0
\$\begingroup\$

I am designing my first PCB using the free edition of Eagle. This is a simple board, with power and signal lines on the top layer, and ground on the bottom layer.

My question: I have components on the top layer, some which have pins to ground (the ground net is called GND). When I create the polygon on the bottom layer, and name it GND, all the airwires for GND connections disappear. Does this mean Eagle has implicitly created the vias for me from the top layer to the bottom layer?

Here is a detail of the schematic, and as you can see, some pins go to ground:

schematic detail

Here is a picture of the same area of the board. Blue is the bottom layer, i.e. the ground plane (or polygon named GND). Red is the top layer (power and signals).

board detail

For those pins that go to ground, I haven't done anything explicitly. Will those solder pads automatically have vias to the ground plane?

\$\endgroup\$
3
\$\begingroup\$

I haven't used Eagle in a while, but if I remember correctly, at the bottom left of the screen after you hit the ratsnest button, it will tell you how many airwires are remaining. I expect the airwires are still there, but since the nearest ground connection is directly beneath the pads then they're vertical (not showing up very well when viewing from the top or bottom). Unless this is a new feature in Eagle 7 (doubtful) then you will still need to create vias next to the pins that need to connect to ground.

\$\endgroup\$
  • \$\begingroup\$ That's it, I was completely overlooking the remaining airwires status that shows up after hitting the ratsnet button. Furthermore, many airwires were hidden. I right-clicked on my GND plane, went into properties, and unchecked the "hide airwires" button. Another tip I read about, when you can find that last tiny airwire that needs routed, is to deliberately zoom way out, hit the route button, then click pretty much anywhere on the board, and it will auto-select the airwire. \$\endgroup\$ – Matt Jun 24 '16 at 13:47
2
\$\begingroup\$

They way Eagle works is that air wires will snap to the closest object with the same net name. As @DerStorm8 mentioned the air wires are probably straight up and down making them very difficult if not impossible to find. As long as air wires exist then connections have not been made. Depending on the polygon to connect the grounds can be problematic.

You have 3ish options

  1. Remove the polygon and route all the grounds by hand. (This is my favorite) This guarantees that everything gets connected because all the air wires are easily seen. When your done routing then and only then flood the board with the polygon.
  2. In board view go to Tools and Statistics. This will show how many unrouted air wires there are under the summary. See picture. One feature(ish) that Eagle has is that an trance can only start with an air wire. If there are unrouted traces in Statistics, zoom out on the board until it's just a little square then click on the board starting a trace. The trace will snap to an air wire. Then zoom in to see where the trace starts. enter image description here
  3. There is a tool called zoom-unrouted.ulp This tool when run zooms in on an unrouted air wire. This makes air wires easier to find. https://www.element14.com/community/thread/6523/l/unrouted-ratsnest-drc?displayFullThread=true
\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.