If I understand the scope correctly, this is a similar question to how to make a pad to solder a wire to. For example: [https://easyeda.com/forum/topic/How-to-wire-directly-to-the-PCB-a0c29f318aff4c59a45cda060d3ca3b7](https://easyeda.com/forum/topic/How-to-wire-directly-to-the-PCB-a0c29f318aff4c59a45cda060d3ca3b7)<br> <br> If you want to wire link from one part of a track to another, you must accept that the two pieces of track must have different net names in the schematic. This is because in EasyEDA Std there is no comcept of a Net-tie or shorting link. For backgrond to this, see: [https://u.easyeda.com/forum/topic/Net-tie-a-copper-only-component-with-2-pads-to-split-nets-without-DRC-errors-and-multiple-netname-warnings-b6a099bf01bb4055b821ab398ee37b60](https://u.easyeda.com/forum/topic/Net-tie-a-copper-only-component-with-2-pads-to-split-nets-without-DRC-errors-and-multiple-netname-warnings-b6a099bf01bb4055b821ab398ee37b60)<br> <br> If you simply represent your wire links in the schematic as 0R resistors then having a different net name either side of the resistor makes sense. The problem with that simple idea however is that in reality, the two pieces of track may be anywhere on the board so no single component can represent the individual and different "footprints" that each of those different wire links across each track pair positions create because a single footprint defines a fixed spacing between the pads.. A solution to this is to place a single pin header (N=1 in the How To above) at the free end of each wire that you want to solder a wire to. Assign a suitable footprint to each of these symbols. These may be through-hole or single layer pads as required for each connection. For each of these symbols, set the: 1. **Convert to PCB** attribute to **Yes** (because you want the pads on the PCB);  2. **Add into BOM** attribute to **No** (because there is no physical component on the PCB); For any connections that are from one track to another on the PCB then find, edit or create a 2 pin symbol for a piece of wire. This could be the symbol for a simple 0R resistor or a more compleicated wiggly piece of wire, it really is up to you. No matter how it is drawn however, it must be assigned a footprint. This footprint can be for any 2 pin component, again it really does not matter what it is: it just has to exist in the library and be assigned to the symbol. For each of these symbols, set the: 1. **Convert to PCB** attribute to **No **(because this component is an off-board component so is not mounted on the PCB and so needs no pads on the PCB); 2. **Add into BOM** attribute to **No** (because there no physical component on the PCB). Note however that if you describe the wire type in the symbol, you could set the Add into BOM attribute to Yes so that you arereminded to order the wire that you will need. Then you can place your connections in the schematic so that where necessary they can be conveniently connected together by your "wire" symbol. Or just place the wires off to one side or even on a separate sheet and use net lablels to make the required connections. There are similar examples to this usage case described in Appendix A to (2.2) 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)<br> <br> which should help you understand this procedure.

Thanks for the infomation and for answering this quickly with so much info! My question was about "to wire link from one part of a track to another" as you said. I had used (on a previous PCB) 2 single-pin headers on the schematics to make the connections, but would have liked a better solution here as (as you say) the two pieces of track may be anywhere on the board. Well, I then have to use 2 single-pin headers. Thanks again and best regards, Sebastien.

Yes, the two single pin headers with different net names either side of the break seems like the way to go. BTW: my suggestion about the "wire link" symbol is really only to improve the readability of the schematic since there's no footprint for the physical link so nothing about it appears on the pcb.