Intro to 3D modelling

Why it matters

Mechanical engineers design almost everything in 3D, civil and electrical engineers increasingly use 3D models (BIM, equipment layouts, cable trays), and maintenance teams use models to order parts and plan repairs. A 3D model is a single source of truth: drawings, 3D prints, CNC programs and assembly checks all come from it.

Parametric, feature-based modelling

Most mechanical CAD tools (SolidWorks, Inventor, Fusion, Onshape, FreeCAD Part Design) work the same way:

1. Sketch a 2D profile on a plane, fully constrained with dimensions.
2. Create a feature from it: extrude (FreeCAD calls it Pad), revolve, sweep or loft to add material, or cut (FreeCAD: Pocket) to remove it.
3. Add more features on faces of the solid: holes, fillets, chamfers, patterns.
4. The feature tree (history) records every step in order. Change a dimension early in the tree and everything after updates. That is what parametric means.

Design intent is the idea behind it: model the part the way it should change. If the holes must always stay 12 mm from the ends, dimension them from the ends, not from each other.

Free 3D tools

• Onshape free plan: runs in a browser, saves automatically, good tutorials. Documents on the free plan are public, so keep private designs out.
• FreeCAD: free and open source, installs locally. Use the Part Design workbench for feature-based solids.

Official sites: https://www.onshape.com/en/products/free and https://www.freecad.org/. Checked on 2026-10-23.

Worked example: the angle bracket in 3D

The bracket from lesson 7: an L 50 mm wide, 40 mm tall, 5 mm thick, 30 mm deep, with two Ø6 holes through the base.

Plan the model: one L-shaped profile extruded 30 mm, then holes, then fillets. Three or four features.

1. New part in millimetres.
2. Sketch on the front plane. Draw the L profile with the line tool starting at the origin: 50 along the bottom, up 5, back 45, up 35, back 5, down 40 to close. Add dimensions 50, 40 and 5 (twice) and constrain it fully; the corner sits on the origin.
3. Extrude (Pad) 30 mm. Use a symmetric extrude (15 mm each side of the sketch plane) if you want the front plane to be a plane of symmetry; it keeps later features centred.
4. Holes. Sketch on the top face of the base: two circles Ø6 with centres 12 mm from each end and centred in depth (a symmetric constraint or 15 mm from the edge). Extrude-cut through all (FreeCAD: Pocket, type "Through all"), or use the dedicated Hole feature, which records the hole as a hole for drawings.
5. Fillet the inside corner of the L with R3 to make it stronger and easier to manufacture.
6. Check: measure the model with the measure tool, rename features ("L profile", "Base holes", "Inner fillet") and set a material if the tool supports it to see the mass.
7. Change test: edit the first sketch and change the height from 40 to 50. The holes and fillet should update without errors. If something breaks, your references or constraints need fixing.

From model to drawing and file

• Make a 2D drawing from the model (Onshape: Drawing; FreeCAD: TechDraw) with front, top, side and isometric views; the dimensions come from the model.
• Export STEP to share with other CAD tools (the universal format for solids) and STL or 3MF for 3D printing.

Common mistakes

• Under-constrained sketches that shift when you edit later.
• Building everything in one complicated sketch instead of simple features.
• Dimensioning features from each other instead of from the edges or datums that matter.
• Referencing edges that disappear when an earlier feature changes, causing errors downstream.
• Sharing a native file when the other side needs STEP.

Recap

• Sketch, constrain, then extrude/revolve or cut; add holes and fillets as features.
• The feature tree makes the model parametric: change early dimensions and the rest updates.
• Capture design intent with good references and constraints.
• Export STEP for CAD exchange and STL/3MF for printing.

Try it

In the Do tab, model the bracket in Onshape's free plan or FreeCAD and test a design change.