DIY Dual Layer PCB

I've been making my own single layer PCBs for years, first chemically and now using a small CNC (isolation routing). Now I want to make an Arduino shield but I'm stuck on connecting the two layers. How do I go about making the interconnect between layers? Is there some trick for this? I use Eagle and it does the work but I don't know how to deal with a pin that has solder on both sides (interconnect). For instance, the shield header used to plug into the Arduino. Those are the only "components" on the bottom side, which is soldered on the top layer. With a regular component, like a resistor, I can easily solder both sides. But not under the header.

Any help will be greatly appreciated.

Thanks!

You can run a ULP that will place tRestrict circles around through-hole pads, which will prevent routing away from the pads on the top layer. Then there will be no need to solder these pads on the top side (where they are obstructed by parts).

I don't remember where this ULP is -- it might even be part of the ones that come with Eagle. Or you can just do it manually.

You can make manual vias by just inserting a wire into the via and soldering both layers, then trimming off the wire ends. I think LPKF actually sells some kind of rivets that you push in to the vias that can make this process a bit faster, but are likely to be expensive. Rather than worrying about vias like this, it might be easier to just forget about milling out the top layer and replacing all traces with wire jumpers that you solder in yourself. Clearly, you'd want to limit top-side routing in this case -- you can set the cost of top-side routing to be high in Eagle's autorouter (or route manually).

--
The Ruggeduino: compatible with Arduino UNO, 24V operation, all I/O's fused and protected

Generally when I mill out 2 layer boards, I ensure in the board design that all throughhole components are connected on the bottom only (apart from resistors and diodes which are easy to solder on both sides). The easiest way to change the design is to put a via hole next to the hole which needs soldering on the top. This via hole can have a piece of wire put through it and soldered on both sides, and the component can be soldered on the bottom.

RuggedCircuits:
You can run a ULP that will place tRestrict circles around through-hole pads, which will prevent routing away from the pads on the top layer. Then there will be no need to solder these pads on the top side (where they are obstructed by parts).

Beautiful and clean solution. Learning something new everyday, which when it comes to Eagle, it means I now know 0.2% instead of the 0.1% I knew yesterday! :slight_smile: I drew a (bRestrict) rectangle covering pins AREF down to D21 and so on (Mega) and it did it in 2 seconds what I had spent the whole day yesterday doing by hand. I had the top layer cost high and it created just a few vias, which I can easily just solder a piece of wire connecting both sides.

Thanks a zillion!