Connecting two nets in Eagle

Question

I'm designing a schematic and board in Eagle 9.4.0. I have couple different power nets: signal 5V, power 5V (for servos) and power 8V (from battery). I'd like the power nets to be wider than others, so I designed specific net class for them. Matching GND nets will also be wider than others.

The problem is that I want all GNDs to connect at some point. However, when I connect nets (for instance, using a net junction), Eagle asks me, whether I want to merge nets and this is not what I want to do, since I'll have to choose one of two net classes for merged net.

How can I merge two nets in Eagle?

Answer 1

You rename them into one single name. That's all.

If you want to keep the different names and properties and simply connect them, use a zero-ohms resistor. You can design such an element consisting of two pads and a track yourself.

Answer 2

Janka's suggestion of zero-ohm resistor (or jumper) is a good one.

If, for some reason, you don't want to do that, I've seen people draw a copper rectangle on the PCB which overlaps both nets. This works, but it has a few drawbacks:

1. It doesn't show up on the schematic, so you should make note of it manually.
2. It will cause DRC errors, which you can ignore (or dismiss)
3. You need to use a "rectangle", not a "polygon". A polygon is assigned a net name, and so will pull away from other nets. But a rectangle is unnamed, and can be forced to overlap multiple nets.

Even with these issues, this seems to be a common practice.

Answer 3

"I'll have to choose one of two net classes for merged net"

So what? Unless you are auto-routing, the traces will stay the same if you change the net name(s) after the routing is done. You may get some PCB checking errors for width but you can Accept those.

Answer 4

The best way to do this is to "short" the net. You can do this by adding "shorts" from short library in Eagle. This would place a rectangular pad(different size available) in the board and will connect two net, easy.