On the project I'm working on in Eagle I've twice found an airwire after running the ERC, which found no errors. You can see the airwire in this image along with the ERC message at the bottom of the screen saying that the board and schematic are consistent. The approved warnings it mentions were just power/supply net name differences.

Does Eagle consider an airwire to be a connection even if there's no copper trace?

 

I'm pretty sure that an airwire is a connection. It has been awhile since I used Eagle but to refresh my memory, I took a board with a good ERC, ripped up a trace and did the ERC. It still passed. ERC looks to see if the schematic and board are consistent and I guess air wires are connections, too.

I usually checked unrouted stuff with the RATSNEST command. It will show any non connected traces as a number of airwires on the status line at the bottom of the screen. It's quite common to have a few little ones when you didn't quite hit the center of an off-grid connector for example. In that case, turn off all layers except air wires to see where the little stubs are and fix them.

I does seem goofy that it wouldn't pick up what you show. Mine didn't either. I know that the way Eagle works, relying on forward and backwards annotation for board checks can miss some errors. My first board with Eagle had a stray trace running across an 8 line bus and it passed ERC and DRC because the board's netlist matched the schematic's. Tango / Autotrax was better in that regard. Go figure.

That said, I did a lot of boards with Eagle back in the day. Seems I'd remember that one, though.

Good luck!

 

For a comparable feature set and similar pricing (including a non-commercial free version,) I'd recommend trying DipTrace.

My first board was in Eagle, and it was a nightmare. Everything is difficult and inconsistent for no reason. Creating footprints is insane. Back annotation is difficult and dangerous. Once something is out of sync, it seems impossible to re-sync.

All my complaints are probably exaggerated, but my point is that you can do better for cheap or free. DipTrace has an intuitive interface for everything I need, has effective DRC and net list checks, and has made my life soooooo much easier!

I'm sure there are other options worth considering too, but I've been happy enough with DipTrace that I haven't searched any further.

 

I could have sworn that the ERC caught something like that on some past project, but maybe I'm just remembering wrong.

 

I could have sworn that the ERC caught something like that on some past project, but maybe I'm just remembering wrong.

Me, too. I was surprised to see it not pick up the deleted trace on my test. Kind of worthless as a rules check, IMHO. I've done dozens of boards with Eagle with good results. I guess routing along the air wires until there aren't any more is the way they expect it to happen. I wonder if there is a ULP for that?

 

ERC is for checking the schematic. It checks for things like missing connections, values and such. ERC is not a useless check. You'd find this out if you forgot to make a connection and sent the board off to be made without doing an ERC.

DRC is for checking PCB rules but doesn't check for airwires - it checks to make sure your layout doesn't violate the rules you have selected.

To check for airwires, use ratsnest.

For what it's worth, you have to learn to do things the Eagle way. It's a modal interface which is counter intuitive for windows users. When I first started, I fought it and hated it. But over time really came to appreciate the power of the interface. Once you understand Eagle, it becomes really fast to do things. I can bang out a new library part in very short order - even fairly complex parts.

 

Let me add just a little to philba's comment:
1) For a final board, I check for airwires by turning off all layers except airwires. (I might leave an outline to help orientation. ) Sometimes the segment of airwire can be very small, such as when the routing missed an endpoint. That is not much of a problem with newer versions of Eagle that snap to origins.
2) If you have turned off airwires for particular signals, nothing will show, even with "ratsnest" (alone). You need to either use the "i" tool, click on a part of the signal that is showing, and uncheck the box to hide airwires. Or, you can also use "ratsnest <signal name>, example: ratsnest N$43. And, if you don't know the signal name, use "ratsnest *" . Don't for get the space between the command and the wildcard. The last method is the one I use most, unless for example, I have turned off VCC and GND and only want to see one of them.

At least it is that way on ver. 7.x.

 

Or, you can just hit the ratsnest button

and look at the lower left corner - it will say the number of airwires left or "nothing to do".

The thing that I dislike the most about airwires in eagle is when you get really short ones. They can be really hard to see. Ratsnest command/button only tells you how many you have, not where they are or which ones. You have to turn off every layer except unrouted and even then they are hard to see. I often wind up having to do what I call a "zoom search" - zoom way in, then scan the board. Wish there was a way to make airwires fat. This problem happens occasionally when you have parts with pads that are slightly off grid and you ripup a prior route and reroute it. Unfortunately, you always have a mix of metric and imperial parts. Sigh. (though, I bet with the really short ones, the board would fab just fine. the purist in me wants to get it perfect)

[edit] and while I'm at it, one would think that just running the autorouter would fix those tiny little airwires. It is not like it has to do much thinking. But no, for some reason it just ignores them and essentially does a whole lot of work for zero changes. Just another reason why the eagle autorouter sucks.