Dimensioning rules, size tolerances, fits, general tolerances, and how to dimension to avoid tolerance accumulation. 17 terms. For each term: meaning, how to show it on a drawing, an example, common mistakes, and JIS vs. ASME differences.
The width of variation allowed in a size such as length or diameter; the difference between the upper and lower limits of size. In the 2016 JIS revision the name changed from "dimensional tolerance" (sunpo kosa) to "size tolerance".[1][2][3]
Three ways to write a size tolerance: add deviations to the nominal size, write the limits of size, or write a tolerance class (such as H7). With 50±0.1, 49.9–50.1 passes.
How to write it on the drawing
Write with deviationsFollow the nominal size with the upper and lower deviations (e.g., 50 +0.1/0).[4]
Write limits of sizeWrite the maximum and minimum sizes one above the other.[4]
Write a tolerance classWrite a tolerance class symbol, as in φ20H7.[4][5]
ExampleWith 50±0.3, anything from 49.7 mm to 50.3 mm passes.[2]
Common mistakes
Thinking a size tolerance also controls form and positionWhy: size tolerances in ISO and JIS control only the length between two points, not bending, tilt, or position error (principle of independency).Fix: if form, orientation, or position matter functionally, also specify geometrical tolerances.[1][6][7]
JIS and ASMEIn ASME Y14.5, the size tolerance of a feature of size also controls form by default (Rule #1, the envelope principle). ISO and JIS do not.[12][6][13]
Standard: JIS B 0401-1:2016 (basics of size tolerances and fits); indication methods in JIS B 0420-1:2016 and JIS Z 8318. ISO 286-1, ISO 14405-1.[8][9][10][11]
The size value written on the drawing, from which deviations are measured. The 2016 revision of JIS B 0401 changed "basic size" (kijun sunpo) to "nominal size" (zushi saizu).[1][2]
Nominal size: the size value written on the drawing (the 20 in φ20H7). The deviations are determined relative to this value.
How to write it on the drawing
Write as the reference for the deviationsFollow the nominal size with deviations or a tolerance class (e.g., 50 +0.1/0, φ20H7).[4][5]
ExampleThe "20" in φ20H7 is the nominal size.(An example built from the rules in the sources)[1][5]
Common mistakes
Assuming the nominal size is the target value for machiningWhy: with a unilateral tolerance (e.g., 50 +0.2/0), exactly the nominal size is at the edge of the allowed range.Fix: look at the tolerance zone and choose an easy-to-machine target, such as near the middle.[13][2]
JIS and ASMEASME Y14.5-2018 added an explicit rule that "the value shown does not imply a functional or manufacturing target" (4.1(q)).[13]
Limits of size and deviationskyoyo genkai saizu to kyoyosalimits of size / upper deviation / lower deviation
Limits of size are the maximum and minimum sizes allowed (upper and lower limits of size); deviations are the differences between those and the nominal size (upper and lower deviations). The 2016 revision renamed terms such as "maximum allowable dimension" and "upper dimensional deviation".[1][2][3]
A deviation is "the difference from the nominal size"; a limit of size is "the maximum or minimum size itself". 50 +0.2/0 and 50.2/50.0 mean the same range.
How to write it on the drawing
Three ways to write itWrite nominal size + deviations, limits of size (maximum and minimum), or nominal size + a tolerance class symbol.[4]
Showing both in the assembled stateAnother method is to write both parts' deviations or fit symbols side by side on a drawing of the two mating parts assembled.[4]
Make numbers large and clearOn the shop floor, drawings get oily or folded, so write deviations and fit symbols large enough that they cannot be misread.[4]
Common mistakes
Cramming deviations in small charactersWhy: dirt and fold lines cause misreading.Fix: write deviations and fit symbols clearly and large.[4]
JIS and ASMEUS teaching materials introduce distinctions such as limit dimensioning with a limit on one side only (MIN, MAX), and bilateral tolerances that are equal or unequal.[3]
Standard: JIS Z 8318 (Indication of limits for linear and angular dimensions), JIS B 0401-1:2016.[10][8][4]
A bilateral tolerance allows variation on both sides of the nominal size (such as ±0.1); a unilateral tolerance allows it in one direction only (such as +0.2/0).[3][14]
A bilateral tolerance allows variation both above and below the nominal size (±0.1); a unilateral tolerance allows it on one side only (+0.2/0). When they differ, write the upper deviation on top and the lower deviation below.
How to write it on the drawing
How to write upper and lower deviationsCombine equal bilateral tolerances as ±0.1; for unequal bilateral or unilateral tolerances, write the upper deviation above the lower deviation.[3][4]
Common mistakes
Specifying ± when function allows variation on only one sideWhy: holes or clearances vary toward the tight side, and parts cannot be assembled.Fix: consider the function and give tolerance only on the allowed side (for a first-of-a-kind research apparatus, for example, confirm in a meeting).[14]
Standard tolerance grade (IT grade)kihon saizu kosa tokyustandard tolerance grade / IT grade
Tolerance magnitudes defined by grade for each size range. The smaller the grade number, the more precise. The 2016 JIS revision renamed "tolerance grade" (kosa tokyu) to "standard tolerance grade".[15][1]
Standard tolerance grade (IT grade): the number that expresses the size of the tolerance. For the same nominal size, the smaller the number, the smaller the tolerance and the more precise.
How to write it on the drawing
Typical usesMisumi's explanation says IT01–IT4 are mainly used for precision parts such as gauges, IT5–IT10 for fits in general machinery, and IT11–IT16 for parts without fits.[15]
Standard: JIS B 0401-1:2016, ISO 286-1:2010.[8][11]
A position symbol for the tolerance (capital for holes, lowercase for shafts) combined with the standard tolerance grade number (H7, g6, etc.). Renamed in the 2016 revision from "tolerance zone class" (kosa-iki kurasu).[15][1][5]
Tolerance class: a position symbol (capital for holes, lowercase for shafts) combined with a tolerance grade number (H7, g6, etc.). Written after the nominal size.
How to write it on the drawing
Write after the nominal sizeWrite as φ20H7, φ20g6.[5][4]
Order of symbolsFor holes there are 28 symbols from A to ZC: the closer to A, the larger the hole, and at H the lower deviation is 0. For shafts, a to zc: the closer to a, the smaller the shaft, and at h the upper deviation is 0.[15]
ExampleIf a φ10 hole for a bearing is H7 and the bearing side that fits in it is h6, the nominal size of both is 10, and the symbols set each deviation.[5]
Common mistakes
Mixing up capital and lowercase lettersWhy: H7 (hole) and h7 (shaft) have deviations in completely different directions.Fix: make it a rule that holes are capital and shafts lowercase, and write them so they are distinguishable.[15][5]
Fit systems (hole basis and shaft basis)hameai hoshikihole-basis fit system / shaft-basis fit system
A system for choosing which of the mating hole and shaft is the basis for combining tolerance classes. Fixing the hole at H and varying the degree of fit on the shaft side is the hole-basis fit system, which is generally the one used.[16][2][1]
Hole-basis fit system: fix the hole at H7 and change the tolerance class of the mating shaft (g6, k6, p6, etc.) to set the degree of clearance or interference.
How to write it on the drawing
Choose from the recommended tableChoose from the recommended table in JIS B 0401-1 (e.g., for H7: f6, g6, h6, js6, k6, m6, n6, p6, r6, s6, etc.).[16]
Start with the colored preferred classesFor your first choice, pick from the tolerance classes highlighted in the recommended table.[16]
Common mistakes
Using shaft-basis for no reasonWhy: holes are generally harder to machine than shafts, so it is easier to handle if the hole is common.Fix: unless there is a special reason, choose hole-basis.[2][16]
Standard: JIS B 0401-1:2016 (ISO fit system).[8][16]
Clearance, transition and interference fitssukimabame, chukanbame, shimaribameclearance fit / transition fit / interference fit
Classification by the condition when hole and shaft are assembled. A clearance fit always has clearance, a transition fit can have either clearance or interference, and an interference fit always has interference.[17][16][5]
With an H7 hole, a g6 shaft always has clearance (clearance fit), k6 can have either clearance or interference (transition fit), and p6 always has interference (interference fit).
How to write it on the drawing
How to write it in the assembled stateOn an assembly drawing, the tolerance classes of the mating hole and shaft can be written side by side.[4]
ExampleWith an H7 hole, g6 is a clearance fit, k6 a transition fit, and p6 an interference fit (recommended table in JIS B 0401-1).[16]
Common mistakes
Using an interference fit at a point that gets disassembledWhy: it becomes hard to disassemble without damaging the parts.Fix: for places that will be disassembled or replaced, choose a combination that can be disassembled and assembled without damaging the parts.[17]
General tolerancesfutsu kosageneral tolerances / ISO 2768-1
Tolerances applied collectively to length and angle dimensions that do not have individual tolerances. There are 4 grades, fine f, medium m, coarse c, and very coarse v, and the deviations are set for each dimension range.[18][2][19][14]
General tolerances: for dimensions without individual tolerances, state the standard and grade, such as "JIS B 0405-m", in a field near the title block to set tolerances all at once.
How to write it on the drawing
Specify in one place in the general tolerance field of the drawing frameIn the general tolerance field near the title block, state the standard and grade that apply, and omit individual tolerances on each dimension.[20][2]
Separate tables for chamfers and anglesChamfer lengths (broken edges: external radii and chamfer heights) and angles have separate deviation tables.[18]
ExampleFor medium m, a length of 50 mm (over 30 up to 120) is ±0.3, and a length of 200 mm (over 120 up to 400) is ±0.5.(An example built from the rules in the sources)[18]
Common mistakes
Applying general tolerances to dimensions under 0.5 mmWhy: the table covers 0.5 mm and above; anything smaller is outside its scope.Fix: write the deviation individually for dimensions under 0.5 mm.[18]
Writing both of two dimensions that conflict under the general tolerancesWhy: general tolerances also apply to dimensions that can be calculated, so they do not add up.Fix: make the conflicting one a reference dimension.[14]
JIS and ASMEUS teaching materials introduce a method where a tolerance block near the title block sets the tolerance by number of decimal places. JIS uses a table of dimension ranges and grades.[23][18]
Standard: JIS B 0405:1991 (its English title is the same as ISO 2768-1). Metal stampings: JIS B 0408; sheared metal sheet: JIS B 0410.[21][22][18]
General geometrical tolerancesfutsu kika kosageneral geometrical tolerances
Geometrical tolerances applied collectively to features without individual geometrical tolerances. There are 3 grades, H, K, and L, and the tables set values for straightness/flatness, perpendicularity, symmetry, and circular runout.[24][19]
General geometrical tolerances: writing "JIS B 0419-mK" applies medium m to lengths and angles and grade K to geometrical tolerances all at once.
How to write it on the drawing
Specify the grade in one place in the drawing frameAs with general tolerances, state the grade that applies to the whole drawing in one place.[19]
How datums are taken is fixedFor perpendicularity, the longer side is the datum; for circular runout, the specified supporting surface is the datum (if none, the longer feature).[24]
ExampleAt grade K, flatness of a 200 mm face is 0.4 mm, perpendicularity with an 80 mm shorter side is 0.4 mm, and circular runout is 0.2 mm.(An example built from the rules in the sources)[24]
Common mistakes
Thinking roundness and cylindricity can also be looked up in the tableWhy: roundness is the same value as the diameter's size tolerance (but not more than the general circular runout tolerance), and cylindricity and coaxiality are not specified.Fix: specify geometrical tolerances individually for features that matter functionally.[24]
Standard: JIS B 0419:1991. The corresponding ISO 2768-2 has been withdrawn (shown as Withdrawn on the ISO standard page).[25][26]
Independency principledokuritsu no gensokuprinciple of independency / independency principle
The idea that the size tolerance and geometrical tolerance written on a drawing are unrelated unless otherwise specified, and each is a separate requirement to be met. Adopted by ISO (1985) and JIS (1988).[1][12][6]
How to write it on the drawing
Add geometrical tolerances to control formSize tolerance alone does not control bending or waviness, so specify the form tolerance needed.[1][6]
Use Ⓔ to link size and formAdd the envelope requirement Ⓔ after the size tolerance.[6][27]
ExampleIf only a size tolerance is given on a φ30 shaft, it passes as to size even if somewhat bent, as long as the two-point diameter is within tolerance in every cross-section.(An example built from the rules in the sources)[1][12]
Common mistakes
Reading an ASME drawing with ISO/JIS assumptionsWhy: in ASME the size tolerance also controls form (Rule #1), so the same indication can give a different pass/fail result.Fix: first confirm which standard the customer's drawing is based on.[1][6][13]
JIS and ASMEASME Y14.5 makes the envelope principle (Rule #1) the default and uses a symbol for independency when wanted (adopted in the 2009 edition). ISO and JIS make independency the default and add Ⓔ when a link is wanted.[12][6][13]
Standard: JIS B 0024:2019 (5.5 "Principle of independency"; adopted from ISO 8015:2011 with modifications).[28][29]
ⒺEnvelope requirementhoraku no jokenenvelope requirement
A condition that a feature of size must not exceed the perfect-form envelope at maximum material size. In ISO and JIS it is specified by adding Ⓔ after the size tolerance.[27][6][30]
How to write it on the drawing
Ⓔ after the size toleranceExample: φ30±0.1 Ⓔ.[6][27]
Applies to a single feature of sizeUsed for a single feature of size defined by a cylindrical surface or two opposite parallel planes.[27]
ExampleShaft φ20 0/−0.1 Ⓔ: the whole shaft must fit in a perfect cylinder (a gauge hole) of φ20.0. If the shaft is bent, the diameter must be made smaller by that amount.(An example built from the rules in the sources)[27]
Common mistakes
Reading an ASME drawing without Ⓔ as meaning form is freeWhy: in ASME the envelope principle applies by default even without a symbol.Fix: read ASME drawings assuming Rule #1.[6][12]
JIS and ASMEASME makes envelope the default and uses no symbol. ISO and JIS add Ⓔ only when needed. Mitutoyo America says "use Ⓔ in ISO when you want to control the fit with the mating part".[6][12][13]
Standard: Ⓔ is referenced to JIS B 0024 in the supplementary symbol table of JIS B 0021. Size specification is in JIS B 0420-1 (based on ISO 14405-1).[31][9]
Two-point sizenitenkan saizutwo-point size / local size
A size obtained as the distance between two opposite points of a feature. In ISO and JIS, unless otherwise specified, size tolerances on lengths are judged by this two-point size.[9][12][13][1]
How to write it on the drawing
Specify other evaluation methodsTo judge by other methods such as least-squares size, maximum inscribed size, or minimum circumscribed size, state it explicitly using the methods of JIS B 0420-1.[9]
Common mistakes
Assuming a part that passes with calipers also passes on formWhy: two-point measurement misses bending and cross-section distortion.Fix: if form matters, specify a geometrical tolerance and inspect with a suitable measuring instrument.[1][32]
JIS and ASMEIn ASME Y14.5, a size tolerance controls both the fit with the mating part (actual mating size) and local size. ISO, unless otherwise specified, uses only the two-point size.[13]
Standard: JIS B 0420-1:2016 (based on ISO 14405-1:2010).[9]
A feature defined by a size such as a diameter or width, like a cylinder, sphere, or two opposite parallel planes. When the size changes, the size of the feature changes.[27][9]
How to write it on the drawing
Where the leader touches changes the targetIf the arrow of the tolerance frame is placed on the extension of the dimension line, the target is the center line or center plane (derived feature); if offset from the dimension line and placed on the surface, the target is the surface (integral feature).[27][33][34]
JIS and ASMEIn ASME, Rule #1 (envelope principle) applies to a feature of size.[12]
Standard: scope of JIS B 0420-1:2016 (cylinders and two opposite parallel planes).[9]
Tolerance accumulationkosa no ruisekitolerance stack-up / tolerance accumulation
When dimensions are chained one after another to locate something, each tolerance adds up, and the variation in the position of features far apart grows.[35][3]
Tolerance accumulation: chaining three ±0.1 dimensions gives variation up to ±0.3 between the two ends. For important distances, dimension directly from a datum.
How to write it on the drawing
Dimensioning to avoid accumulationPut functionally important distances directly from a common datum (parallel dimensioning), or specify them with TEDs (theoretically exact dimensions) and a position tolerance.[35][36][5]
ExampleIn Keyence's example, if hole positions are set by chaining size tolerances, the distance between the holes is up to 45.3 mm; if set with TED and position tolerance, it is up to 45.1 mm.[35]
Common mistakes
Chaining important positional relationships in chain dimensionsWhy: tolerances accumulate, and parts do not fit at assembly.Fix: specify important positions directly from a common datum, or with TED and position tolerance.[35][3]
Standard: dimension arrangement is in section 8 of JIS Z 8317-1:2008 (parallel, progressive, chain, coordinate, combined).[37]
The idea that the maximum-material side should be checked with a GO gauge that checks the whole feature at once, and the least-material side with a NO-GO gauge that checks elements individually. It began with inspecting threaded fits.[19][12]1 source (for reference)
Standard: no JIS that defines only this principle could be confirmed in this research.
A group of ISO standards (ISO/TC 213) for specifying requirements such as form, size, and position on drawings without ambiguity and for systematically aligning how they are verified. JIS also maintains its standards for size tolerance, geometrical tolerance, and surface texture as GPS.[19][28][1]
Standard: the fundamental principles are in JIS B 0024:2019 (adopted from ISO 8015:2011 with modifications).[28][29]
Explanations without a mark are those on which two or more sources from different publishers agree. Because the text of the standards is paid, they were checked against technical materials from measuring-instrument and parts manufacturers, teaching materials from universities and public testing institutes, and public pages of the standards, and the explanations are written in Kezuriba's own words. The diagrams of the entry fields were drawn by Kezuriba.