Extrusion
Constant cross section along an axis, uniform thickness. One sketch in one plane, extruded perpendicular to it. The overwhelming majority of brackets, plates and covers.
Classification
Four types of CAD model
From a creation point of view every part falls into one of four classes, and the class determines the build strategy.
Revolve
Axisymmetric: a constant profile swept through an angle about an axis. One sketch containing both the profile and the axis of revolution.
Composite
A combination of extrusions and revolves, often with patterns. Most mechanical hardware sits here. Build order matters more than in the simple cases.
Free form
No uniform shape — an automotive panel, a hand tool grip, a mouse. Requires multiple sketches in multiple planes and the curve and surface techniques covered in Parts 11 and 12.
Reading the clues
Before touching a sketch, ask four questions. What type is this part? Is it symmetric — can half be built and mirrored? Does it contain a repeated feature that a pattern can generate? And which points already exist in the geometry (ends, midpoints, intersections) that can be snapped to instead of calculated? Answering these four before starting typically halves build time.
Foundations
Solid model topology
A solid model is the most complete geometric definition of a part. Its structure has a formal vocabulary and a validity test.
- Body (B)
- The solid itself. A model may contain more than one disjoint body, which matters for Boolean operations and for weldment and multi-body workflows.
- Face (F)
- A bounded surface, planar or non-planar. Faces meet at edges.
- Edge (E)
- A bounded curve, which may be a straight line. Edges meet at vertices.
- Vertex (V)
- A point — in practice, a corner.
- Loop (L) and ring (R)
- A loop is a closed set of contiguous edges bounding a region of a face. Every face has one outer loop; additional inner loops are rings, and each ring appears visually as a hole in that face.
- Genus (G)
- The number of through holes in the solid — a hole in three dimensions rather than a hole in a face. A washer has genus one.
The validity test
A topologically valid solid satisfies the Euler–Poincaré relation, which links the element counts to the number of shells (S) and the genus:
V − E + F − R = 2(S − G)
where R counts only inner loops (rings), S counts the closed shells bounding the solid, and G is the genus.
| Solid | V | E | F | R | S | G | V−E+F−R | 2(S−G) | Valid |
|---|---|---|---|---|---|---|---|---|---|
| Plain rectangular block | 8 | 12 | 6 | 0 | 1 | 0 | 2 | 2 | Yes |
| Block, one square through hole | 16 | 24 | 10 | 2 | 1 | 1 | 0 | 0 | Yes |
| Block, two square through holes | 24 | 36 | 14 | 4 | 1 | 2 | −2 | −2 | Yes |
Designers never evaluate this by hand in practice — the modelling kernel enforces it, which is precisely why a CAD system will refuse to produce an invalid solid and will report a failure instead. The value in knowing the relation is diagnostic: when a Boolean or a thicken operation fails, it is usually because the requested result would not be a valid closed solid.
Core concept
Parameters and dimensions are not the same thing
A parameter is a variable that can take any value. A dimension is a specific numerical value currently assigned to a parameter. Parametric systems define geometry in terms of parameters, and dimensions are simply the present state of those parameters. Change the values and the model regenerates.
Ease of editing
The dominant benefit. Sketch freely, dimension afterwards, and change dimensions until the shape is right. Conceptual design becomes far less committal.
Families of parts
Identical topology, different geometry. One definition can produce a whole size range — the basis of configurations and design tables, covered in Part 07.
Relations between parameters
Equations such as length = 2 × width encode design
intelligence directly into the sketch, so that intent survives editing.
Practical consequence
Because the system creates parameters as you sketch, there is no need to know the dimensions before starting. Sketch the shape approximately, then let the dimensioning step define it. Beginners frequently do the opposite — fighting to place every entity precisely by eye — and lose a great deal of time to it.
Working vocabulary
The control set inside a sketch
A handful of mechanisms do nearly all the work of holding geometry where it belongs.
| Mechanism | What it does | Use it when |
|---|---|---|
| Sketch relations | Constrain entities to one another: horizontal, vertical, parallel, perpendicular, tangent, concentric, equal, collinear. | The relationship must survive a dimension change. |
| Equations and link values | Drive one dimension from another arithmetically, or force several dimensions to share a single value. | A proportion or a repeated size is part of the design intent. |
| Construction geometry | Reference entities that guide the sketch without generating material. | Centrelines, mirror axes, bolt-circle references, layout skeletons. |
| Reference geometry | Planes, axes, points and coordinate systems created for the model rather than inherited from the default set. | A feature must be built on something that does not yet exist as a face. |
| Patterns | Reproduce a feature linearly, circularly, along a curve, by mirror, or from a table of positions. | The repetition is real design intent — a bolt circle, a vent array. |
| Sketch status | Reports whether a sketch is under-defined, fully defined or over-defined. | Always. Fully defined sketches are the goal for production models. |
Under-defined is not free
An under-defined sketch has degrees of freedom that nothing controls. It will look correct and will move unpredictably when an upstream dimension changes. Over-defined sketches are noisy but honest; under-defined sketches fail quietly. Drive production sketches to fully defined.
Signature artefact
The feature tree as a modelling plan
Each new feature is added to or subtracted from what already exists, so at any instant there is a single combined result. The tree is the record of how that result was reached.
- Plate
Renamed from the default. A reader now knows what it is.
- Front Plane Chosen because the plate is dimensioned in front view on the drawing.
- Sketch1 — outer profile, fully defined Centre rectangle from the origin, so the part stays symmetric about the origin when resized.
- Mid-plane extrude, 12 mm Built about the sketch plane rather than from one face, so the sketch plane remains a valid mirror plane.
- Bolt Holes
A patterned feature, not four separate cuts.
- Sketch2 — single hole on a construction circle
- Circular pattern, 4 instances, equal spacing Changing the count is now one edit, not four.
- Edge Break Fillets and chamfers last, so earlier features reference clean edges.
Two habits make trees readable. Rename features to describe what they are rather than how they were made, and keep cosmetic operations — fillets, chamfers, draft — near the end so that the structural features above them reference unrounded geometry. Part 06 develops this into a full treatment of design intent.
Underlying mathematics
Boolean operations
Booleans are the set-theoretic functions the kernel uses to combine bodies. They are implemented on top of surface-to-surface, curve-to-curve and curve-to-surface intersection.
Union
The sum of two bodies. Selection order is irrelevant.
Intersection
The overlapping volume common to both. Selection order is irrelevant.
Subtraction
What remains of the target after the tool body is removed. Order is critical: subtracting A from B is not the same as subtracting B from A.
The vocabulary is borrowed from machining deliberately: the body you subtract from is the target, the body doing the subtracting is the tool. By default most systems merge each new feature with the previous result, giving a single body at all times. Switching that merge off produces multiple bodies, which is what makes explicit Boolean work possible — and is the standard route to creating moulding, casting and forming tools from a finished part shape, as Part 20 shows.
Best practice
Modelling management in practice
Build off centre planes
Extruding symmetrically about the sketch plane keeps that plane usable as a mirror reference for the life of the model.
Standardise with templates
Set units, dimensioning standard, annotation styles and material defaults once, save as a template, and start every new document from it. This removes an entire class of downstream drawing inconsistency.
Prefer relations to dimensions
Where a relationship is the intent — tangency, concentricity, equality — capture it as a relation. A dimension that happens to produce tangency today will not produce it after the next edit.
Pattern rather than copy
Copied features are independent and must each be edited. Patterned features carry a single definition and an instance count.
Key takeaways
- Classify the part — extrusion, revolve, composite or free form — before choosing a build.
- Topology has a formal validity condition; failed operations usually mean the requested result would not be a valid closed solid.
- Parameters define shape, dimensions supply current values; separating the two is the whole point of parametric modelling.
- Relations, equations and construction geometry hold intent; dimensions alone do not.
- Drive production sketches to fully defined, and keep the feature tree readable by renaming features.
- Booleans are order-sensitive for subtraction and are the standard route to tooling geometry.
Series
Continue the pathway
The SOLIDWORKS Design Approach series works through computer aided design as an engineering discipline, from first principles to manufacture.
KEVOS®
Precision to Vision
Engineering · Mechanical Engineering
Written by Kevin Jogin
7 min read