@bencfd, Welcome to EasyEDA. The basic problem is that you have  tried to use tracks inside a PCB Footprint. This should explain the problem: [https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6](https://easyeda.com/forum/topic/How-to-avoid-DRC-errors-when-connecting-to-PCB-Footprints-a-k-a-PCB-Libs-90bf944fe3644b21a7d27a9e9d8df8d6) Your footprint looks very interesting but at the end of the day, unless you are trying to create the copper patterns for a capacitive or resistive touch pad or key, I suspect it is far too detailed for the job it is required to fulfil. All a PCB footprint has to do is represent the pads that are in turn represented by the pins on the schematic symbol, with the correct numbering and in the correct positions to connect the pins of the physical device onto the PCB and to show an outline to make sure than nothing overlaps or otherwise mechanically interferes with it. It is not necessary to represent any of the internal structure of a device in a footprint other than perhaps to assist in orienting the device correctly. The biggest problem with what you have created is that the only way to represent your internal structure on any relevant layers is to either use pads to avoid the DRC errors or to draw it on the Document Layer. If you are trying to create a capacitive or resistive touch switch then this may help (because the copper patterns for a resistive touch switch may be similar to those for a capacitive switch but with the copper exposed): [https://easyeda.com/forum/topic/How-to-create-a-capacitive-touch-pad-f6395e879953426bb6c31531553ac160](https://easyeda.com/forum/topic/How-to-create-a-capacitive-touch-pad-f6395e879953426bb6c31531553ac160)

If you need the internal copper detail in your (what is now called) PAD-ONLY KEY FOOTPRINT you could convert the tracks into pads using the right click menu. You will then need to change the pad numbering to avoid DRC errors in the footprint (remember that in a footprint multiple pads can have the same number). If necessary you then may also have to play about with the Solder Mask Expansion attributes to get it to cover the pads.

@andyfierman thank you very much for your detailed answers! I indeed tried a couple of things before reaching back to you. You're right, I overlooked to give some info about the project. I'm trying to arrange 55 elements (11x5) on a board. Each element consists of a key (as for a keyboard) that contains a WS2812B LED (that is the central drawing on the top silk layer), and comes with a capacitor and a resistor to avoid ghosting. One element itself needs quite some tracks, this is why I'm trying to use a symbol. I successfully converted a track to a pad in the PCB footprint as you suggested, and I am now able to connect the two elements with a wire on the board. As you anticipated there are still some DRC errors. I will control the pad numbers and the solder mask expansion.

As explained in my links sbove and in (2.3) in (2) in: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a) you can have more than one pad with the same pad number so your schematic symbol does not have to physically represent the shape and pad distribution of the actual device. The simple example is a PCB mounted TO-220 packaged mosfet with a metal tab. It has a source pin, a gate pin and two connections to the drain, one the centre pin, the other the tab. The symbol only needs to show three pins:  source, gate and drain but the Footprint can have 4 pads with the drain pin and tab having the same number. Actually to do what you want, you might be better off using the Schematic and PCB Modules.