Starting point
The four features that do most of the work
Extruded boss, extruded cut, revolved boss and revolved cut between them create parts with constant cross section — uniform-thickness components from the extrudes, axisymmetric components from the revolves. It is a widely quoted rule of thumb in CAD practice that these four features alone will generate the large majority of ordinary mechanical parts, on the order of four in five.
The parts they cannot create are those with variable cross section, non-planar faces, or geometry that has to follow a path. That is what the remaining feature set exists for.
Mastery of feature-based modelling reduces to being able to answer three questions: what features does the system offer, what input does each one require, and which feature is the right choice for the problem in front of you? The third question usually has several workable answers and one best answer.
Catalogue
The extended feature set
| Feature | Input required | Choose it when |
|---|---|---|
| Sweep | One profile plus one path; optionally guide curves and a twist specification. | The cross section is constant along a curved path — handles, tube runs, gaskets, coil springs. |
| Loft | Two or more profiles in different planes; optionally guide curves and centreline. | The cross section changes between stations — transitions, ducting, blended housings. |
| Hole wizard | Standard, fastener type, size, fit and end condition; placement sketch. | Any hole that a fastener will occupy. Produces standards-compliant geometry and a drawing callout in one step. |
| Rib | An open sketch line, thickness and draw direction. | Stiffening a wall without thickening it — essential in moulded parts. |
| Draft | Neutral plane or parting line, faces to draft, draft angle. | The part must release from a mould or die. See Part 20. |
| Shell | Faces to remove and wall thickness (uniform or per face). | Converting a solid into a thin-walled body — enclosures, containers. |
| Dome | A face and a height. | A smooth raised or recessed cap where a revolve would be clumsy. |
| Fillet and chamfer | Edges or faces, plus radius or distance and angle. | Stress relief, handling safety, tool-radius realism, mould release. Apply late in the tree. |
If the cross section is constant along a curve, a sweep is the better choice — it needs fewer inputs and produces a cleaner, more predictable result. If the cross section varies, a loft is required. Choosing a loft where a sweep would do is a common source of unnecessarily complex, fragile geometry.
Worked domain
Spur gears as a modelling problem
Gears illustrate the gap between buying a component and understanding it.
Gears come in many forms — spur, helical, bevel, spiral, worm, planetary, rack and pinion. The spur gear is the simplest, and it is worth constructing at least once even though gears are standard purchased items and can be dropped in from a component library.
The intricate part is the tooth. Meshing gear teeth must maintain a constant velocity ratio through the engagement, which requires a conjugate tooth profile. The involute curve satisfies that condition and is therefore the profile used almost universally in mechanical power transmission. From a CAD standpoint the practical consequence is that a correct gear tooth is not an arc — it is a generated curve, and modelling it properly means constructing that curve (analytically or from an equation-driven sketch) rather than approximating it with tangent arcs.
- Define Module or diametral pitch, tooth count, pressure angle, face width.
- Derive Pitch, base, addendum and dedendum circles from those inputs.
- Generate The involute flank as an equation-driven or constructed curve.
- Build One tooth space, then circular-pattern it around the blank.
- Finish Bore, keyway, hub and edge breaks as separate features.
This is a construction exercise, not a gear design exercise. Selecting module, face width, material and hardness against a duty cycle is a mechanical design calculation governed by strength and wear criteria, and it belongs outside the CAD system. Model the gear after it has been designed, not instead.
Reuse
Design libraries and library features
Design reuse is one of the cheapest available forms of productivity. Standard components — fasteners, bearings, gears, seals, structural sections — should almost never be modelled from scratch, and any company will additionally accumulate geometry that is standard within its own work but nowhere else.
Library features
A feature or group of features created once, saved to the library, and dropped into new parts thereafter. Typical candidates: proprietary keyway profiles, standard mounting-boss geometry, recurring cutout patterns.
Component libraries
Off-the-shelf parts inserted directly into assemblies at the correct size and standard. The associated fastener wizards will additionally select and place hardware to match a hole stack.
Governance
A library only pays back if it is curated. Uncontrolled growth produces several near-identical entries and destroys confidence in all of them. Assign ownership.
Families
Configurations and design tables
A direct consequence of parametrics: if a part is defined by parameters, the same definition can produce a family of parts.
Configurations are the family members. Each shares the topology of the original and differs in geometry — a longer boss, a wider flange, a different bore. Design tables, held as a spreadsheet embedded in the document, are the practical way to create and control them at scale.
Change sizes
Drive named dimensions from table columns, so a whole size range is defined in one readable grid.
Change state
Suppress or unsuppress features per configuration — an optional mounting lug present in three variants and absent in the fourth.
Change assembly relationships
In an assembly, tables can control component configurations, mate states, and distance or angle relationships between components.
Design tables reference dimensions and features by name. Renaming driving
dimensions to meaningful terms — Bore,
FlangeOD, Length — before building the table
turns an unreadable grid of system-generated identifiers into a document a
colleague can maintain.
Automation
Macros and the automation ladder
A macro is a short program that repeats a commonly performed sequence. It is generated by the CAD system itself, in the background, by recording actions between the moment recording starts and the moment it stops. Recorded macros can then be replayed, paused, edited, and bound to a toolbar button or keyboard shortcut.
Automation returns value in two ways: it raises throughput, and it removes the error rate associated with mundane repetition. The pragmatic rule is to automate a task once you have done it identically three times.
Automating a process that is still changing is how organisations end up maintaining code that enforces a workflow nobody follows any more. Stabilise the manual process first, then capture it.
Key takeaways
- Four features — extruded and revolved bosses and cuts — build most ordinary mechanical parts; the rest of the set handles variable sections and non-planar faces.
- Prefer a sweep to a loft where the cross section is constant along the path; fewer inputs means more predictable geometry.
- Use the hole wizard for any fastener hole: standards-compliant geometry and the drawing callout arrive together.
- Correct gear teeth are generated involute curves, not arcs — and gear design happens before, not inside, the CAD model.
- Configurations and design tables turn one parametric definition into a whole product family; name your dimensions first.
- Climb the automation ladder in order, and only automate processes that have stopped changing.
Series
Continue the pathway
The SOLIDWORKS Design Approach series works through computer aided design as an engineering discipline, from first principles to manufacture.