Technical Product
Documentation:
Convention & Practice

1.1 Terminology

• TPD: technical product documentation, including drawings, notes, specifications, revision control, and associated definition data (ISO 01.110 domain).
• GPS: geometrical product specification system used by ISO to define how geometry is specified and interpreted.
• Datum: theoretically exact reference derived from a datum feature and used for orientation or location.
• General tolerance: default tolerance that applies unless a tighter or different tolerance is explicitly stated.
• Feature control frame: the boxed symbol-and-value structure used in GD&T.

1.2 TPD Layout

Standardized sheet layouts guarantee that any stakeholder knows where to look for critical meta-information. ISO 5457 (and ASME Y14.1) defines sheet sizes and layout principles for technical drawing sheets. ISO 7200 defines the data fields required in the title block.

Sheet structure

• A drawing frame defining the clear working area.
• A minimum 20 mm border on the left (binding edge) and 10 mm on all other sides (per ISO 5457).
• A title block anchored at the bottom right.

Title block content (ISO 7200)

The title block identifies the drawing uniquely, states the release level, and provides the interpretation context needed to read the sheet. The following fields should be present:

• Drawing number: Unique identifier that does not change between revisions.
• Part or assembly title: Descriptive name for the object being defined.
• Revision identifier: Current revision index, matched to the revision table.
• Drawing scale: Applies to all views on the sheet; any individual view at a different scale must note it locally above that view.
• Sheet number and total sheet count: e.g. Sheet 1 of 3.
• Projection method symbol: First-angle (ISO/European) or third-angle (ASME/US) per ISO 5456-2 / ASME Y14.3.
• Material specification: Material grade and standard (e.g., EN AW-6082-T6 per EN 573-3).
• Default surface finish: Often stated in the title block if applicable globally.
• Signatures: Drawn by, checked by, and approved by fields with dates.

1.3 Drawing Rules

ISO 128 (consolidated 2020/2022 updates) provides the general rules for graphical representation, including lines, cuts, views, and sections. ISO 129-1 defines dimension presentation. (The equivalent US overarching standard is ASME Y14.100 along with ASME Y14.2 and Y14.3).

Per ISO 128-3:2022 and ASME Y14.3, orthographic representation should use either First Angle Projection (viewer looks through object to projection plane) or Third Angle Projection (viewer looks directly at object with projection plane in between). Both norms mandate that the cutting plane be clearly identified (e.g. A-A) and cross-hatched appropriately for the material if necessary.

1.4 GD&T Fundamentals

ISO 1101:2017 (and its US counterpart ASME Y14.5) defines the symbol language for geometrical tolerancing and the rules for interpreting tolerances of form, orientation, location, and run-out.

Feature control frame logic

Every feature control frame strictly identifies what is being controlled, the tolerance zone shape (e.g. diameter symbol if cylindrical), the tolerance value, and the applicable datum reference frame.

GD&T symbols overview

Table 1 – GD&T symbols, meaning, and datum use

1.5 Standards Overview

The following standards form the backbone of technical product documentation definitions. A standard should only be cited on a drawing when its rules are directly used — citing an unused standard gives the false impression of compliance and creates an unnecessary checking burden.

Table 2 – Standards reference guide

2.1 Dimensioning Strategy

Dimensioning order

1. Dimension functional interfaces first.
2. Dimension features that control assembly or fit second.
3. Dimension manufacturing-critical features third.
4. Leave non-critical geometry to general tolerances.

Minimum-dimensioned TPD

A minimum-dimensioned drawing carries the dimensions necessary for manufacture, verification, and functional acceptance, while pushing repetitive geometry definition out of the way.

• Use direct dimensions for critical interfaces and envelope-defining features.
• Let the declared general tolerance standard (e.g. ISO 2768-mK) handle unspecified non-critical dimensions. Do not restate those dimensions with individual tolerances unless there is a functional reason to override the default.
• Do not restate geometry multiple times in different views simply because space is available.

2.2 GD&T Application Guidance

• When to apply: Apply GD&T to features where fit, function, or interchangeability depends on geometric control — for example: mounting faces, bearing bores, locating pin holes, sealing surfaces, and mating flanges. Avoid adding GD&T indiscriminately to non-critical geometry.
• Datum selection: Datums should be derived from features that function as real references in assembly or inspection. A three-datum reference frame follows the 3-2-1 principle: the primary datum constrains three degrees of freedom (typically the largest flat face or main bore axis), the secondary datum constrains two (a long edge or locating bore), and the tertiary datum constrains the last one (an end face or secondary feature).

FCF selection flowchart

The feature control frame should be chosen from the simplest control that fully protects function. Do not jump to profile when a simpler form or orientation control already defines the requirement.

2.3 Multiple parts on a single drawing

For assemblies, the documentation strategy is generally an internal workflow decision rather than a strict ISO mandate, though best practices apply.

Detailing and documentation recommendation

As a standard rule, always prefer to create a separate, detailed drawing for each individual part. This ensures proper revision control, procurement traceability, and absolute clarity for manufacturing.

A possible exception to this rule is a weldment that explicitly only makes use of parts that can be manufactured using a cut list (such as standard stock profiles and tubes). In these specific cases, a main fabrication drawing supplemented by a comprehensive cut list may suffice.

2.4 Revision Practice

A revision system works best when the change history and the changed geometry are both easy to find on the drawing.

• Use one revision identifier format across the company. Common options are alphabetic (A, B, C…), numeric (1, 2, 3…), or alphanumeric (A1, A2, B1…). The active revision in the title block must always match the current row in the revision table.
• Place the revision table near the title block or upper-right sheet area so it is easy to find.
• Use revision clouds only to highlight the changed area, not to replace the written change description in the table.
• Place the revision symbol close enough to the change that the intended modification is obvious during review.
• Remove obsolete clouds when a new baseline issue is released.

Table 3 – Example recommended revision table structure

2.5 Drawing Conventions

Drawing titles and naming

• A drawing title should be brief, describe the item, and distinguish it from similar items.
• Use a noun or noun phrase followed by a modifier to group similar parts together in sorted lists (e.g., use "BRACKET, MOUNTING" or "GEAR, SPUR, 80 TOOTH" rather than "Mounting Bracket").
• Avoid vague nouns alone (e.g., "PLATE") without a functional modifier.

Letter reservations

These conventions work well in practice and reduce visual ambiguity on dense drawings:

• Datums: start with A, B, C for primary datum structure (reserve A–E).
• Section views: use repeated letters in order, e.g. A-A, B-B, C-C. (Reserve F–W).
• Detail views: use single-letter or alphanumeric detail labels such as Detail X, Detail Y. (Reserve X–Z).
• Avoid I, O, and Q to reduce confusion with 1 and 0.

View strategy

• Define one preferred front-view selection rule: use the view that best explains the part's function and its main interfaces.
• Always keep auxiliary and section views in line with the default orthographic projection system (first- or third-angle) to prevent reading errors.
• If a view must be moved out of direct alignment due to space constraints, it must be clearly identified (e.g., VIEW A) and a bounding box should be drawn around it to explicitly signal that it is out of projection.
• Use the minimum number of views necessary to fully define the part.
• Prefer section views over complex webs of hidden lines.

Text and notes

• Keep all default notes standardized in one notes block.
• Put general tolerances in the title block or note block, not repeated in multiple places.
• Use one approved phrase list for standard notes such as deburr, finish, coating, sharp edge break, and unspecified radius treatment.

2.6 Process Defaults

Different manufacturing routes often benefit from different default note sets, tolerance strategies, and inspection priorities. Standardising these internally reduces repeated drafting decisions.

Table 4 – Recommended default approach by process

2.7 Typical Note Sets

To ensure consistency and avoid drafting omissions, standard notes should be pre-populated in the drawing template. Below is a refined, modular approach to standard notes.

Universal foundation notes (All drawings)

1. ALL DIMENSIONS ARE IN MILLIMETERS UNLESS OTHERWISE SPECIFIED.
2. DO NOT SCALE DRAWING. GEOMETRY DRIVES TOOLPATHS.
3. UNLESS OTHERWISE SPECIFIED, GENERAL TOLERANCES APPLY PER ISO 2768-[class].
   (Note: While mK is the recommended default for general machining, the engineer should adjust these classes based on the specific part's manufacturing process—e.g., changing to c or v for rough fabrication, or f for precision work.)
4. GEOMETRICAL TOLERANCING APPLIES PER ISO 1101.
5. SURFACE TEXTURE INDICATIONS APPLY PER ISO 1302.

Process-specific additions

For Machined Parts:

6. UNSPECIFIED EDGES TO BE BROKEN OR DEBURRED PER ISO 13715 (SEE TITLE BLOCK SYMBOL).
7. MACHINED SURFACES TO BE FREE OF OIL, COOLANT, AND CHIPS PRIOR TO PACKAGING.

For Weldments:

6. GENERAL WELDMENT TOLERANCES APPLY PER ISO 13920 - CLASS B/F.
7. WELDING SYMBOLS PER ISO 2553. WELD QUALITY LEVEL PER ISO 5817 - CLASS C.
8. REMOVE ALL WELD SPATTER AND SLAG PRIOR TO FINISHING.

2.8 Quick Self-Check