For engineers who already know the math—but still lose projects. For the last few years, I’ve been sharing technical guides here on Mechanical Design Handbook —how to size a motor, how to calculate fits, and (as you recently read) how to choose between timing belts and ball screws. But after 25 years in industrial automation, I realized something uncomfortable: Projects rarely fail because the math was wrong. They fail because: The client changed the scope three times in one week. A critical vendor lied about a shipping date (and no one verified it). The installation technician couldn’t fit a wrench into the gap we designed. University taught us the physics. It didn’t teach us the reality. That gap is why I wrote my new book, The Sheet Mechanic . This is not a textbook. It is a field manual for the messy, political, and chaotic space between the CAD model and the factory floor. It captures the systems I’ve used to survive industrial projec...
Mechanical Design Handbook · Reference
A working reference for reading and creating mechanical drawings under the two systems you will meet in practice: ASME Y14 (common in North America and US-linked supply chains) and ISO GPS (common in Europe and Asia). It covers drawing fundamentals, the geometric tolerancing symbols with use cases, worked bonus-tolerance examples, and a self-check quiz.
Standards cited by edition are the ones generally current as of 2026. Tables are summaries for learning. For release work, check your licensed copy and the edition your drawing calls out.
Advertisement
1. Standards map: ASME vs ISO
Both systems describe the same physical part. They differ in defaults, some symbols, and how a drawing is interpreted when something is not stated. Always know which system governs a drawing before you read a single tolerance. A drawing should say so in or near the title block, for example "DIMENSIONING AND TOLERANCING PER ASME Y14.5-2018" or "ISO 8015".
| Topic | ASME (Y14 series) | ISO |
|---|---|---|
| Dimensioning and geometric tolerancing | ASME Y14.5-2018 | ISO 1101:2017 (geometrical tolerancing), ISO 5459 (datums), ISO 2692 (MMR, LMR), ISO 14405 (size), ISO 129-1 (dimension presentation) |
| Fundamental interpretation | Built into Y14.5 (Rule #1, Rule #2) | ISO 8015:2011 (GPS fundamentals, independency principle) |
| Mathematical definition | ASME Y14.5.1 | Distributed across the GPS standards |
| Drawing practices and types | ASME Y14.100, Y14.24 | ISO 128 series, ISO 7200 (title block) |
| Views and projection | ASME Y14.3 | ISO 128-3, ISO 5456-2 |
| Line conventions | ASME Y14.2 | ISO 128-2 |
| Sheet sizes | ASME Y14.1 (inch), Y14.1M (metric) | ISO 5457 (A-series) |
| Surface texture symbols | ASME Y14.36 | ISO 21920-1 (replaces ISO 1302) |
| General tolerances | Stated in the title block or notes | ISO 2768-1 (linear and angular), ISO 22081 (general geometrical and size specifications; replaces ISO 2768-2) |
| Limits and fits | ANSI B4.1 (inch), B4.2 (metric) | ISO 286-1, ISO 286-2 |
| Model-based definition | ASME Y14.41 | ISO 16792 |
2. Sheets, title blocks and projection
Sheet sizes
| ISO 5457 | Size (mm) |
|---|---|
| A0 | 841 × 1189 |
| A1 | 594 × 841 |
| A2 | 420 × 594 |
| A3 | 297 × 420 |
| A4 | 210 × 297 |
| ASME Y14.1 | Size (in) |
|---|---|
| A | 8.5 × 11 |
| B | 11 × 17 |
| C | 17 × 22 |
| D | 22 × 34 |
| E | 34 × 44 |
Title block essentials
ISO 7200 defines the data fields; ASME Y14.100 covers the equivalent practice. Whatever the template, a title block should let anyone answer these questions without asking the designer:
- What is it? Title, part or drawing number, revision.
- Who owns and approved it? Legal owner, creator, approver, dates.
- How do I read it? Units, projection symbol, scale, governing standard (ASME Y14.5 or ISO 8015 and related).
- What applies when nothing is stated? General tolerance callout (for example ISO 2768-mK, or an ASME-style tolerance block by decimal places).
- What is it made of? Material, finish or treatment, sheet number of total.
First angle vs third angle projection
The two methods place the same views in mirrored positions. Getting this wrong flips a part. The projection symbol in the title block is the only reliable way to tell.
3. Line types and views
ISO 128-2 and ASME Y14.2 agree on the main ideas: two line widths (thick for what you are meant to see, thin for everything that explains it) and a small set of patterns. ISO uses a thick-to-thin ratio of 2:1.
| Line | Pattern | Use |
|---|---|---|
| Continuous thick | Visible edges and outlines | |
| Continuous thin | Dimension, extension and leader lines, hatching | |
| Dashed thin | Hidden edges | |
| Long dash dot thin (chain) | Center lines, axes, lines of symmetry, pitch circles | |
| Long dash double dot thin | Adjacent parts, alternate positions (phantom lines) | |
| Chain, thick at ends and changes | Cutting planes (ISO). ASME draws cutting planes as thick dashed or thick phantom lines. | |
| Freehand or zigzag thin | Break lines, partial views |
Choosing views
- Pick the front view that shows the most characteristic shape, in the part's functional or machining orientation.
- Use the minimum number of views that fully define the part. Add a view only when it removes ambiguity or hidden lines.
- Use sections (full, half, offset, revolved, removed) to show internal features instead of dense hidden lines.
- Use detail views (enlarged, with scale noted) for small features that carry tight tolerances.
- Use auxiliary views to show the true shape of inclined surfaces.
4. Dimensioning and tolerancing basics
Fundamental rules (paraphrased from ASME Y14.5 and ISO 129-1)
- Every dimension has a tolerance, stated directly or through a general tolerance note. Exceptions: basic (theoretically exact), reference, and stock dimensions.
- Dimension completely, but only once. No double dimensioning, no closed chains.
- Choose dimensions to define function and mating, not to describe how the shop should make it.
- Do not specify manufacturing methods unless the method is part of the requirement.
- Dimension to visible outlines and true-shape views, not to hidden lines.
- Unless stated otherwise, lines shown at 90° are 90°, and the general angular tolerance applies.
- Dimensions apply in the free state at 20 °C unless otherwise specified (ISO 1 sets 20 °C as the reference temperature).
General tolerances: ISO 2768-1 linear (summary)
A callout such as ISO 2768-mK means tolerance class m (medium) for untoleranced linear and angular dimensions under ISO 2768-1, and class K for general geometrical tolerances under ISO 2768-2. Note that ISO 2768-2 has been replaced by ISO 22081:2021, so new drawings should state general geometrical specifications per ISO 22081 instead of the letter H, K or L.
| Nominal range (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5 to 3 | ±0.05 | ±0.1 | ±0.2 | n/a |
| over 3 to 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| over 6 to 30 | ±0.1 | ±0.2 | ±0.5 | ±1 |
| over 30 to 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| over 120 to 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| over 400 to 1000 | ±0.3 | ±0.8 | ±2 | ±4 |
| over 1000 to 2000 | ±0.5 | ±1.2 | ±3 | ±6 |
| over 2000 to 4000 | n/a | ±2 | ±4 | ±8 |
Limits and fits (ISO 286, hole-basis examples)
In the hole-basis system the hole is H (lower deviation zero) and the shaft letter sets the fit. A few classic pairings:
| Fit | Type | Typical use |
|---|---|---|
| H11/c11 | Loose running clearance | Loose pivots, parts exposed to dirt or heat growth |
| H9/d9 | Free running clearance | Large clearance bearings, idler shafts |
| H7/g6 | Close sliding clearance | Sliding gears, locating pins that must be removable by hand |
| H7/h6 | Locational clearance | Spigots and locating registers that assemble freely |
| H7/k6 | Transition | Hubs, couplings, accurate location with light force |
| H7/p6 | Locational interference | Bushings, permanent location, pressed with force |
| H7/s6 | Medium drive interference | Permanent torque-carrying assemblies, press or shrink fit |
Surface texture
The basic symbol is a check mark. A bar across the top means material removal is required. A circle in the vee means material removal is not permitted. The parameter and value sit above or beside it, for example Ra 1.6 (µm). ASME uses Y14.36. ISO now uses ISO 21920-1, which replaced ISO 1302 in 2021 and changed some default rules, so check which edition your template follows.
5. Rule #1 vs the independency principle
This is the single most important difference between the two systems, and the one most often missed when a drawing moves between suppliers.
ASME Y14.5: Rule #1 (envelope principle)
For a regular feature of size, the surface may not extend beyond a perfect-form boundary at maximum material condition. A Ø10.0 to 10.2 pin with no geometric tolerance must fit inside a perfect Ø10.2 cylinder. Size controls form automatically.
Exceptions include stock material, parts in the free state, and features marked with the independency symbol Ⓘ (added in the 2018 edition).
ISO 8015: independency principle
Size and form are independent by default. A Ø10.0 to 10.2 pin is checked by two-point local size only; it may be bent or lobed and still conform. To require the envelope, add Ⓔ after the size (ISO 14405-1), or apply a form tolerance.
The same drawing therefore accepts different parts depending on which system governs it.
Rule #2 (ASME) and the ISO default: geometric tolerances apply regardless of feature size (RFS in ASME, RFS by default in ISO) unless Ⓜ or Ⓛ is shown. The old Ⓢ symbol is no longer used in either system.
6. GD&T building blocks
The feature control frame
A feature control frame reads left to right as one sentence: "the characteristic of this feature must be within a zone of this shape and size, at this material condition, relative to datums A then B then C."
Datums and the datum reference frame
- Datum feature: the real, imperfect surface or feature on the part, identified with a datum feature symbol (a capital letter in a box, attached by a triangle).
- Datum: the theoretically exact plane, axis or point derived from that feature by a simulator (a surface plate, a chuck, a gauge pin).
- Datum reference frame (DRF): three mutually perpendicular planes. Primary datum constrains up to three degrees of freedom, secondary up to two, tertiary the rest. Order matters: A | B | C and B | A | C can accept different parts.
- Choose datum features that match how the part is located and clamped in its assembly, not what is convenient to measure.
- Datum targets (points, lines, areas) are used when a whole surface is unsuitable, such as castings, forgings, sheet metal and weldments.
Material conditions
| Term | External feature (pin, shaft) | Internal feature (hole, slot) |
|---|---|---|
| MMC, maximum material condition | Largest size | Smallest size |
| LMC, least material condition | Smallest size | Largest size |
| Bonus tolerance (at Ⓜ) | MMC − actual size | Actual size − MMC |
| Virtual condition (at Ⓜ) | MMC + geometric tolerance | MMC − geometric tolerance |
Virtual condition is the worst-case boundary the mating part sees. It is the size of a fixed functional gauge pin or ring. ISO calls the same idea the maximum material virtual condition (MMVC) under ISO 2692.
Advertisement
7. The geometric characteristic symbols
ASME Y14.5-2018 has 12 characteristics. ISO 1101 keeps two more, concentricity/coaxiality and symmetry, which ASME removed in 2018. Filter the cards by group.
Straightness
Zone: two parallel lines (surface line elements), or a cylinder when applied to the derived median line of a feature of size.
Use case: a long ground shaft or linear guide rod that must slide through a bushing. Applied to the axis with Ⓜ, it lets the shop trade size for bend while a ring gauge still checks assembly.
Ø0.05 Ⓜ
Flatness
Zone: two parallel planes the tolerance value apart. The planes float; they are not tied to any datum.
Use case: the mounting face of a machine base plate, a sealing face for a gasket, or a primary datum surface that must sit stably on its mating part.
0.02
Circularity (roundness)
Zone: two concentric circles in each cross section, perpendicular to the axis. Each section is judged on its own.
Use case: an O-ring groove bore or a bearing journal where lobing would cause leakage or vibration but taper is controlled separately.
0.01
Cylindricity
Zone: two coaxial cylinders. Controls circularity, straightness and taper of the whole surface at once.
Use case: a pneumatic or hydraulic cylinder bore, or a precision shaft running in a long plain bearing.
0.01
Profile of a line
Zone: a 2D band either side of the true profile, in each section parallel to the view. Without datums it controls form only; with datums it also controls orientation and location.
Use case: the cross section of an aluminum extrusion, or an airfoil or cam section where each slice matters more than the whole surface.
0.1A
Profile of a surface
Zone: a 3D band around the true surface defined by basic dimensions or the CAD model. Equal bilateral by default; use Ⓤ (ASME) or UZ (ISO) for unequal zones.
Use case: a cam track, a formed sheet-metal flange, a cast or molded surface, or locating a non-cylindrical cutout. Often the cleanest replacement for ± location of non-round features.
0.2ABC
Parallelism
Zone: two planes parallel to the datum (or a cylinder for an axis). Controls orientation and flatness of the surface, not its distance from the datum.
Use case: the top and bottom faces of a spacer block or riser, so a stacked fixture stays level.
0.02A
Perpendicularity
Zone: two planes at 90° to the datum, or a cylinder at 90° for an axis (with Ø).
Use case: a dowel pin hole perpendicular to the mounting face, or the vertical wall of an L-bracket that locates a sensor.
Ø0.02A
Angularity
Zone: two planes at a basic (boxed) angle to the datum. The angle itself carries no ± tolerance.
Use case: the inclined face of a wedge clamp, a chamfered lead-in that guides a part, or an angled coolant hole.
0.05A with a basic angle 30°
Position
Zone: usually a cylinder (Ø) centered on the true position set by basic dimensions from the datums. Also controls orientation of the axis within that zone.
Use case: bolt hole patterns, dowel holes, and any feature that mates with another part. The most used GD&T control, and the main one that benefits from Ⓜ.
Ø0.1 ⓂABC
Concentricity / coaxiality
Zone (ISO 1101): a cylinder around the datum axis (coaxiality), or a circle around a datum point in a section (concentricity).
Use case: ISO drawings of stepped shafts and turned parts. Under ASME 2018, use position, runout, or profile instead; they are easier to measure and state the real function.
Ø0.03A
Symmetry
Zone (ISO 1101): two parallel planes centered on the datum median plane.
Use case: a keyway or slot centered on a shaft or block on an ISO drawing. Under ASME 2018, use position (often with Ⓜ) or profile.
0.05A
Circular runout
Zone: at each measuring position, the indicator reading over one full rotation about the datum axis (full indicator movement) must not exceed the value. Controls circularity and coaxiality per section, not taper.
Use case: a pulley or sprocket seat, a gear hub, or a seal running surface on a rotating shaft.
0.02A-B
Total runout
Zone: the whole surface, with the indicator traversed along it while the part rotates, stays within the value. On a diameter it controls cylindricity and coaxiality together; on a face it controls flatness and perpendicularity to the axis.
Use case: a motor shaft bearing seat, a spindle nose, or the face of a rotary indexing plate.
0.02A-B
Quick rules for choosing a control
| Group | Controls | Datum | Can use Ⓜ or Ⓛ? |
|---|---|---|---|
| Form | Shape only | Never | Only straightness or flatness of a derived median line or plane |
| Profile | Form, plus orientation and location when datums are given | Optional | Not on the tolerance in ASME; datum features may be referenced at MMB |
| Orientation | Orientation and, for surfaces, form | Always | Yes, when applied to a feature of size |
| Location | Location, orientation (and form for surfaces) | Usually | Position: yes |
| Runout | Form, orientation and location relative to an axis | Always (axis) | No, always RFS |
Each level of control should be tighter than the one that contains it. For example, flatness of a datum face should be tighter than its parallelism, which should be tighter than its location (size or profile) tolerance. A refinement that is looser than its parent adds nothing.
8. Modifiers and supplementary symbols
| Symbol | Meaning | Where | Example use |
|---|---|---|---|
| M | Maximum material condition (MMR in ISO 2692) | ASME + ISO | Clearance holes for bolts; allows bonus tolerance and functional gauging |
| L | Least material condition (LMR) | ASME + ISO | Protecting minimum wall thickness around a bored hole |
| P | Projected tolerance zone | ASME + ISO | Tapped holes and press-fit pins, where the mating bolt or pin extends beyond the part |
| F | Free state | ASME + ISO | Thin rubber, plastic or sheet parts measured unrestrained |
| T | Tangent plane | ASME + ISO | Controlling the contact plane of a face rather than every high and low point |
| U / UZ | Unequally disposed profile zone | ASME Ⓤ, ISO UZ | Profile tolerance that may only add material, for example on a casting |
| E | Envelope requirement | ISO (ASME has this by default via Rule #1) | Mating pins and bores on ISO drawings |
| I | Independency | ASME 2018 | Overriding Rule #1 on a specific feature |
| ST | Statistical tolerance | ASME | Stack-ups toleranced statistically, with process control |
| CF | Continuous feature | ASME | A shaft interrupted by a groove, treated as one feature |
| CZ / SZ | Combined zone / separate zones | ISO 1101 | Several surfaces in one common zone, or each in its own |
| Ø, SØ, R, SR, CR | Diameter, spherical diameter, radius, spherical radius, controlled radius | ASME + ISO (CR is ASME) | Size and zone shape |
| 25 | Basic dimension (ISO: theoretically exact dimension, TED) | ASME + ISO | Locating true positions and profile zones |
| (25) | Reference dimension | ASME + ISO | Information only, not inspected |
| Circle at leader bend | All around | ASME + ISO | Profile applying all around a contour in the view |
| Double circle | All over | ASME + ISO | Profile applying to every surface of the part |
| ↔ with letters | Between | ASME + ISO | Profile from point X to point Y only |
| n× | Number of places | ASME + ISO | 4× Ã˜6.6 for a four-hole pattern |
| ⌴ ⌵ ↧ | Counterbore / spotface, countersink, depth | ASME (ISO uses words or the same symbols per ISO 129-1) | Hole callouts |
Advertisement
9. Worked examples and calculator
All figures below were computed, not estimated. The rules used are stated with each example so you can check the premise as well as the arithmetic.
Example 1: Bonus tolerance on a hole
Given: hole Ø10.0 to 10.2, position Ø0.1 Ⓜ | A | B | C. Internal feature, so MMC = 10.0 and LMC = 10.2.
Rule: allowed position tolerance = stated tolerance + (actual size − MMC).
| Actual hole size | Bonus | Allowed position zone |
|---|---|---|
| Ø10.0 (MMC) | 0.0 | Ø0.1 |
| Ø10.1 | 0.1 | Ø0.2 |
| Ø10.2 (LMC) | 0.2 | Ø0.3 |
Virtual condition: 10.0 − 0.1 = Ø9.9. A fixed gauge pin of Ø9.9 at true position accepts every good hole.
Example 2: Checking a measured hole
A hole measures Ø10.15 and its axis is 0.06 off in X and 0.05 off in Y from true position.
Rule: positional deviation as a diameter = 2 × √(ΔX² + ΔY²) = 2 × √(0.06² + 0.05²) = Ø0.156. Allowed at Ø10.15 = 0.1 + 0.15 = Ø0.25. Result: accept.
The same 0.156 deviation on a hole at exactly Ø10.0 would be rejected, since only Ø0.1 is allowed at MMC. Also note that a ±0.05 coordinate tolerance would have rejected this hole outright, since ΔX = 0.06. A ±0.05 square zone has a diagonal of 0.141, and the Ø0.141 circle through its corners has 57% more area than the square. Every point of that circle is as far from true position as the square's worst corner, which is why position tolerancing gives usable extra tolerance.
Example 3: Bonus tolerance on a pin
Given: pin Ø7.9 to 8.0, position Ø0.05 Ⓜ | A | B. External feature, so MMC = 8.0.
| Actual pin size | Allowed position zone |
|---|---|
| Ø8.0 (MMC) | Ø0.05 |
| Ø7.95 | Ø0.10 |
| Ø7.9 (LMC) | Ø0.15 |
Virtual condition: 8.0 + 0.05 = Ø8.05.
Example 4: Fastener formulas (ASME Y14.5 nonmandatory appendix)
For an M6 screw (F = 6.0, the screw's MMC) through clearance holes of H = 6.4 at MMC (ISO 273 fine series), with zero clearance left over in the worst case:
- Floating fastener (clearance holes in both parts, nut on the end): T = H − F = 6.4 − 6.0 = Ø0.4 position in each part.
- Fixed fastener (clearance hole in one part, tapped hole in the other), equal tolerances: T = (H − F) / 2 = Ø0.2 in each part. Use a projected tolerance zone Ⓟ on the tapped hole, because tilt of the thread axis moves the screw where it passes through the clearance hole.
Assumptions: perfect orientation is not assumed for the fixed case unless Ⓟ is applied; the formulas give zero interference at worst case, not a design margin.
Bonus tolerance calculator
Enter sizes in mm. Uses the rules from Examples 1 to 3 with Ⓜ applied. The starting values are Example 2.
10. Key ASME vs ISO differences
| Topic | ASME Y14.5-2018 | ISO GPS |
|---|---|---|
| Size and form | Rule #1: envelope by default | Independency by default (ISO 8015); envelope only with Ⓔ |
| Size definition | Envelope plus local size | Two-point size by default; other size types by modifier (ISO 14405-1), such as GG, GX, LS |
| Concentricity, symmetry | Removed in 2018 | Retained in ISO 1101 |
| Projection | Third angle | First or third angle; first angle common |
| Datum feature symbol | Filled triangle | Filled or open triangle |
| Datum shift at MMB | Datum feature letter followed by Ⓜ means maximum material boundary | Same symbol, maximum material requirement applied to the datum (ISO 2692) |
| Unequal profile | Ⓤ | UZ |
| ± location of features | Allowed but discouraged for mating features | ISO 14405-2 treats ± on distances between features as ambiguous; use geometric tolerances |
| Dimension text | Unidirectional reading preferred | Aligned or unidirectional (ISO 129-1) |
| Decimal values | Metric: leading zero (0.5); inch: no leading zero (.5) | Leading zero; decimal comma or point by local practice |
Practical tip for suppliers working with both: when quoting or inspecting, write down the governing standard and edition from the title block first. If none is stated, ask before quoting a tight feature.
11. Common drawing mistakes
- No governing standard or edition stated, so nobody knows whether Rule #1 or independency applies.
- Using ± coordinates to locate mating holes instead of position from datums.
- Datum features chosen for convenience in measurement rather than function in the assembly.
- A position or orientation tolerance with no datum reference where one is needed, or datums referenced in the wrong precedence.
- Basic dimensions used without any geometric tolerance that refers to them, leaving the feature untoleranced.
- Applying Ⓜ to features that are not features of size, such as a flat face.
- Calling out concentricity on an ASME 2018 drawing.
- Over-tolerancing: tight values everywhere instead of on the features that carry function.
- Double dimensioning and closed dimension chains.
- Mixed projection: views laid out in one angle while the title block shows the other symbol.
- General tolerance note missing, or ISO 2768-mK used on new drawings without considering ISO 22081.
- No projected tolerance zone on tapped holes in a fixed-fastener assembly.
12. Self-check quiz
Try each question before opening the answer.
Q1. Which four GD&T characteristics never use a datum?
The form controls: straightness, flatness, circularity and cylindricity.
Q2. A pin is Ø12.0 to 12.1 with no geometric tolerance. It is bent but every two-point size reads Ø12.05. Good part?
Under ASME Y14.5 it may be rejected, because Rule #1 requires the pin to fit inside a perfect Ø12.1 envelope. Under ISO 8015 without Ⓔ it is accepted on size; form would only be limited by a stated form tolerance or general geometrical specification.
Q3. What is the virtual condition of a Ø20.0 to 20.2 hole with perpendicularity Ø0.05 Ⓜ to A?
MMC 20.0 − 0.05 = Ø19.95.
Q4. Why can runout not take Ⓜ?
Runout is measured with an indicator on a surface rotated about the datum axis. It controls the surface directly, so there is no size-dependent boundary to give bonus tolerance from. It is always regardless of feature size.
Q5. What replaces concentricity on an ASME 2018 drawing?
Position with a datum axis (often with Ⓜ for assembly), runout for rotating parts, or profile of a surface for non-cylindrical features.
Q6. Parallelism 0.05 to A is applied to a top face. Does that control the face's height from A?
No. Parallelism controls orientation (and flatness) only. Height is controlled by the size dimension or by a profile of a surface tolerance to A.
Q7. How do you tell first angle from third angle on a drawing?
Read the projection symbol in the title block. In third angle, the end view circles are on the right of the cone; in first angle, they are on the left.
Q8. What does ISO 2768-mK mean, and what should a new ISO drawing use instead of the K?
Medium class linear and angular general tolerances (ISO 2768-1) and class K general geometrical tolerances (ISO 2768-2). ISO 2768-2 was replaced by ISO 22081, so new drawings should state general geometrical specifications per ISO 22081.
13. Standards reference list
- ASME Y14.5-2018, Dimensioning and Tolerancing
- ASME Y14.5.1, Mathematical Definition of Dimensioning and Tolerancing Principles
- ASME Y14.100, Engineering Drawing Practices; Y14.24, Types and Applications of Engineering Drawings
- ASME Y14.1 and Y14.1M, Drawing Sheet Size and Format; Y14.2, Line Conventions and Lettering; Y14.3, Orthographic and Pictorial Views
- ASME Y14.36, Surface Texture Symbols; Y14.41, Digital Product Definition Data Practices
- ISO 8015:2011, GPS Fundamentals: concepts, principles and rules
- ISO 1101:2017, GPS Geometrical tolerancing: form, orientation, location and run-out
- ISO 5459:2011, GPS Datums and datum systems
- ISO 2692:2021, GPS Maximum material requirement (MMR), least material requirement (LMR) and reciprocity requirement (RPR)
- ISO 14405-1 and -2, GPS Dimensional tolerancing
- ISO 128 series, Technical product documentation: general principles of representation
- ISO 129-1, Presentation of dimensions and tolerances
- ISO 5456-2, Projection methods: orthographic representations
- ISO 5457, Sizes and layout of drawing sheets; ISO 7200, Data fields in title blocks
- ISO 2768-1, General tolerances; ISO 22081:2021, General geometrical and size specifications
- ISO 286-1 and -2, ISO code system for tolerances on linear sizes
- ISO 21920-1, Surface texture: profile, indication of surface texture
- ISO 273, Clearance holes for bolts and screws
Comments