If a component is not on - or does not form an integral part of - the PCB then it should not be in the schematic from which you create the PCB. By all means in a schematic in a separate wiring diagram project but not the diagram from which you generate the PCB. Presumably you have assigned some sort of 2 pin header to it as a PCB footprint? A workaround would be to clone the switch symbol and save a uniquely named copy with the common and the unused pins given the same pad number. If you do this however it must be very clear in the symbol Description field that it is a special case and why. This will help avoid other users misusing it.

This principle: "If a component is not on - or does not form an integral part of - the PCB then it should not be in the schematic from which you create the PCB." is explained in more detail in (2), (4) and (6) 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)

What bothers me is that it used to work! In fact, I have ordered three batches of this very PCB from JLCPCB over the course of several years and there was never a problem. Now I come back to this project to make some small changes and some of the old components within the schematic prevent updating the PCB. This particular switch I mentioned isn't the only part causing trouble. I don't really understand your workaround. Care to elaborate?

Hi You need to make sure your part has the same pin count and pin number with assigned package. [https://docs.easyeda.com/en/Schematic/Footprint-Manager/index.html](https://docs.easyeda.com/en/Schematic/Footprint-Manager/index.html)

@fripholm, Your project is private so only you can see it so I am guessing what you may have done. The [Tesseract](https://easyeda.com/example/Tesseract_Guitar_Practice_Amp-MjP71jBni) project has a number of components that are off-board. These are are represented by Schematic Symbols appropriate for the parts but the PCB Footprints assigned to them are simply 0.1" pitch SIL headers (and in fact no headers were used: the wires to the switches were soldered directly to the PCB). This works OK because every pin on the switch maps to a pad on the header. If you are using a 3 pin SPDT switch in place of a 2 pin SPST switch then you have only 2 wires connecting the switch to the PCB and you either have an unconnected pin or have two pins (the common and the unused pin) connected together at the switch itself. I am assuming that you therefore have a 2 pin header of some sort on the PCB. So you have a Schematic Symbol with 3 pins that you are trying to map onto a PCB Footprint with only 2 pads. Let's assume that the pins on your switch symbol are numbered "1", "2" and "3" and the pads on this footprint are numbered "1" and "2". You have 2 options. **Edit the symbol directly in the schematic:** 1. Select the symbol in the schematic; 2. Click on the Package attribute and assign your chosen 2 pad footprint to the symbol using the Footprint Manager; 3. With the symbol still selected in the schematic, press the "I" key;  4. Edit the pin numbering of the symbol so that the common and the unused pins have the same number so you now have a symbol with pins numbered "1", "2" and "2" or "1", "1" and "2"; **Make a dedicated Schematic Symbol:** 1. Find your Schematic Symbol in the Search Libraries tool;  2. Edit it so that the common and the unused pins have the same number so you now have a symbol with pins numbered "1", "2" and "2" or "1", "1" and "2";  3. Save it with a unique name and enter in the Description field very clear information stating that the symbol is a special case and why.