Etching homebrew PCBs - design

One question we're asked - quite regularly, but especially after posting anything with a custom PCB - is how we make our homebrew boards. So we'll do a complete run-down of making a board, from design to printing and transfer, through to etching and drilling.

The first thing is to design the board properly.
For this, we use ExpressPCB. It's not Eagle. It's easier to use than Eagle. But it does a lot of things differently. If you must use Eagle, then use Eagle. But there are a couple of things to pay particular attention to - and very few people do, so play close attention!

First up, avoid square corners.
It's amazing the number of designs available online that use "square" corners.

When performing the toner transfer, you could end up with "weak points" across square corners - this is where the toner might easily flake off during etching, making the traces very thin at the square corner points. It's also easier to under-cut on a square corner than one "rounded-off" with a 45-degree section.

Secondly, use large pads and thick traces.

Those nasty "lozenge" shaped pads in Eagle might look cool - but drill one out of a homebrew board and it's very easy to separate the two parts of a pad with the hole. Make your pads big and round.

We use 2.03mm pads with a 0.89mm hole. Even if we have to go up to a 1mm drill bit, this still leaves plenty of copper around the entire hole once it's been drilled.

We tend to stick with 0.5mm traces for single sided boards. If the traces are going to SMT components (soic or 1206-sized pads/pins) we sometimes go down to 0.38mm. The smallest trace we'd normally try to etch is not less than 0.3mm.

Also, use "copper pour" or "fill plane" where available.

Your finished board might look cool with just the traces on it, but that leaves an awful lot of exposed copper on your board for the ferric chloride to have to etch away. More copper not only means a longer etching time, it also means you're using up your ferric chloride much more quickly than you need to.

A filled plane or copper pour with clearance of around 0.8mm not only gives your board a nice finish, it means far less copper actually has be etched away. Which in turn means faster etching - and in the longer term, your etchant lasts much, much longer.

When making boards for through-hole components, we print our single-sided designs directly from ExpressPCB. This means that when the design is copied onto the copper clad board, it arrives "flipped". But since the design is for the underside of the board, not the top, this is exactly what we want anyway.

When making boards for SMT components, we want the final board to look exactly as it does on-screen. To achieve this, we print our designs from inside Robot Room's Copper Connection software. This does a great job of flipping the design before sending it to the printer - which means after the toner transfer stage, the flipped design appears the right-way-around on the copper clad board.