@pastudan, Perhaps the warnings about having a No Connect X flag on a completed net could be better but if the correct procedures and checks are followed carefully then there are a number of warnings that will be issued which will lead to the detection of such a situation. The No Connect X flag is intended to indicate to the net listing process and the DRC that a pin to which it is attached has no electrical connection to it and so should not be detected and highlighted as an "Incomplete net" when a DRC is run in the Schematic Design Manager. [https://docs.easyeda.com/en/Schematic/Wiring-Tools/index.html#No-Connect-Flag](https://docs.easyeda.com/en/Schematic/Wiring-Tools/index.html#No-Connect-Flag)<br> <br> In the screenshot of the schematic, the CS0 pin is wired to the TXD0 pin and therefore both are connected to the left hand end of R5 (assuming the labelling matches the schematic placement). It can therefore only be assumed that either; 1. the placing of a No Connect X flag on the CS0 pin or; 2. the connection between the CS0 and TXD0 pins is accidental. Although it would not be good practice, it is possible to imagine a situation where in one version of a board a whole net is to be excluded from the PCB whereas in another it is to be included and that the selection between versions is controlled only by the placement of a single No Connect X flag. In that case, the operation of the No Connect X flag that has been observed seems reasonable. Normally however the placing of a No Connect X flag onto a pin that has more than zero connections to it might be expected to create a warning when a DRC is run in the Schematic Design Manager (because even a single connection to a hanging net should not be ignored but should be flagged as an incomplete net and the accidental placing of it on a complete net is, as your case shows, disastrous). It turns out that if a No Connect X flag is placed onto a net which has no explicit net label or net flag (e.g. VCC or GND) attached to it then when a DRC is run, that net simply disappears from the list of Nets in the Schematic Design Manager with no warning. If a net label or flag is then placed on that unlabelled net then a warning pops up to say that a "Net label cannot be placed on a wire which has a No Connect flag on it". In fact, EasyEDA does then allow a net label to be attached to the wire and if a DRC is run in the Schematic Design Manager, then it marks the net name as an error and warns that "This net label is not connected with any pin". If a No Connect flag is placed on a net that already has a net label on it then although no warning is given in the schematic, if a DRC is run in the Schematic Design Manager, then it marks the net name as an error and warns that  "This net label is not connected with any pin". A  warning about unfinished nets is issued on execution of a Convert to PCB... or Update PCB... or Import Changes... command. A net with a No Connect X flag cannot be highlighted by selecting it in the schematic and then pressing the H key. It is recommended that all nets should be given unique and indicative net labels. This helps to improve readability, the outcome of DRC and in cross probing between the schematic and the PCB during debugging.

When you have a situation like this or need to connect 2 nets use a 0R resistor.