Enter `GND` (or whatever you have called your ground net) as the **Net** attribute of the vias and the traces you add.

Super! Thank you!

Hi Daniel, From your description, I'm guessing that: 1. the slots are in the ground on the bottom layer and 2. the slots are cause by traces on the bottom layer breaking the plane up so you're adding the 'bridge' traces on the top layer adjacent to the traces that are crossing the slots? Is that right? If yes, your plan seems like a good way to reduce EMC and signal integrity problems on a simple 2 layer PCB. * It might also be worth considering putting a copper area assigned to ground over the whole of the top layer and then dropping ground vias into it around wherever signal traces cross slots in the ground on the bottom layer. That way you may get a lower return path inductance without having to place individual tracks at each crossing point. This may also help you because you can move top layer traces if you see a better way to route over the slots and the copper area will move as you rebuild the them (though you'll still have to move the vias manually).

You are correct about what I am trying to do. I appreciate the suggestion of doing a ground fill on the top side of the board as well. Fortunately, the number of 'high-speed' signals is small and grouped together, so a couple of well-placed bridge traces should suffice. Thanks again for the excellent information and prompt response. ~ D

One more thought. If you are routing signals across a 2 layer board with fast enough edges to be worried about return paths then don't forget that the clearance you'll need to keep crosstalk down to acceptable levels is going to be > 3 times the height of the traces above the ground plane (not the more commonly quote 3 times the trace width: that assumes that the traces are much wider than their spacing to the ground plane). So if you're using a standard 1.6mm thick board, you'll need to keep any adjacent traces away by around 5mm. When crossing the gaps then they need to be even further apart (because the distance to the ground plane just went to a long way away!). Unless you don't care about the crosstalk between the adjacent traces (because they're all on the same synchronous bus with adequate setup and hold times) then it would be advisable to put grounds tracks so that there's one each side of every signal track. It's not a perfect solution but it will help. I'm assuming you aren't routing differential signals? If you are, have a look at my post here: https://easyeda.com/forum/topic/Differential_pairs_routing_tool-OPlDxPJ1j

Excellent tips, for sure. My signals are probably not changing quite that fast, but I'm kind of particular about how Things Should Be Done. :) My main concern isn't the signals being driven on the traces in question, but more about preventing the physical arrangement of the traces from picking up unwanted interference from outside sources. You are correct: these are not differential signals. ~ D