Parametric CAD

Why it matters

In Technical Drawing & CAD Basics you sketched shapes and turned them into solids. Professional CAD goes one step further: the model remembers why it has its shape. If the customer asks for a bracket 10 mm wider, or the bolt changes from M6 to M8, you change one number and the whole part, its drawing and the assembly update. That is parametric modelling, and it is how almost all mechanical design work is done in tools such as SolidWorks, Creo, Inventor, Fusion, Onshape and FreeCAD.

The core ideas

Sketches, constraints and dimensions. A sketch is a 2D profile on a plane. Geometric constraints fix relationships (horizontal, parallel, tangent, coincident, symmetric, equal). Dimensional constraints fix sizes and positions. A sketch is fully defined when nothing can move without breaking a constraint; most tools show this by changing the line colour (for example, from blue to black in SolidWorks and Onshape, or green in FreeCAD's Sketcher).

Features. Each solid operation (extrude/pad, revolve, cut/pocket, hole, fillet, chamfer, pattern, mirror) is a feature that builds on the ones before. The ordered list is the feature tree (or history).

Variables and equations. You can name key values, such as thickness = 6 mm or hole_spacing = 40 mm, and drive dimensions with them or with expressions like width = hole_spacing + 2 * edge_distance. Onshape calls these variables (and Configurations for families of parts); FreeCAD uses expressions and spreadsheets or VarSets.

Design intent. The skill is not clicking tools; it is choosing constraints that behave sensibly when something changes. Ask: what should stay fixed, and what should follow?

Worked example: an L-bracket

Suppose you need a 90° bracket to hold a small motor to a frame with two M6 bolts.

1. Name the drivers: t = 6 mm (thickness), w = 50 mm (width), leg = 60 mm, bolt_d = 6.6 mm (an M6 clearance hole, medium fit per ISO 273), edge = 12 mm (hole centre to edge).
2. Sketch the L profile on the side plane, constrained to the origin, with the leg lengths set to leg and the thickness set to t on both legs (use an equal constraint so you only change one number).
3. Extrude the profile by w, symmetric about the mid plane, so the part stays centred if the width changes.
4. Add the holes with a Hole feature, positioned from the edges by edge and spaced w - 2 * edge apart. Because the spacing is an expression, changing w moves the holes correctly.
5. Add an inside fillet of radius t at the bend to reduce stress concentration (and to match how sheet or bent parts are made).
6. Test the intent: change w to 70 and t to 8. If anything breaks, flips or ends up in the wrong place, your constraints are not capturing the intent yet.

Good habits

• Sketch simple, add detail with features. Put fillets and chamfers in their own features near the end, not inside the sketch. They are the features most likely to fail when geometry changes.
• Reference stable geometry. Constrain to the origin and default planes, not to edges created by later features. Edges referenced by later features can be renamed internally when the model changes, causing the "topological naming" breakages FreeCAD users know well.
• Name features and variables. Pocket003 tells nobody anything; motor_mount_holes does.
• Fully define every sketch. An under-defined sketch can shift silently when you edit something else.
• Model in real units and real sizes. Use the units you will manufacture in and real standard sizes (hole sizes, material thicknesses).

Free tools

• Onshape (browser-based) has a free plan for hobby and non-commercial use. Documents in the free plan are public, so never put an employer's or client's design in it. Check the current plan terms on onshape.com. Checked on 2026-10-23.
• FreeCAD is free, open source and runs on Windows, macOS and Linux. Its Part Design workbench covers sketch-based solid modelling.

Common mistakes

• Over-constraining. Adding a dimension that conflicts with an existing constraint. The tool will complain; delete one rather than forcing it.
• Dimensioning to the wrong thing. Dimension the hole position from the edge the assembly cares about (the datum), not from whatever edge was handy. The next lesson explains datums.
• Building everything in one sketch. Huge sketches are fragile and hard to edit.
• Never flexing the model. If you have not changed the drivers, you do not know whether the model is really parametric.

Recap

• Parametric models are driven by constraints, dimensions and named variables.
• The feature tree is a recipe; order and references matter.
• Design intent means the model changes the way the design should.
• Test every model by changing its key parameters.

Try it

On the Do tab, build the L-bracket in Onshape or FreeCAD, drive it with variables and check that it updates cleanly.