If you have started by creating a schematic and then done Convert to PCB, check the connectivity of your schematic using the Design button in the left hand panel. The Nets section will allow you to check which nets and component pins are connected together and any that are unconnected. Manually assigning netlabels to all the nets in the schematic makes this much easier. If the schematic is correct then the ratlines in the initially unrouted PCB will be correct. Do not try to edit the connectivity in the PCB. Do it in the schematic and then do Update PCB... from the schematic or Import Changes... from the PCB.

Thanks for pointing this out. Everything is connected, still I don't understand why I get wrong ratlines. I probably am doing something wrong while drawing/connecting the components in the schematics

If this is a public project then post the URL to the project and maybe someone can gave a look at it and help you out.

Here it is: [https://easyeda.com/chickengun/usb-motor-control-with-temp-sensor](https://easyeda.com/chickengun/usb-motor-control-with-temp-sensor) It's a usb DC motor and a temperature sensor hooked to an arduino. The flyback diode D1 should be directly attached to +5V and GND on the usb motor, but when I convert the schematics to PCB the rat lines are wrong depending on the position where I place that Diode

When you move the footprint together you will see the ratline is correct. the ratline will show by the close objects. 

Yes, the ratlines are not like tracks. They're dynamic and snap between the nearest pins on the same net as footprints are moved around which can be quite confusing the first few times you see it.

Looks like I am missing some basic information how to create prober rat lines. Just as an example this should not happen right?   Arduino nano's VIN should not be connected to the OLED's GND. I am still a little bit confused, do I have to introduce netlabels to solve it?

If you click on a pad in the PCB and then press the "H" key, all the pads connected to the same net will light up. I've had a look at your schematic and then converted it to PCB. I see the problem. I think it is because the because the pin labelling of the footprint you have used for the OLED PCB does not match the pin numbering of the schematic symbol. Zoom right in to the pins in the schematic and you'll see the pin numbers and/or names:  But now look at the OLED Schematic Symbol in the Schematic or in the Schematic Lib Editor (search for it in the Shift+F component search under the Sch Lib tab, select it then open it for editing):  It looks like the footprint is user contributed and has not been checked by the contributor. This is why the Search Libraries window has the warning at the bottom:  Also, Click on the package attribute for the symbol in the schematic and then look at the pin mapping in the Footprint Manager:  You can re-map the pins here to fix the problem for your PCB. "...do I have to introduce netlabels to solve it?" No but they make tracing and debugging schematics and PCB much easier. You can find some hints on how to make properly documented Schematic Symbols and PCB footprints in my two comments here: [https://easyeda.com/forum/topic/Part-used-is-not-found-so-I-want-to-edit-a-part-so-it-can-be-mine-how-do-I-do-that-80f71b52df2e4cb89affd38a765ba78d](https://easyeda.com/forum/topic/Part-used-is-not-found-so-I-want-to-edit-a-part-so-it-can-be-mine-how-do-I-do-that-80f71b52df2e4cb89affd38a765ba78d)  Reply I also recommend that you see: [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f)

@chickengun, Do you have a manufacturer's or supplier's datasheet for the OLED part?