Just to confirm: the two polys are the same net (i.e. both GND)?
Considering your isolation looks good around the other traces, there must be something else going on. If you turn on the other relevant layers (top, holes, vias, tkeepout, bkeepout, trestrict, brestrict at least) and post another picture there might be something to explain it.
Do you mean for there to be that many traces that go nowhere? (AKA net antennas)
As for your problem - there should be a setting for deleting isolated sections of copper. Further, there may be a setting for controlling the width of the tracks used for your pour. I’m not familiar with your software so I can’t comment on where these settings are.
Right click on the edge of the polygon and select ‘properties’ make sure the ‘orphans’ box is checked. This is supposed to remove isolated copper but I’ve had problems with it myself. If that doesn’t work I see two possibilities for your case. Redefine your polygon to exclude this area (use 2 if neccesary) but this is probably not as easy as simply changing the width of the tracks for the copper pour as NleahciM mentions. The width of the line you use to define the polygon is the width used in the pour.
Hopefully this helps. I’m new to Eagle and PCB design myself so maybe someone else can shed more light on this.
You have a couple of isolated copper pour areas, including that one. The software I use won’t create them in the first place. If you can’t do that with Eagle, just delete them.
That acute angle where a track joins a pad looks nasty, I’d fix that as well.
You need to name the polygon, otherwise there will be orphans because none of the fill is tied to any net. Use the Name tool and give it the same name as your ground net. Don’t try this with the orphans themselves because they are all part of the same polygon, even though they don’t appear to be. Do it on the main outline. Another way of avoiding orphans is to move things a little bit to leave enough room for them to connect. The reason they aren’t connecting is because your polygon line thickness is too high for the space between the other copper to make it through and pass the DRC.
I’d also encourage you to refrain from using the autorouter at all, because it really leaves a lot of bad stuff behind. Your traces could stand to be quite a bit thicker and better organized. You’ll also find that hand routing can save you a lot of board space.
