Purpose
Two reasons drawings still matter
The first is documentation: a drawing is how a design is recorded in a form that survives software versions, staff changes and company boundaries. The second is communication: it remains the de facto standard interface between design and every downstream function — manufacturing, tooling, production, inspection, purchasing and assembly.
Model-based definition is steadily displacing some of this, but the reasoning does not change. Whether the tolerance is written on a sheet or attached to a face in a 3D annotation, someone has to decide what it is, and the rules that govern that decision are the same.
The same discipline that applies to sketches applies to drawings. A drawing
that omits a needed dimension forces the machinist to invent one. A drawing that
repeats a dimension creates two sources of truth and the possibility of
contradiction. Aim for a fully defined drawing. Where a redundant dimension
genuinely helps the reader, mark it as reference — the abbreviation
REF or parentheses around the value.
Governing rules
Drafting and dimensioning conventions
Both ANSI/ASME and ISO committees publish the conventions. The rules below follow the ASME line; ISO practice differs in detail rather than intention.
Drafting rules
Every dimension carries a tolerance
Stated explicitly, inherited from a general note, or inherited from the title block. The only exceptions are dimensions marked as reference.
Define each feature fully, once
Enough dimensions to be unambiguous, and no more. Minimise reference dimensions. There must be exactly one way to read the drawing.
Follow functional requirements
Select and arrange dimensions to match how the part functions and mates, not how it happened to be modelled. This is where design intent becomes visible to manufacturing.
Do not specify the process
Define the required result, not the method used to reach it. Specifying “drill” where a hole is required removes the manufacturer's freedom to choose a cheaper equivalent process.
Dimension types
| Type | Describes | Notes on use |
|---|---|---|
| Cartesian | Horizontal and vertical extents in the view plane. | The default for prismatic geometry. |
| Radial | Radius or diameter of an arc or circle. | Diameter for full circles, radius for arcs — and the choice is a design-intent decision, not a stylistic one. |
| Angular | An angle between features. | Watch tolerance accumulation over long angular chains. |
| True length | A length along a line that is neither horizontal nor vertical. | Preferable to decomposing into two Cartesian dimensions when the oblique length is what is functionally controlled. |
| Ordinate / baseline | All dimensions in one direction, measured from a single reference face or datum. | Eliminates chain accumulation. Use as few datums as possible — each additional datum is another face that must be machined accurately. |
Abbreviations
Abbreviation practice is governed by its own standard, and the standard's own stated purpose is to make abbreviations consistent rather than to encourage them. Four working rules follow from that: minimise their use; avoid them entirely on drawings that will cross language boundaries, since abbreviations are language-dependent; use them only where they genuinely save space and remain unambiguous; and check for duplicates, because the same short form can carry more than one meaning.
Geometry of views
First angle and third angle projection
A CAD system generates two-dimensional views by projecting the model onto a projection plane. There are two conventions, and they are mirror opposites of one another. Third angle projection produces the front, top and right views; first angle projection produces the back, bottom and left views. Both yield correct orthographic representations; they simply arrange them differently.
Third angle
Standard practice in the United States and Canada. The view appears on the same side as the direction from which it is observed.
First angle
Standard practice across Europe and much of the rest of the world, including common use in Australian industry alongside third angle. The view appears on the opposite side.
A drawing read in the wrong convention produces a mirror-image part. The projection symbol in the title block is not decoration — it is the single piece of information that makes the rest of the sheet interpretable. Set it deliberately in the sheet properties and confirm it on every template.
View types
Choosing views that answer questions
A typical drawing carries front, top and right views, often with an isometric added for readability. Anything beyond that should earn its place.
- Named orthographic views
- Front, top, right, back, bottom, left. The structural backbone of the sheet.
- Section view
- Cuts through the model to reveal internal geometry. The cut may be straight or stepped, and is defined by a section line whose direction the system requires.
- Projected view
- Derived by projecting from an existing view, preserving the projection convention automatically.
- Detail view
- An enlarged region, used where a feature is too small to dimension legibly at sheet scale.
- Auxiliary view
- Projected normal to an inclined face, so that face appears in true shape and can be dimensioned honestly.
- Broken and break-out views
- Shorten a long uniform part, or remove a region of material to expose what is behind it, without a full section.
- Exploded assembly view
- Components displaced along assembly axes to show the build order and relationships. Usually taken from the isometric.
Sheet management
Sheets, templates and the title block
A drawing may contain several sheets. Multiple sheets let a single drawing file carry more views than one sheet can hold — standard orthographic and isometric views on the first, a detail and a section on the second, an exploded assembly view on a third — without fragmenting the documentation across several files.
Creating a drawing opens a template, which consists of the sheet itself plus the sheet format. The format holds the border, the title block and the projection symbol, and can be saved and reused. Title block fields are typically linked to custom properties rather than typed, so that part number, description, material, revision and author flow automatically from the model.
Link title block fields to properties held at part or assembly level, and the same information populates the drawing, the bill of materials, the file metadata, the PDM record and any downstream report. Type it into the title block directly, and it has to be corrected in every one of those places separately.
Assembly documentation
Bills of materials
The bill of materials is a table, most often placed on assembly drawings and tied to balloons on the views. A default BOM carries four columns — item number, part number, description and quantity — each linked to properties held in the assembly itself, so that any change at assembly level flows through automatically. Item numbering follows the order in which components appear in the assembly.
Columns can be added, replaced or re-linked to other properties: material, mass, supplier, finish, cost code. The table behaves much like a spreadsheet, with the usual row and column operations available.
Indented versus parts-only
An indented BOM shows subassembly structure; a parts-only BOM flattens it. Choose according to who reads the sheet — the assembler or the buyer.
Balloon discipline
Every BOM line should appear as a balloon on the view, and every balloon should resolve to a line. Auto-ballooning is fast but should be checked.
Purchased items
Fasteners and bought-in components need supplier part numbers, not modelled geometry descriptions. Set this in the component properties, once.
The critical property
Model–drawing associativity
Associativity links edits in both directions. Modify the model and its drawing views update; change a model item dimension on the drawing and the model updates. It applies to model item dimensions — those imported from the part — and not to dimensions drawn independently on the sheet.
The property can be controlled per dimension. Marking a sketch dimension for drawing use determines whether it will be available as a model item; turned off, the dimension simply will not appear when model items are inserted. That control is worth using deliberately: a drawing populated with every construction dimension the modeller happened to create is unreadable.
The most common way associativity is lost is not a software failure but a process one: someone edits a PDF, marks up a print, or re-draws a view manually because it was faster. From that moment the organisation has two definitions of the part and no reliable way to know which is current.
Assurance
The design checker role
Many organisations designate someone to check drawings before release. The checker sits between engineering and manufacturing and typically holds experience in both. Automated design checking tools exist and are useful for standards conformance, but they check conformity, not judgement.
- Check 1 Can the documented design be produced at the least manufacturing cost?
- Check 2 Are there inconsistencies in the part dimensioning?
- Check 3 Can the specified tolerances actually be produced by the available processes?
- Check 4 Does the dimensioning scheme follow the standard and the functional intent?
- Check 5 Is material specified?
The outcome is binary: return to engineering for correction, or sign off and release to manufacturing. Formalising that gate — and giving the checker real authority — removes a category of expensive downstream surprise.
Key takeaways
- Drawings serve documentation and communication; both survive the shift to model-based definition.
- Fully define the sheet: no missing dimensions, no duplicates, reference dimensions clearly marked.
- Dimension for function and mating, not for the order in which the model was built.
- Declare the projection convention — misreading it produces a mirrored part.
- Link title block and BOM fields to custom properties so information is entered once.
- Protect associativity: the drawing must be generated from the model, never maintained beside it.
Series
Continue the pathway
The SOLIDWORKS Design Approach series works through computer aided design as an engineering discipline, from first principles to manufacture.