix the hole at H and adjust with the shaft symbol. Because hole diameters are easily standardized by drill/reamer, hole basis is the common choice.
• Shaft basis (h): fix the shaft at h and adjust on the hole side. Handy when using off-the-shelf shafts (ground round bar, etc.).

Common fits quick table (hole basis H7)

Combination	Type	Guide / use
H7 / g6	Clearance	Light slide. Plain bearings, locating pins
H7 / h6	Clearance (min clearance 0)	Push/pull by hand, guiding
H7 / js6	Transition	Hand-assembled without play
H7 / k6	Transition	Light press, keyed location
H7 / m6	Transition	Firmer press
H7 / p6	Interference	Press-fit, non-removable joint

※ The exact deviations (μm) are defined per size range in JIS B 0401. Always check the numeric table when designing.

IT basic tolerance grades

They run from IT01 to IT18; a smaller number means higher accuracy (smaller tolerance). For the same IT grade, a larger nominal size gives a wider deviation. The number in a fit symbol (H7, g6...) is this IT grade.

Achievable accuracy by machining method

Method	Achievable IT grade (guide)	Surface roughness Ra (guide, μm)
Turning · milling (general)	IT9–IT11	1.6–6.3
Precision turning · CNC milling	IT7–IT9	0.8–3.2
Reaming (finish)	IT7–IT8	0.8–1.6
Grinding (cylindrical · surface)	IT5–IT7	0.2–0.8
Lapping · superfinishing	IT3–IT5	0.05–0.2

※ Guideline values that vary with machine/tool/material/conditions. Use them to check process consistency — don't chase a grinding-level tolerance on a lathe.

How to read tolerances on a drawing

• ± form: 50±0.1 → 49.9–50.1.
• Separate upper/lower: φ20 +0.02 / 0 → 20.00–20.02.
• Fit symbol: φ20 H7 → hole tolerance class H7. φ20 H7/g6 specifies the combination.
• Dimensions with no tolerance: the general tolerance (JIS B 0405 grade) from the title block applies.
• Geometric tolerances (straightness, flatness, perpendicularity...) use separate symbols; if none is given, the JIS B 0419 general geometric tolerances apply.

Try the math (examples)

Ex. 1 — general tolerance (grade m): nominal 45 mm, grade m → range "30–120" is ±0.3. Allowed range 44.7–45.3 mm.

Ex. 2 — chamfer: a C2 chamfer, grade m → the "3–6" chamfer deviation is ±0.5 → 1.5–2.5 mm is acceptable.

Ex. 3 — fit clearance: for φ20 H7/g6, hole H7 = 20.000–20.021, shaft g6 = 19.980–19.993 (JIS B 0401 values). Minimum clearance 0.007, maximum 0.041 mm → a smooth-rotating, lubricated design.

Common mistakes

• Forgetting general tolerances and reading "no tolerance = anything goes."
• Mixing up hole basis (H) and shaft basis (h).
• IT grade not matching the machining method (chasing a grinding tolerance on a lathe).
• Overlooking that chamfers and angles also carry general tolerances.
• Tightening non-critical features and inflating cost.

Frequently asked questions (FAQ)

Q. What about a dimension with no tolerance? A. The general tolerance (JIS B 0405 grade) in the title block applies. If no grade is stated, confirm with the customer.

Q. What do H7 and g6 mean? A. The letter is the position of the tolerance zone, the number is the IT grade (tolerance size). Uppercase = hole, lowercase = shaft.

Q. Which general-tolerance grade should I pick? A. Medium (m) for typical parts. Use coarse (c) for cosmetic/non-functional features to cut cost; reserve fine (f) for precision parts.

Q. Is a tighter tolerance always better? A. No. Tighter means higher machining and inspection cost. Specify only as tight as the function requires.

Q. Are ±0.1 and +0.2/0 the same? A. Both have a 0.2 tolerance width, but the target center differs. The first centers on the nominal size; the second biases to the plus side.

Q. Are general tolerances and geometric tolerances different? A. Yes. Dimensional general tolerances are JIS B 0405; general geometric (form/orientation) tolerances are JIS B 0419.

Summary

A tolerance is the agreement on "how much variation we allow." Use general tolerances (JIS B 0405) to cover the whole part, specify individual tolerances or fits only where function demands, and pick a grade that matches the machining method — that's how you balance cost and quality. Always verify values against the latest JIS standard.

Sontis Management centralizes materials, dimensions, and machining conditions and links quoting, orders, and inspection. Try it now on the free plan.