Design a Parametric Electronics Enclosure, Step by Step

What we are making

A 100 x 60 x 40 mm open-top box with 2 mm walls, 5 mm rounded corners, four screw bosses for an M3 lid, and a slot for a cable. It takes ten features.

Step 1: the outer block

1. Start a new CAD part and sketch on the Top plane.
2. Draw a centred rectangle 100 x 60 mm.
3. Extrude it 40 mm. This is "Box".
4. Add a Fillet of 5 mm to the vertical edges for rounded corners.

Step 2: hollow it out

Add a Shell feature with 2 mm thickness and remove the top face. The box becomes an enclosure with even walls everywhere, and the rounded corners carry through to the inside.

Step 3: screw bosses

1. Sketch on the Top plane, offset 2 mm (the inside floor).
2. Draw four circles of 3.5 mm radius at x ±42, y ±22.
3. Extrude them 30 mm with "add" so they join the floor.
4. Sketch four points on top of the bosses (Top plane, offset 32) and add a Hole of 2.5 mm, 20 mm deep: the pilot holes for M3 screws.

Step 4: a cable port

Sketch on the Front plane, offset 30 mm (the outer face of the front wall), draw a slot 16 mm long with 4 mm radius, and extrude it 10 mm into the box with "remove".

Change it for your board

This is where parametric CAD pays off. Need a bigger box? Change the 100 x 60 rectangle in the first sketch, move the boss circles, and everything else follows: the shell, the fillets and the holes. Need thicker walls for a stronger print? Change the shell thickness.

Or describe it to the AI

In VIZON you can type "an electronics enclosure 100 x 60 x 40 mm with 2 mm walls, open top, rounded corners and four M3 screw bosses" and get the same kind of feature list to refine.