Please read (2.2) and (4) in: [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f) You have to create 2 schematics. A) with everything on it. B) with only the parts that are on or form an integral ppart of the PCB. Suggest you create (A) first then remove the extra parts and save that (B) to a second project from which you create the actual PCB.

Surely the pots and switches still need to connect to the PCB somehow, presumably by some sort of plug/socket or soldered pins ?  So just create footprints for the pots and switches that are these sockets or pins.  Avoids having the two diagrams.

@MikeDB, @Shedman, My apologies. I should re-read my own documentation! Of course that's what you do. The pots and switches etc., are connected to the PCB by some sort of wiring either through connectors or soldered directly to the PCB. So, place the pots and switches in the schematic but change the Package attribute of each to assign the PCB Footprint for a suitable pin header or other connector to them. For direct wired connections, this pin header or connector is not fitted but is used simply to define a set of plated through holes that must have a large enough diameter to accommodate the wire ends. If a suitable footprint does not exist, you can create a new or edit an existing one and save it with a suitably descriptive name. There's a detailed description of how to create footprints and assign them to symbols here: [https://docs.google.com/document/u/1/d/1ZRkPPMID68mBz9j9RMIJARNSXK12PDULZXP7kiThvDg/mobilebasic](https://docs.google.com/document/u/1/d/1ZRkPPMID68mBz9j9RMIJARNSXK12PDULZXP7kiThvDg/mobilebasic)

If only it were that simple... **Problems with putting everything into a single schematic** In (2.2 and (4) of: [https://easyeda\.com/andyfierman/Welcome\_to\_EasyEDA\-31e1288f882e49e582699b8eb7fe9b1f](https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f) I have defined a schematic as showing "Everything that is on - or forms an integral part of - the PCB." In other words anything that is not fixed to the PCB in some mechanically rigid way is, by that definition, Off-PCB. So for example a pot that is mounted Off-PCB on a front panel but is wired either directly to the PCB or through a connector, is Off-PCB. A switch whose shaft is (for whatever reason) mounted through a hole in the PCB but is connected to it using discrete wires is an On-PCB part. There is a problem with the single schematic approach described above which for hobbyist or small commercial projects may not be a problem but which can become messy on large projects. By including Off-PCB things like input signal and power supply sources, jack sockets, pots, switches, loads such as loudspeakers, motors etc., in the schematic but assigning PCB footprints to them for the connectors that are actually fitted to the PCB to connect to them, you can end up with a BoM that includes the components but not the connectors (or the other way round). This isn't a problem if components are wired directly to the PCB but for indirect connections through connectors this can get complicated. For example, suppose a pot is connected to the PCB through a 2 part connector. The pot has a plug wired to it and a matching socket is mounted on the PCB. So you have three components (four or even six if you include the wire used) that from a project point of view should be represented in the BoM. For the purposes of designing the PCB, you only need to show the symbol for pot in the schematic with the PCB Footprint of the socket assigned to it. The BoM however only lists the pot and not the PCB mounted socket so the BoM is incomplete and from the point of view of the PCB itself is incorrect. Also, from a project point of view you may want a separate schematic to show that a pot is wired to a plug so that an assembly drawing can be produced generating a BoM and wire lengths etc. for just that assembly. EasyEDA does allow extra fields to be added to a library symbol after it has been placed into a schematic so it is possible to add a second set of fields for the part name, supplier, supplier part number, manufacturer and manufacturer part number for the socket used as the means of connecting the off-PCB part to the PCB. i.e. for the part whose PCB footprint has been assigned to the package attribute of the physical off-PCB part. For completeness however, two or even three sets of fields should be added to allow for both halves of the connector and the wire to connect the pot to the plug. It is also possible to select which of these fields is visible in the BoM, although editing the BoM visibility attribute once the new field has been added is currently only possible by editing the EasyEDA Source JSON file for the schematic. A similar complication arises where the PCB itself is used as the mounting for, for example, the shaft of a rotary switch but which is wired to the PCB through wires or a connector. As defined above, this is effectively an On-PCB part but again it is not so straightforward to represent all the elements for the Schematic, the BoM and the PCB. From a schematic point of view the schematic may could show only the switch or the switch and one side or both of the connectors but a complete BoM needs to list the switch and both halves of the connector (and possibly the wire used for the connections). From a PCB point of view the switch has to have a dedicated (custom) PCB footprint that has a hole for the shaft and a set of pads for whatever type of connector with however many wires that are needed to go between the switch and the PCB. Another way of looking at creating two seperate schematics clearly represent Off-PCB parts might be to create a multi-sheet schematic with all the On-PCB parts on the main sheet and all the Off-PCB parts on separate sheets. Then generate a project BoM for all the sheets (it is currently not possible to generate a BoM for each sheet in a project individually). Then copy just the main sheet into a new project which is specifically to produce the PCB with only those parts mounted on it. **Other ways to deal with Off-PCB parts?** To explore other ways to deal with Off_PCB parts, I have tried a few tricks in a simple test project which has two connectors and a resistor on a PCB with a pot and two resistors wired to it externally. One is to put everything into a single schematic but delete the package names (leave it empty) in the symbols for the Off-PCB parts. This fails because EasyEDA sees a part with no package assigned to it and errors. A second idea was to create a null package called OFF PCB which has no pads and then assign that to the Off-PCB symbols. This fails because EasyEDA sees a part with mismatched pin mapping and errors.