Have you set the netname for your copper area to the same as that of the net you want to connect it to?

@andyfierman Yes. The copper area for both the top and bottom layer of the PCB have the same net name called "GND". But after building it and checking the GND connection in the Design Manager tab, it still says that they are all unconnected. I also tried connecting GND terminal from the top layer to the GND terminal on the bottom layer, but no luck with that either. :(

You are getting this warning:  because you have several GND nodes that are not yet connected. The red backed white cross on a net only disappears when everything on that net is connected. If you take a step back and look carefully at your PCB you will find many nodes that are unconnected. For example: C8 GND pin is shown as unconnected because the copper area it is on is not connected to ground anywhere else:  The pads on U2 and U6 are not connected to a ground anywhere (they're on the other side of the board from the nearest copper area):  If you want to connect things using copper areas, you must make sure that the copper can connect up to other areas either just by the flood of the copper area itself or by adding dedicated ground tracks. Note that such tracks should be no wider than and at be routed at the same angle as the spokes that they will have to pass along.

@andyfierman Understood. I always thought that using the Copper Area tool was always going to connect all the GND nodes together on a PCB, but I guess that's not the case here as shown. I'll fix the schematic by manually adding the unconnected GND nodes to GND. Thank you so much for looking into this for me.

No, the thing you have to fix is not in the schematic: it's in the PCB. You have to get you head around this so I'll try to explain what's going on in the PCB in a slightly different way. First of all, note that the **Keep Islands** setting for the copper areas only removes copper that has nothing at all connected to it. So if the copper area can form around a pad or a via that in the netlist is connected to the same net as that assigned to the copper area then a copper area will form. That does not mean that it automatically connects via some copper to any other copper area. It just means that that copper area has a connection in it that the netlist says should be connected to the same net as that assigned to the copper area. If you have an open area containing a pad on a footprint that is connected to the net assigned to the copper area but which is hemmed in by tracks or closely spaced rows of pads all of which are _not_ connected to the net assigned to the copper area, you can have an area of copper surrounding a pa both of which are on the same net but which are cut off from any other track or copper area on the same net. So you can end up with lots of copper areas each of which has something within it that needs to be connected to the same net as that assigned to the copper area but each of which is not connected by any copper to any other. There's nothing wrong with this: checking the DRC will show you that the net is incomplete and checking the pins on the net will (eventually) show you which ones are not connected and which you therefore need to do some rerouting or additional routing and/or adding vias, in order to connect. The **Keep Islands = No** setting will stop remove any isolated islands of copper which are completely unconnected and do not even have a pad to form around but it will not prevent isolated areas of copper forming around one or more adjacent but otherwise isolated pads.

@andyfierman Sorry, I meant PCB. Not schematic.

How do I remove all the copper ground plane? after correcting an inverted 8 terminal plug, the auto router fails.

@autobeyours, [https://docs.easyeda.com/en/PCB/Copper-Pour/index.html](https://docs.easyeda.com/en/PCB/Copper-Pour/index.html) You can try just making it not visible using the visibility switch in the right hand panel or Right-click > Canvas Attributes To remove an individual copper area, just select the outline for it an delete it. To remove all the copper areas, see: [https://docs.easyeda.com/en/Introduction/Shortcut-Keys/index.html](https://docs.easyeda.com/en/Introduction/Shortcut-Keys/index.html) SHIIFT+M or: **Edit > Global Delete... > Copper Area**

Hi @autobeyours Shift+M only remove the copper fill data, you need to select the copper area outline and press delete key to delete it. cc to Andy @andyfierman

@UserSupport, Thanks for clarifying that. :)