The 14 geometric characteristics, feature control frame, datums, maximum material requirement, projected tolerance zone, common tolerance zone and TED. 46 terms. For each term: meaning, how to show it on a drawing, examples, common mistakes, and differences between JIS and ASME.
A tolerance that specifies, by symbol and numeric value, the allowed range of deviation (tolerance zone) in form (straightness, flatness, roundness), orientation (parallelism, perpendicularity, angularity), position and run-out. It can convey design intent that size tolerances cannot.[1][2][3][4]
Geometric tolerances fall into four groups: form, orientation, location and run-out. Only form tolerances use no datum; for the others, the orientation or location of the tolerance zone is defined relative to datums.Example of a feature control frame
How to write it on the drawing
Specify with a feature control frameWrite the geometric characteristic symbol, tolerance value and datums in the frame, and connect it to the target feature with a leader.[5][3]
Check whether a datum is requiredForm tolerances need no datum; orientation and run-out tolerances require one. For position, the table in JIS B 0021 says "required / not required".[6][2][7]
ExampleSpecifying parallelism on the top face of a plate as "∥ | 0.02 | A" (A = bottom face) lets you reject plates that are machined at a slant or warped, even if the thickness is within tolerance.(An example built from the rules in the sources)[1][4]
Common mistakes
Expecting parallelism or perpendicularity from size tolerances aloneWhy: a thickness tolerance alone does not guarantee that the top and bottom faces are parallel, and a slanted plate would still pass according to the drawing. KEYENCE says the responsibility lies with the designer's specification, not with the machining side.Fix: specify the form and orientation that the function needs with geometric tolerances.[1][4][2]
JIS and ASMEMost symbols are common to ISO, JIS and ASME, but ASME Y14.5-2018 dropped concentricity and symmetry. There are also ASME-only symbols, such as the unequally disposed profile Ⓤ and continuous feature CF.[12][3][13][14]
Standards: JIS B 0021:1998 (indication of form, orientation, location and run-out tolerances), with datums in JIS B 0022. The international standard is ISO 1101:2017 and the US standard is ASME Y14.5-2018.[8][9][10][11]
Tolerance indication frame (feature control frame)kosa kinyuwakufeature control frame / tolerance frame
A rectangular frame in which a geometric tolerance is written. From the left, it contains, separated by dividers, the geometric characteristic symbol, the tolerance value (preceded by φ or Sφ if needed), additional symbols, and datum letters.[5][2][3]
Read the frame from the left as "geometric characteristic | tolerance value and additional symbols | datums". A form tolerance has no datum compartment, so the frame has two compartments.Example of a feature control frame
How to write it on the drawing
Write in order from the left, separated by dividersThe first compartment holds the geometric characteristic symbol, the second the tolerance value (mm) and additional symbols (Ⓜ, Ⓛ, CZ, etc.), and the third onward the datum letters.[5][3]
Characteristics that need φAdd φ when the tolerance zone is a circle or cylinder. 2D circle: position, concentricity; 3D cylinder: straightness, parallelism, perpendicularity, angularity, position, coaxiality; sphere: position (Sφ).[5][7]
Datums from the left in order of precedenceArrange multiple datums from the left in descending order of precedence.[5][2]
Connect to the feature with a leaderDraw a leader from the end of the frame and put the arrow on the target. On the extension of the dimension line, the target is the center (axis or median plane); offset onto the outline, the target is the surface.[15][16][7]
ExampleExample "⌖ | φ0.05 Ⓜ | A | B | C": position, cylindrical tolerance zone of diameter 0.05, maximum material requirement, datums in the order A, B, C.(An example built from the rules in the sources)[5][2]
Common mistakes
Ordering datums arbitrarilyWhy: if the precedence changes, the way of measuring and the result change even for the same part.Fix: write them from the left in order of importance for function and assembly.[5][2]
JIS and ASMEIn ASME, the feature control frame has the same order (symbol, tolerance value, modifiers, datums).[3]
In geometric tolerancing, the region within which a feature must lie. Depending on the target and symbol, its shape is two parallel lines, two parallel planes, a circle, a cylinder, concentric circles, coaxial cylinders, a sphere, and so on.[6][7][2]
The shape of the tolerance zone is determined by the target (line, surface, axis, point), the symbol, and whether φ precedes the tolerance value. The width t of two parallel planes is taken in the direction of the leader arrow.
How to write it on the drawing
Tolerance zone of a pointFor a point, a circle (in a plane) or sphere centered on that point.[6][7]
Tolerance zone of a lineFor a straight line, two parallel planes spaced t/2 either side of it, or a cylinder of diameter t when φ is added.[6][2]
Specifying directionThe tolerance zone of two parallel planes has width t in the direction of the leader arrow.[17][7]
Standard: JIS B 0021:1998, clause 18 (definition of tolerance zones).[7][8]
Single features and related featurestandoku keitai / kanren keitaisingle feature / related feature
A feature whose tolerance is set by the feature alone, regardless of datums, is a single feature; a feature whose orientation, location or run-out tolerance is set in relation to a datum is a related feature.[6][2]
How to write it on the drawing
Difference in framesThe frame for a single feature has no datum compartment; the frame for a related feature does.[6][2][5]
Integral features and derived featuresgaikaku keitai / yudo keitaiintegral feature / derived feature
An integral feature is a feature with substance, such as a surface or a line on a surface; a derived feature is a center line, median plane or center point derived from an integral feature. Where the leader arrow of the frame is placed changes which one is controlled.[18][16][12]
Even with the same frame, the target changes with where the arrow is placed. On the outline, it is the surface (integral feature); in line with the dimension line, it is the axis or median plane (derived feature).
How to write it on the drawing
To indicate a surfacePlace the arrow on the outline (or its extension), offset from the dimension line.[19][16]
To indicate the centerPlace the arrow on the extension of the dimension line of the feature of size.[19][15]
Common mistakes
Putting the arrow on the surface when you want to control the axisWhy: the surface lines become the controlled target, and bending of the axis is not controlled.Fix: to control the center, put the arrow on the extension of the dimension line.[16][19]
Standard: feature terms are in JIS B 0672-1 (a normative reference of JIS B 0001).[20]
A tolerance that controls deviation in the form of a feature itself without using a datum. It comprises straightness, flatness, circularity and cylindricity, plus profile of a line and profile of a surface without datums.[15][2][7][3]
Form tolerances look only at the form of the feature itself, so the frame has no datum compartment (two compartments: "symbol | tolerance value").
How to write it on the drawing
Frame has no datum compartmentWrite it in two compartments: "symbol | tolerance value".[2][5]
Standards: JIS B 0021:1998, 18.1-18.5 and 18.7; ISO 1101.[7][8][9]
A tolerance that controls how far a feature may tilt from its intended orientation (parallel, perpendicular, at a set angle) relative to a datum. Parallelism, perpendicularity, angularity, and profile of a line or surface with datums.[17][2][7][3]
Orientation tolerances control only orientation (parallel, perpendicular, at a set angle) relative to a datum. Distance from the datum is set by size tolerances or location tolerances.
How to write it on the drawing
Frame has a datum compartmentWrite it as "symbol | tolerance value | datum", and attach a datum symbol to the reference surface or axis.[17][2]
Standards: JIS B 0021:1998, 18.6 and 18.8-18.11; ISO 1101.[7][8][9]
A tolerance that controls how far a feature may deviate from its true position, defined from datums by theoretically exact dimensions. Position, concentricity, coaxiality, symmetry, and profile of a line or surface with datums.[21][2][7][3]
Position tolerance limits deviation from the true position defined by the datums and TEDs. Keeping the feature inside the tolerance zone also limits its orientation error.
How to write it on the drawing
Location by TED, datums in the tolerance frameShow the theoretically exact location with TEDs and list the datums in the tolerance frame.[6][2]
Standards: JIS B 0021:1998 18.12–18.14, ISO 1101.[7][8][9]
Tolerance that limits how much a surface runs out when the part is rotated about a datum axis. There are circular runout and total runout. A datum is always required.[22][2][7][3]
Runout tolerance checks the runout of a surface when the part is rotated about the datum axis. A datum that serves as the rotation reference is always required.
How to write it on the drawing
Make the rotation reference the datumMake the part that serves as the rotation reference, such as a bearing seat, the datum (a common datum A-B if there is one at each end).[7][22]
Standards: JIS B 0021:1998 18.15–18.16, ISO 1101.[7][8][9]
Form tolerance that limits the deviation from straightness of a line element (a line on a surface, a cylinder generatrix, or an axis). No datum is used.[15][2][7][3]
Straightness of an axis (with φ): the actual axis only has to lie inside a cylinder of diameter t. If the arrow is placed on the outline without φ, the surface line must lie between two parallel lines t apart.Example of a feature control frame
How to write it on the drawing
Tolerance frame"⏤|tolerance value". There is no datum field.[5][2]
To control a line on the surfaceOffset the arrow from the dimension line and place it on the outline. The tolerance zone is two parallel lines in the specified direction (two parallel planes for a cylinder generatrix).[7][19]
To control an axisPlace the arrow on the extension of the diameter dimension line and put φ before the tolerance value. The tolerance zone is a cylinder of diameter t.[15][2][7]
ExampleAttach "⏤|φ0.1" to the diameter dimension of a φ20 shaft, and the axis must lie inside a cylinder of diameter 0.1 mm.(An example built from the rules in the sources)[15][2]
Common mistakes
Putting the arrow on the surface when you want to control the axisWhy: It becomes straightness of a generatrix, and bending of the axis is not controlled.Fix: For an axis, place the arrow on the extension of the dimension line and add φ.[16][15][7]
Using the height gauge reading directly as straightnessWhy: The value changes with the tilt of the workpiece and the contact force, so it is unstable.Fix: Level both ends to remove the tilt before reading, or use a coordinate measuring machine (CMM).[23]
JIS and ASMEASME also distinguishes straightness of a surface from straightness of an axis. In ASME, straightness of a surface of a feature of size is also controlled by the size tolerance through Rule #1.[3][13]
Standards: JIS B 0021:1998 18.1, ISO 1101.[7][8][9]
Form tolerance that limits deviation from flatness of a plane. The whole surface must lie between two parallel planes a distance t apart.[15][2][7][3]
Flatness: the whole surface only has to lie between two parallel planes a distance t apart. The planes may be tilted freely (they need not be parallel to a datum).Example of a feature control frame
How to write it on the drawing
Tolerance frame"⏥|tolerance value". Place the arrow on the outline of the target surface (or its extension).[2][15]
Several separate surfaces in one tolerance zoneFor several surfaces that must lie in the same plane, add CZ after the tolerance value.[2]
Example"⏥|0.08": the surface must lie between two parallel planes 0.08 mm apart.[7]
Common mistakes
Giving only flatness when parallelism to a mating surface is neededWhy: Flatness has no datum, so parallelism to a reference surface is not controlled.Fix: If parallelism to a reference surface is needed, specify parallelism.[17][3]
Measuring by moving a dial indicator by handWhy: The measuring points change with how it is moved, so the value is not repeatable.Fix: Fix the measuring points on a surface plate, or use a CMM.[24][2]
JIS and ASMEIn ASME, the flatness of a surface of a feature of size, such as plate thickness, is automatically controlled within the size tolerance by Rule #1. In KEYENCE's example, flatness stays at the indicated value under ISO, while under ASME the maximum material boundary takes precedence. US teaching materials also say the flatness value should be smaller than the related size tolerance.[13][3]
Standards: JIS B 0021:1998 18.2, ISO 1101.[7][8][9]
Form tolerance that limits roundness: in any cross section of a shaft, hole, cone, etc., the outline must lie between two concentric circles whose radii differ by t.[15][2][7][3]
Circularity: in each cross section perpendicular to the axis, the outline only has to lie between concentric circles with radial difference t. The center of the circles can be placed freely for each section. Taper and barrel shape are not checked by circularity.
How to write it on the drawing
Tolerance frame"○|tolerance value". Place the arrow on the surface of the cylinder or cone.[2][15]
The tolerance zone applies per cross sectionCheck whether the outline lies between concentric circles with radial difference t in any section perpendicular to the axis.[7][2]
ExampleCircularity 0.02 on a φ55±0.2 cylinder: the diameter is within 54.8–55.2 and the roundness of each section is within 0.02. Even if the cylinder is tapered or barrel-shaped, that is not controlled by circularity.[2]
Common mistakes
Determining circularity from two-point micrometer measurementsWhy: Two-point measurement cannot capture roundness correctly, so accuracy is limited.Fix: Evaluate with a roundness measuring machine or a CMM.[25][2]
Assuming circularity also guarantees the shape along the axisWhy: Circularity covers only the roundness of each section and does not control taper or barrel shape.Fix: Use cylindricity to include the axial direction.[2]
JIS and ASMEASME calls it circularity (also roundness); the concept is the same.[3]
Standards: JIS B 0021:1998 18.3, ISO 1101.[7][8][9]
Form tolerance that controls the roundness and straightness of a cylindrical surface together. The whole surface must lie between two coaxial cylinders whose radii differ by t.[15][2][7][3]
Cylindricity: the whole cylindrical surface only has to lie between two coaxial cylinders with radial difference t. It controls roundness (circularity) and straightness (of the generatrix) together.Example of a feature control frame
How to write it on the drawing
Tolerance frame"⌭|tolerance value". Place the arrow on the outline of the cylindrical surface. No datum is used.[2][15]
Example"⌭|0.1": the cylindrical surface must lie between two coaxial cylinders 0.1 mm apart in radius.[7][15]
Common mistakes
Trying to verify a tight cylindricity with a general-purpose CMMWhy: Mitutoyo's material says it is difficult to evaluate products with tolerances of 0.01 mm or less on a general-purpose CMM.Fix: Set tight tolerances on the assumption that they will be inspected on a roundness/cylindrical form measuring machine.[2][26]
Standards: JIS B 0021:1998 18.4, ISO 1101.[7][8][9]
⌒Profile of a linesen no rinkakudoprofile of a line / line profile
Tolerance that controls, as a line in each cross section, how closely a curved outline follows the shape defined by theoretically exact dimensions (TEDs). Without a datum it acts as a form tolerance; with datums it acts as an orientation/location tolerance.[27][2][7][3]
Profile of a line: the profile in each cross section only has to lie between the two envelopes formed by a circle of diameter t centered on the theoretical profile (chain line). To apply it all around the outline, add the all-around symbol (a small circle) at the bend of the leader line.Example of a feature control frame
How to write it on the drawing
Define the shape with TEDsShow the radii and positions of the profile with boxed TEDs.[2][7]
Tolerance zoneBetween the two envelopes formed by a circle of diameter t centered on the theoretical profile line (t/2 on each side).[27][2][7]
To apply it all aroundAdd a small circle (all-around symbol) at the bend of the leader line.[2][14]
Example"⌒|0.05" with the all-around symbol on the whole outline: the profile in each section lies within a band of ±0.025 on both sides of the theoretical shape.[2]
Common mistakes
Defining the profile with ordinary toleranced dimensions and then adding a profile toleranceWhy: The theoretical shape that serves as the reference for the profile tolerance is not defined.Fix: Write the dimensions that define the profile as TEDs (boxed).[2][7]
JIS and ASMETo shift the tolerance zone to one side of the theoretical profile, ISO and JIS use UZ and ASME uses Ⓤ.[13][14]
Standards: JIS B 0021:1998 18.5 and 18.6; dimensions and tolerances of profiles: JIS B 0027.[7][8][28]
⌓Profile of a surfacemen no rinkakudoprofile of a surface / surface profile
Tolerance that controls how closely a whole surface, such as a curved surface, follows the theoretical surface defined by TEDs. Without a datum it acts as a form tolerance; with datums it acts as an orientation/location tolerance.[27][2][7][3]
Profile of a surface: the whole surface only has to lie between the two envelope surfaces formed by a sphere of diameter t centered on the theoretical surface (the shape defined by TEDs). Because a datum is given, the location of the theoretical surface is also fixed from A.Example of a feature control frame
How to write it on the drawing
Define the shape with TEDsShow the shape and location of the theoretical surface with TEDs.[2][7]
Tolerance zoneBetween the two envelope surfaces formed by a sphere of diameter t centered on the theoretical surface.[27][7][2]
Example"⌓|0.1|A": the surface must lie between the two envelope surfaces formed by a sphere of diameter 0.1 centered on the theoretical surface, which is at its theoretically exact location relative to datum A.[7]
Common mistakes
Assuming profile of a line controls the whole surfaceWhy: Profile of a line looks only at the lines in each section parallel to the projection plane.Fix: Use profile of a surface to control the whole surface.[27][7]
JIS and ASMEASME Y14.5-2018 strengthens the idea of using profile also to control location, and reorganized profile, orientation, and form into separate sections.[11]
Standards: JIS B 0021:1998 18.7 and 18.8, JIS B 0027.[7][8][28]
Orientation tolerance that limits deviation from parallelism of a plane or a line (axis) to a datum.[17][2][7][3]
Parallelism: the surface the arrow points to only has to lie between two parallel planes that are parallel to datum A and t apart in the direction of the arrow. Whether the surface is warped or tilted, it is rejected if it does not fit within this width.Example of a feature control frame
How to write it on the drawing
Tolerance frame"∥|tolerance value|A". Add the datum symbol to the surface or axis used as the reference.[17][2]
Parallelism of an axisWith φ before the tolerance value, the tolerance zone is a cylinder of diameter t parallel to the datum.[2][7]
Example"∥|0.05|A": the surface the arrow points to must lie between two parallel planes parallel to datum plane A and 0.05 mm apart in the direction of the arrow.[17]
Common mistakes
Leaving out the datumWhy: What it is parallel to is undefined, so the callout is meaningless.Fix: Always specify a datum, and give the datum surface an accuracy suitable for a reference.[17][2]
Measuring a soft part by pressing on it with a probeWhy: Plastic and rubber deform under the probe force and cannot be measured correctly.Fix: Measure with a low-force method, or consider a free-state specification.[29]
Standards: JIS B 0021:1998 18.9, ISO 1101.[7][8][9]
Orientation tolerance that limits deviation from perpendicularity of a plane or line (axis) to a datum. The tolerance value is expressed as a length (mm), not an angle.[17][2][7][3]
Perpendicularity of an axis (with φ): the pin axis only has to lie inside a cylinder of diameter t perpendicular to datum A. Write the tolerance value as a length (mm), not an angle.Example of a feature control frame
Axis of a hole or shaftWith φ before the tolerance value, the tolerance zone is a cylinder of diameter t perpendicular to the datum.[2][7]
Example"⟂|φ0.1|A" on a hole axis: the hole axis must lie inside a cylinder of diameter 0.1 mm perpendicular to datum plane A.[7][2]
Common mistakes
Writing perpendicularity as an angle (°)Why: A perpendicularity tolerance is expressed as a length, and writing it as an angle makes no sense.Fix: Write the tolerance value in mm.[17]
Standards: JIS B 0021:1998 18.10, ISO 1101.[7][8][9]
Orientation tolerance that limits deviation of a surface or axis that should be inclined at a specified angle other than 90° to a datum. The angle is shown as a TED, and the tolerance value is given in mm.[17][2][7][3]
Angularity: the surface only has to lie between two parallel planes t apart that are inclined at the theoretically exact angle (the boxed 40°) to datum A. Do not add ± to the angle; give the variation in mm.Example of a feature control frame
How to write it on the drawing
Write the angle as a TED (boxed)Make the inclination angle a boxed, theoretically exact angle.[2][7]
Example"∠|0.08|A" with a TED of 40° on a surface: the surface must lie between two parallel planes 0.08 mm apart that are inclined at exactly 40° to A.[7][2]
Common mistakes
Giving the angle a ± tolerance and also adding angularityWhy: The angle tolerance and the angularity overlap, and the reference angle is not defined.Fix: Make the angle a TED and give the allowance with angularity.[2][7]
Standards: JIS B 0021:1998 18.11, ISO 1101.[7][8][9]
Location tolerance that limits how far a point, line (axis), or surface may deviate from its theoretically exact location (true position) defined by the datums and TEDs.[21][2][7][3]
Position: define the hole location with TEDs (boxed dimensions) without ±, and the hole axis only has to lie inside a cylinder of diameter t centered on the true position. The figure on the right is an enlarged top view of the hole, and the vermilion dotted line is the actual hole.Example of a feature control frame
How to write it on the drawing
Define the location with TEDsShow hole locations and the like with boxed TEDs, without ±.[6][2]
Tolerance frame"⌖|φt (Ⓜ if needed)|A|B|C". For the axis of a hole or shaft, add φ for a cylindrical tolerance zone; for the center of a sphere, use Sφ.[5][2][7]
Multiple holesConnect the tolerance frame to the note giving the number and size of holes (e.g. 6×).[2]
Example"⌖|φ0.05 Ⓜ|A|B|C" on a φ20H7 hole: the hole axis must lie inside a cylinder of diameter 0.05 mm centered on the true position defined by datums A, B, C and the TEDs. The position tolerance may grow by the amount the hole is finished larger than the maximum material size φ20.000.(An example built from the rules in the sources)[2][30][5]
Common mistakes
Chaining hole locations with toleranced dimensionsWhy: The tolerances accumulate and the positions of the holes relative to each other vary.Fix: Give locations as TEDs and the variation as position tolerance.[6]
Forgetting φWhy: Without φ the tolerance zone is two parallel planes in one direction, not a cylinder.Fix: Add φ to the position tolerance of the axis of a hole or shaft.[7][5][2]
JIS and ASMEASME calls it position (also true position). Since concentricity and symmetry were withdrawn in the 2018 edition, the location of coaxial or symmetric features is also controlled with position, runout, or profile.[3][12]
Standards: JIS B 0021:1998 18.12; positional tolerancing: JIS B 0025.[7][8][31]
Location tolerance that limits deviation of an axis that should lie on the same line as the datum axis. φ is added to the tolerance value, and the tolerance zone is a cylinder of diameter t coaxial with the datum axis.[21][2][7]
Coaxiality: the axis of the narrow section only has to lie inside a cylinder of diameter t coaxial with datum axis A. ASME has no coaxiality characteristic and uses position or runout instead (◎ means concentricity in ASME, which was withdrawn in the 2018 edition).Example of a feature control frame
How to write it on the drawing
Tolerance frame"◎|φt|A". The bearing seats at both ends are often made a common datum A-B.[2][7]
Example"◎|φ0.03|A": the axis of the cylinder the arrow points to must lie inside a cylinder of diameter 0.03 mm about datum axis A.[21]
Common mistakes
Using the dial indicator runout reading directly as coaxialityWhy: The value changes with the contact angle and force and varies from operator to operator.Fix: Determine the axis with a roundness measuring machine or a CMM and evaluate it.[32][2]
JIS and ASMEMitutoyo America points out that ISO coaxiality controls the axis (center line), whereas ASME 2009 concentricity controls the midpoints of opposing points, so the same symbol means different things. ASME 2018 controls the location of coaxial features with position, runout, or profile.[12]
Standards: JIS B 0021:1998 18.13.2, ISO 1101.[7][8][9]
Location tolerance that limits deviation of the center of a circle from the center of the datum circle in a plane figure (cross section). It uses the same symbol as coaxiality, but the target is a center point rather than an axis.[21][2][7]
Concentricity: in a cross section of a thin part, the center of the outer circle only has to lie inside a circle of diameter t concentric with datum circle A. The symbol is the same ◎ as coaxiality, but the target is a center point rather than an axis. Withdrawn in ASME Y14.5-2018.Example of a feature control frame
How to write it on the drawing
The symbol is the same ◎ as coaxialityWith φ before the tolerance value, the tolerance zone is a circle of diameter t centered on the datum point.[7][2]
Example"◎|φ0.1|A" (A = bore circle) on the center of the outer circle of a thin disc: the center of the outer circle must lie inside a circle of diameter 0.1 mm concentric with datum circle A.(An example built from the rules in the sources)[7]
Common mistakes
Confusing concentricity with coaxialityWhy: Concentricity controls the center point of a section, whereas coaxiality controls the whole axis.Fix: Use coaxiality for deviation of the whole shaft, and concentricity for a thin disc or a single section.[21][2][12]
JIS and ASMEConcentricity was withdrawn from ASME Y14.5-2018 entirely: term, symbol, and concept. US teaching materials note that it may still appear on older drawings.[12][3]
Standards: JIS B 0021:1998 18.13.1, ISO 1101.[7][8][9]
Location tolerance that limits deviation of the median plane of a feature that should be symmetric about a datum center plane (or axis). The tolerance zone is two parallel planes a distance t apart, symmetric about the datum.[21][2][7]
Symmetry: the median plane of the slot only has to lie between two parallel planes a distance t apart placed symmetrically about datum center plane A (the center of the full width). Withdrawn in ASME Y14.5-2018; specify with position or similar.Example of a feature control frame
How to write it on the drawing
Tolerance frame"⌯|tolerance value|A". Make the datum the center plane of the width, for example.[21][2]
Example"⌯|0.05|A" on the keyway width (A = center plane of the shaft): the median plane of the keyway must lie between two parallel planes 0.05 mm apart, symmetric about A.(An example built from the rules in the sources)[21][7]
Common mistakes
Checking only the wall thickness difference between left and right with a caliperWhy: A caliper measures the length between two points, but it is hard to evaluate symmetry as a geometric characteristic.Fix: Determine the median plane with a CMM or similar and evaluate it.[33]
JIS and ASMESymmetry was withdrawn in ASME Y14.5-2018 and is controlled with position or similar.[12][3]
Standards: JIS B 0021:1998 18.14, ISO 1101.[7][8][9]
Runout tolerance that limits surface runout (the difference between the maximum and minimum readings) at any measuring position when the part is rotated one full turn about the datum axis. There are radial, axial, and oblique directions.[22][2][7][3]
Circular runout: when rotated one full turn about datum A-B, the runout (maximum − minimum reading) is t or less in every cross section. If the arrow is placed on an end face, it becomes axial runout.Example of a feature control frame
How to write it on the drawing
Tolerance frame"↗|tolerance value|A" (A-B for a common datum).[7][22]
The arrow direction shows the directionAn arrow placed perpendicular to a cylindrical surface gives radial runout; placed on an end face, it gives axial runout.[7][2]
ExampleWith the bearing seats at both ends as common datum A-B, "↗|0.1|A-B" on the central outer surface: during one turn, the runout is 0.1 mm or less in every cross section.[7]
Common mistakes
Supporting and rotating the part on surfaces other than the drawing datumsWhy: If it is rotated about an axis different from the datum, that error is mixed into the runout.Fix: Support and rotate the part on the drawing datums (bearing seats, etc.) when measuring.[22][7]
JIS and ASMEASME uses the same concept under the name circular runout.[3]
Standards: JIS B 0021:1998 18.15, ISO 1101. The difference between the maximum and minimum runout readings is called T.I.R. (total indicator reading).[7][8][18]
Runout tolerance that limits runout over the whole surface, measured by rotating the part about the datum axis while moving the gauge along the surface.[22][2][7][3]
Total runout: while rotating about datum A-B and moving the gauge along the axis, the runout over the whole surface is t or less. Circular runout works section by section, whereas total runout evaluates the whole surface in a single tolerance zone.Example of a feature control frame
How to write it on the drawing
Tolerance frame"⌰|tolerance value|A-B". Place the arrow on a cylindrical surface (radial total runout) or an end face (axial total runout).[7]
Example"⌰|0.1|A-B": the cylindrical surface must lie between two cylinders coaxial with the common datum axis A-B and 0.1 mm apart in radius.[7]
Common mistakes
Assuming circular runout controls the whole surfaceWhy: Circular runout works section by section and cannot fully control overall taper or bending.Fix: Use total runout when you want to control runout of the whole surface.[22][3]
Standards: JIS B 0021:1998 18.16, ISO 1101.[7][8][9]
A theoretically exact reference (plane, line, or point) set up to define the tolerance zones for orientation, location, and runout. It is established from an actual surface or hole (the datum feature) on the part.[19][2]
The actual surface carrying the datum symbol (the datum feature) has irregularities. Place it on a precision surface such as a surface plate and treat that surface as the datum (a theoretically exact plane).
How to write it on the drawing
Indicate with the datum symbolAdd the datum symbol to the surface or axis used as the reference.[19][2]
Establish it by contacting a precision surfaceBecause the actual surface has irregularities, set up the reference by placing it on a precision surface (a datum feature simulator) such as a surface plate or mandrel.[19][2]
ExampleWhen the center of a hole is the datum: insert a precision shaft that fits the hole as the maximum inscribed cylinder, and take its axis as the datum axis.[34]
Common mistakes
Using a wavy surface as a full-surface datum as it isWhy: The contact points change every time, causing large errors in machining and inspection.Fix: Specify an accuracy suitable for a reference, or limit the contact points with datum targets.[35][2]
JIS and ASMEASME calls the tool or surface that physically establishes a datum from a datum feature a datum feature simulator (equivalent to the JIS practical datum feature).[34]
Standards: JIS B 0022:1984 (Datums for geometrical tolerancing), ISO 5459:2024. Term definitions: JIS Z 8114.[10][36][19]
Symbol that shows on the drawing which surface or axis is the datum. Put a capital letter identifying the datum in a square frame, connect it to an open or filled triangle, and attach it to the datum feature.[19][2][3]
If the datum triangle is offset from the dimension line and placed on the outline, the surface becomes the datum; if it is aligned with the extension of the dimension line, the axis or median plane becomes the datum. The triangle may be open or filled.
How to write it on the drawing
The triangle may be open or filledPlace the triangle on the outline or the dimension line.[19]
Letters face the viewing direction of the drawingDo not rotate the letter in the frame; write it upright as the drawing is read.[19]
To make a surface the datumPlace the triangle on the outline or its extension, offset from the dimension line.[19][2]
To make an axis or median plane the datumPlace the triangle on the extension of the dimension line of the feature of size (in line with the dimension line).[19][2]
ExampleTo make the center of a φ30 shaft datum A: place the datum triangle on the extension of the φ30 dimension line and write A in the frame.(An example built from the rules in the sources)[19][2]
Common mistakes
Thinking an offset triangle indicates the center of the shaftWhy: When offset, the surface (generatrix) becomes the datum, not the axis.Fix: To make the center the datum, place the triangle in line with the dimension line.[19]
JIS and ASMEASME is similar: a letter in a square frame is attached to the feature with a triangle.[3]
Standards: JIS B 0022; supplementary symbols (datum indication) in JIS B 0021.[7][10]
Datum system (three-plane datum reference frame)dētamu keidatum system / datum reference frame
A combination of two or more datums in order of precedence. A set of three mutually perpendicular datum planes that fully constrains the orientation of the part is called a three-plane datum system.[37][2]
Three-plane datum system: the datums in the tolerance frame are, from the left, primary, secondary, and tertiary. Contact A (primary) at 3 points, B (secondary) at 2 points, and C (tertiary) at 1 point (the same idea as 3-2-1 locating in jigs). The numbered points are on the far faces and are drawn as if seen through the part.Example of a feature control frame
How to write it on the drawing
Precedence runs from the left of the tolerance frameWrite the datums in the datum fields from the left in the order primary, secondary, tertiary. Designers usually assign letters in order of precedence.[5][2]
Order of contactPress the part against the primary, secondary, and tertiary datums in that order to fully constrain it (this corresponds to 3-2-1 locating in jigs).[37][38]
Example"⌖|φ0.1|A|B|C": establish the reference by contacting A (bottom face), then B (long side face), then C (short side face).(An example built from the rules in the sources)[37][5][2]
Common mistakes
Choosing the datum order without regard to how the part is located in machining and assemblyWhy: If the order of precedence changes, the measurement result changes even for the same part.Fix: Make the surface most important for function and assembly the primary datum.[5][2]
JIS and ASMEASME calls it a datum reference frame and explains it as constraining degrees of freedom (the 2018 edition expanded the description of datums and degrees of freedom).[11]
A single datum made from two datum features. For example, the bearing seats at both ends of a shaft are combined into one common axis. In the tolerance frame, write them in one field joined by a hyphen, as in "A-B".[37][7]
Common datum: attach datums A and B to the bearing seats at the two ends and write "A-B" in a single field of the tolerance frame. The reference is the single axis formed by simultaneously contacting both bearing seats.Example of a feature control frame
How to write it on the drawing
Hyphen in the datum fieldAttach a datum symbol (A, B) to each of the two datum features, and write them together as "A-B" in one datum field of the tolerance frame.[37][7]
ExampleMake the bearing seats at both ends datums A and B, and specify the runout of the central section with "↗|0.1|A-B".[7][37]
Common mistakes
Confusing "A-B" with "A|B"Why: "A-B" is one common datum, while "A|B" is two datums with an order of precedence (a datum reference frame).Fix: When two features are to serve as equal references, write them in one field with a hyphen.[37][5]
A method of setting a datum by specifying the points, lines, or limited areas that the machining or measuring equipment contacts, instead of the whole surface. Used for parts with wavy surfaces, such as castings, forgings, and sheet metal.[35][2]
Datum target: datum A is established by supporting only at specified points (×) or areas (hatching), not on the whole wavy surface. The frame is a circle divided by a horizontal line: the datum letter and number go in the lower half and the size of the area in the upper half.
How to write it on the drawing
Datum target frameDraw a circle divided by a horizontal line, and write the datum letter and number (such as A1) in the lower half and the size of the area (such as φ2) in the upper half.[35][2][14]
Showing points, lines, and areasPoints, lines, circular areas, and rectangular areas are each shown with the prescribed graphical symbol.[35][2]
Common mistakes
Using the whole wavy cast surface as the datumWhy: The contact points change every time, so repeatability and reproducibility get worse.Fix: Limit the contact points with datum targets.[35][2]
JIS and ASMEASME has a symbol for movable datum targets (KEYENCE explains that ISO and JIS have this under proposal).[13][14]
Standards: JIS B 0022; supplementary symbols (datum target) in JIS B 0021:1998.[10][7]
Datum feature simulatorjitsuyō dētamu keitaisimulated datum feature / datum feature simulator
A sufficiently precise surface or shaft (surface plate, bearing, mandrel, etc.) that is brought into contact with the datum feature to physically establish the datum.[19][34][2]
Datum feature simulator: apply the maximum inscribed cylinder (a precision shaft that just fits) to a hole and the minimum circumscribed cylinder (a precision hole that just fits) to a shaft, and take its axis as the datum axis. The green dotted line is the datum feature simulator and the black outline is the actual feature (exaggerated).
How to write it on the drawing
Planes: surface plateMake the datum plane with the surface of a surface plate.[34][2]
Hole: maximum inscribed cylinder; shaft: minimum circumscribed cylinderApply a tight-fitting precision shaft to a hole and a tight-fitting precision hole to a shaft, and take its axis as the datum.[34]
Obtained with a CMMA datum calculated from measured points is sometimes called a substitute datum.[2]
JIS and ASMEASME Y14.5 calls it a datum feature simulator.[34]
□Theoretically exact dimension (TED)riron-teki ni seikaku na sunpōtheoretically exact dimension / TED / basic dimension
A theoretical dimension with no tolerance, used to define the location and shape of tolerance zones for position, profile, angularity, and so on. The value is enclosed in a rectangular frame, and the variation is given by the geometric tolerance in the tolerance frame.[6][2][3]
Theoretically exact dimension (TED): enclose the value in a frame and do not add ±. The location variation is given for each hole by the position tolerance in the tolerance frame, so chaining dimensions does not accumulate error (the small yellow circles are the tolerance zones of each hole).
How to write it on the drawing
Enclose the value in a frameExample: [50]. The same applies to angles.[2][14]
Give variation in the tolerance frameDo not add ± to TEDs; give the allowance with a tolerance such as position.[6][3]
ExampleKEYENCE example: linking the holes with size tolerances gives a maximum of 45.3, whereas defining them with TEDs and position tolerance gives a maximum of 45.1, so the tolerances do not accumulate.[6]
Common mistakes
Assuming general tolerances also apply to TEDsWhy: A TED is a value without tolerance, and the general tolerances in the title block do not apply.Fix: Specify variation in location or shape with geometric tolerances.[3][6]
JIS and ASMEASME calls it a basic dimension, and the boxed notation is the same.[3]
Standard: supplementary symbols (theoretically exact dimension) in JIS B 0021:1998.[7][8]
ⓂMaximum material requirement (MMR)saidai jittai kōsa hōshikimaximum material requirement / MMR / MMC modifier
A requirement that allows orientation or location tolerances to be increased by the amount the feature is finished away from its maximum material condition (smallest diameter for a hole, largest diameter for a shaft). It lets you use the tolerance effectively while still ensuring that mating parts assemble.[30][39][2][3]
Maximum material requirement ("⌖|φ0.1 Ⓜ" on a φ10 +0.1/0 hole): the parts assemble if the feature fits over the pin φ9.9 (= 10.0 − 0.1, the virtual size) of a functional gauge that represents the mating part. The larger the hole is finished, the more the center may deviate, so the position tolerance can be widened (clearance exaggerated).Example of a feature control frame
How to write it on the drawing
Ⓜ after the tolerance valueAdd Ⓜ after the geometric tolerance value in the tolerance frame. To apply it to a datum as well, add Ⓜ after the datum letter.[39][30][2]
Check with a dynamic tolerancing diagramPlot the size tolerance on the horizontal axis and the geometric tolerance on the vertical axis to see how the geometric tolerance increases (bonus tolerance) with the finished size.[30]
Example"⌖|φ0.1 Ⓜ|A|B|C" on a φ10 +0.1/0 hole: if the hole is φ10.00 (maximum material), the position tolerance is φ0.1; if it is finished at φ10.06, up to φ0.16 is allowed (φ0.2 at most).(An example built from the rules in the sources)[2][30]
Common mistakes
Thinking the size tolerance is relaxed tooWhy: Ⓜ relaxes only the geometric tolerance; the size tolerance must always be met.Fix: Judge separately whether the size is within tolerance and whether the geometric tolerance is within the value allowed for the finished size.[30]
Adding Ⓜ to features unrelated to fitsWhy: Ⓜ exploits assembly clearance, and on features where the location itself matters for function it can loosen the tolerance too much.Fix: Use it mainly on features of parts that are fitted together.[39][30]
JIS and ASMEISO and JIS call it the "maximum material requirement (MMR)", while ASME treats the symbol as a modifier for "maximum material condition (MMC)". In ASME, with no symbol the tolerance applies regardless of feature size (RFS), and the old ANSI Ⓢ symbol was deleted in the 2009 edition.[39][3][14]
Standards: JIS B 0023 (maximum material principle and least material principle); supplementary symbols in JIS B 0021:1998.[40][7]
Maximum material condition (MMC) and maximum material size (MMS)saidai jittai jōtai / saidai jittai saizumaximum material condition / MMC / maximum material size / MMS
Maximum material condition (MMC) is the limit condition of the permitted range in which the feature has the most material (volume): the smallest diameter for a hole and the largest diameter for a shaft. The size in that condition is the maximum material size (MMS).[16][2][41]
MMC is the limit on the side where the most material remains: the largest diameter for a shaft and the smallest for a hole. In both cases the fit is at its tightest (size difference exaggerated).
ExampleKEYENCE's figure example gives the maximum material size of a φ20 shaft (convex) as φ20.1 and that of a hole (concave) as φ19.9 (the larger side for the shaft, the smaller side for the hole).[16]
Common mistakes
Mistaking the largest diameter for the maximum material condition of a holeWhy: The smaller the hole diameter, the more material remains.Fix: Remember that MMC is the smallest diameter for a hole and the largest for a shaft.[2][41]
JIS and ASMEASME defines MMC and LMC the same way. US teaching materials explain that starting to cut from the MMC side lets you machine while leaving material.[41]
ⓁLeast material requirement (LMR)saishō jittai kōsa hōshikileast material requirement / LMR / LMC modifier
A requirement that allows the geometric tolerance to be increased by the amount the feature is finished away from its least material condition (largest diameter for a hole, smallest diameter for a shaft). Used to secure strength, such as the remaining wall thickness of a hole near an edge or the wall thickness of a pipe.[42][39][2]
How to write it on the drawing
Ⓛ after the tolerance valueAdd Ⓛ after the geometric tolerance value in the tolerance frame. In some cases, also add it after the datum letter.[42][39]
ExampleKEYENCE example: if Ⓛ is added to a position tolerance φ0.5 on a φ24 hole (LMC is φ24.1), φ0.5 applies when the hole is φ24.1, and the smaller the hole is finished, the more the position tolerance is relaxed.[42]
Common mistakes
Adding Ⓜ to a hole where remaining wall thickness must be securedWhy: Ⓜ allows more position error the larger the hole is, which works in the direction of leaving too little wall thickness to the edge.Fix: Consider Ⓛ for features where remaining wall thickness matters.[42]
JIS and ASMEASME treats it as a modifier for LMC (least material condition).[3]
The limit of perfect form (virtual condition; its size is the virtual size) determined by the combined effect of the maximum material size and a geometric tolerance with Ⓜ. For an external feature (shaft) it is MMS + geometric tolerance, and for an internal feature (hole) it is MMS − geometric tolerance; this becomes the design dimension of the functional gauge.[2][18][30]
Virtual size: the limit combining the maximum material size and a geometric tolerance with Ⓜ. For a shaft φ150 0/−0.04 with "⟂|φ0.05 Ⓜ|A", it passes if it goes into a φ150.05 hole (functional gauge) perpendicular to A (tilt exaggerated).Example of a feature control frame
How to write it on the drawing
Use it for the gauge dimensionMake the dimension of the functional gauge hole (or pin) the virtual size.[2]
ExampleMitutoyo example: shaft φ150 0/−0.04 with "⟂|φ0.05 Ⓜ|A" → virtual size is φ150.05.[2]
Common mistakes
Making the functional gauge at the maximum material sizeWhy: The geometric tolerance with Ⓜ is not included, so good parts are rejected.Fix: Make the functional gauge at the virtual size.[2]
The amount added to the geometric tolerance according to the finished size under the maximum (least) material requirement.[18][2][30]
"⌖|φ0.1 Ⓜ" on a φ10 +0.1/0 hole: the horizontal axis is the finished hole diameter and the vertical axis is the allowed position tolerance. The amount away from MMC φ10.00 is added as bonus, so up to φ0.16 is allowed at φ10.06 and up to φ0.2 at φ10.1.
How to write it on the drawing
How to judgeAdd the difference between the measured size and the maximum material size to the tolerance value in the tolerance frame and judge with that.[2][18]
ExampleMitutoyo example: hole lower limit φ59.9, position φ0.02 Ⓜ, measured hole diameter φ60.000 → bonus 0.1, so the position tolerance used for judgment is φ0.12.[2]
Common mistakes
Judging by the position value alone without looking at the finished diameterWhy: If you ignore the bonus on a drawing with Ⓜ, you end up scrapping good parts.Fix: Calculate the bonus from the measured diameter and judge with it.[2][18]
Zero geometric tolerancing at MMCzero kika kōsa hōshikizero geometric tolerancing at MMC
A specification that sets the geometric tolerance to zero at maximum material condition and gives the difference as geometric tolerance as the feature approaches least material condition (zero geometric tolerancing at MMC).[18]1 source (for reference)
"⌖|φ0 Ⓜ" on a φ10 +0.1/0 hole: if the hole is φ10.00 (MMC) the position error is 0, and position tolerance is allowed by the amount the hole is finished larger (φ0.06 at φ10.06, φ0.1 at φ10.1).Example of a feature control frame
Example"⌖|φ0 Ⓜ" on a φ10 +0.1/0 hole: no position error is allowed if the hole is φ10.00, and up to φ0.1 is allowed if it is finished at φ10.1.(An example built from the rules in the sources)[18]
Maximum material requirement applied to datums (datum shift)dētamu no fudōdatum feature at MMB / datum shift
When the datum is a feature of size, add Ⓜ after the datum letter to apply the maximum material requirement to the datum as well, so that the datum is not fixed (it floats).[18][39]1 source (for reference)
How to write it on the drawing
Ⓜ after the datum letterIn the datum field of the tolerance frame, add Ⓜ after the letter.[39][30]
JIS and ASMEKEYENCE explains that ASME has symbols for maximum material boundary (MMB) and least material boundary (LMB), while ISO and JIS have no corresponding symbols.[13]
Ⓢ (formerlyRFS (regardless of feature size)āru efu esuregardless of feature size / RFS
Applying the specified geometric tolerance value as is, regardless of how the size is finished (RFS, regardless of feature size). Old ANSI standards showed it with the symbol Ⓢ, which was deleted in ASME Y14.5-2009.[14]1 source (for reference)
JIS and ASMEIn ISO and JIS, the tolerance has always applied regardless of material condition unless Ⓜ or Ⓛ is added.[39][2]
ⓅProjected tolerance zonetosshutsu kōsa-ikiprojected tolerance zone
A specification that applies the tolerance zone not to the feature itself but to an imaginary region projected out toward the mating part. It ensures that a bolt or pin standing in a threaded hole will reliably enter the hole in the mating part.[43][3][2]
Projected tolerance zone Ⓟ: the tolerance zone of the threaded-hole axis is placed in the region projected toward the mating part, where the bolt goes (boxed length 30). If the threaded hole is slightly tilted, the deviation becomes larger at the position of the mating part (tilt exaggerated).
How to write it on the drawing
Ⓟ and projection length in the tolerance frameAdd Ⓟ to the tolerance value in the tolerance frame and specify the projection length.[43][3]
Projected portion as a thin two-dot chain lineDraw the imaginary projected portion with a thin two-dot chain line (as explained by KEYENCE).[43]
ExampleKEYENCE example: the axis of the φ28 feature in the imaginary space is perpendicular to datum A and located 40 from datum B, and must lie inside a φ0.5 cylinder over the entire projected length of 30 mm.[43]
Common mistakes
Controlling the position of a threaded hole only inside the holeWhy: If the hole is slightly tilted, the position error grows at the tip of the protruding bolt and it interferes with the mating part.Fix: Control the thickness of the mating part with a projected tolerance zone.[43][3]
JIS and ASMEIn US teaching materials, the projected region is shown with a thick chain line. The JIS-based explanation (KEYENCE) uses a thin two-dot chain line.[45][43]
Standard: JIS B 0029 (projected tolerance zone). The supplementary symbol table in JIS B 0021 refers to ISO 10578.[44][7]
CZCommon tolerance zonekyōtsū kōsa-ikicommon zone / CZ
A specification that controls several separated features together in a single tolerance zone. Write CZ after the tolerance value.[2][14][5]
Common zone CZ: two separate surfaces are controlled together by one pair of parallel planes (0.1 apart). Without CZ, each surface only has to be within 0.1 separately.Example of a feature control frame
How to write it on the drawing
CZ after the tolerance valueWrite it like "⏥|0.1 CZ" and draw leader lines from one tolerance frame to each target surface.[2]
Example"⏥|0.1 CZ" on two separate surfaces: both surfaces must lie within the same pair of parallel planes (0.1 apart). Without CZ, each surface only has to be within 0.1 separately.[2]
Common mistakes
Specifying several surfaces with one tolerance frame without CZWhy: Each surface is judged against its own tolerance zone, and the step between the surfaces is not controlled.Fix: Add CZ when the surfaces must be coplanar.[2]
Standard: supplementary symbols (common zone) in JIS B 0021:1998.[7][8]
ⒻFree state (non-rigid parts)jiyū jōtaifree state / non-rigid part
Symbol that shows the tolerance applies in the free state, with only gravity acting, for parts that may deform beyond the tolerance in the free state (non-rigid parts), such as rubber, plastic, and thin-walled parts.[46][7][2]
How to write it on the drawing
Ⓕ after the tolerance valueAdd Ⓕ to geometric tolerances that apply in the free state.[46]
Note the restraint conditionsState in a note that the part is non-rigid and the conditions (such as gravity direction) for tolerances that apply in the restrained state.[46]
ExampleKEYENCE example: circularity 5.0 Ⓕ on datum B (within 5.0 in the free state in any orientation), and the circular runout on the left applies in the restrained state given in the note.[46]
Standards: JIS B 0026 (non-rigid parts); JIS B 0420-1 7.8.[47][7][48]
All-around symbol (profile)zenshū kigōall around symbol
Symbol, a small circle at the bend of the leader line of the tolerance frame, used when profile tolerance or the like applies all around the outline shown in the view.[2][14][7]
Example of a feature control frame
How to write it on the drawing
Circle at the bend of the leader lineDraw a small circle at the bend of the leader line from the tolerance frame.[2][14]
Example"⌒|0.05" with the all-around symbol on the whole outline: the entire outline lies within a band of ±0.025 on both sides of the theoretical shape.[2]
Common mistakes
Confusing it with the all-around symbol of weldingWhy: They look similar, but the circle in a welding symbol means weld all around.Fix: Tell them apart by which symbol system they are used in.[49][2]
Standard: supplementary symbols (all around (profile)) in JIS B 0021:1998.[7][8]
UZ (ISO, JIS) / Ⓤ (ASME)Unequally disposed profilefukintō haibun no rinkakudounequally disposed profile
A specification that places the profile tolerance zone unevenly, shifted toward one side of the theoretical profile instead of equally on both sides (unequally disposed profile). ISO and JIS use UZ; ASME uses Ⓤ.[13][14]1 source (for reference)
Composite position tolerancingfukugō ichido kōsa hōshikicomposite positional tolerancing
A method that uses a two-tier tolerance frame with a single position symbol, giving different tolerance values in the upper tier for location relative to the datum reference frame and in the lower tier for the relative location between features (composite positional tolerancing).[18]1 source (for reference)
How to write it on the drawing
Two-tier tolerance frameCombine the position symbol into one, and write the tolerance relative to the datum reference frame in the upper tier and the tolerance for the relative location between features in the lower tier.[18]
A diagram with the size tolerance on the horizontal axis and the geometric tolerance on the vertical axis, showing both variations and the bonus tolerance obtained under the maximum material requirement at the same time (dynamic tolerancing diagram).[30]1 source (for reference)
"⌖|φ0.1 Ⓜ" on a φ10 +0.1/0 hole: the horizontal axis is the finished hole diameter and the vertical axis is the allowed position tolerance. The amount away from MMC φ10.00 is added as bonus, so up to φ0.16 is allowed at φ10.06 and up to φ0.2 at φ10.1.
How to write it on the drawing
Choosing the axesPlot size on the horizontal axis and the allowed geometric tolerance on the vertical axis, and show the change from MMC to LMC as a line.[30]
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.