@Dmc I am not sure I see the difference. It looks the same to me unless I am missing something.
There are two switches controlling the power source
The point is to use the battery only when there is no power supply AND there is a guitar plugged in the audio jack. This way, disconnecting the guitar will put the battery to rest.
In theory, the forum tries gracefully kick out “just electronics design questions, not-specifically-KiCAD” after a short but decent interval (so in my previous reply to you, I admit I was intruding a bit on the forum’s goodwill policy 
However I think you made a subtle error (KiCAD-specific!) in your original schematic, so I think that this reply is legitimately ON TOPIC…
Here is a snip of your original schematic. I have hit the “backtick” key (`) to highlight this net; According to KiCAD, everything in magenta is connected together:
The top “9V” item I have circled in blue is a “net label” (aka a “local label”), which assigns the net name “9V” to that wire, which among other places goes to J1 pin-2
The lower “9V” item I have circled is a “global label”. It happens to have the same name “9V”, and therefore assigns that exact same net name to among other places J1 pin-3.
KiCAD has a rule (I think) that a global label named “x” is the same net as any local label named “x”. I think this caught you here.
In your schematic, you DO NOT show pins 2 and 3 connected together by wires… because I believe that your design intention was that they NOT be connected. HOWEVER, because you have assigned the “9V” net name to the wires connected to J1 pin 2, and you have also assigned “9V” to J1 pin 3, you have told KiCAD “these are the same net; join them”
This connecting of pin-2 and pin-3 is also reflected on your PCB (when you were laying out the PCB it probably didn’t twig):
In your most recent reply you have a slightly different schematic; I believe this is correct and will work as you intend. The important thing to notice is that there is no “9V” label on the positive terminal of BT2 nor the wire going to pin-3 of the jack… therefore KiCAD knows that pin 2 is distinct from and not connected to pin 3:
One more comment, I think this will not work as you expect it to:
When a plug is inserted into J2, it will not cause the “R” terminal to be electrically connected to the “S” terminal.
@Dmc ah I see! Yes the label will be an issue! I will rework this.
As for J2 acting as a switch, this is achieved by using mono jacks on stereo connectors which is hard to show on the schematic. When inserting a mono audio jack on a stereo connector T and R can be short circuited.
Also, thank you for the clarification of the rules, I am also a bit worried that what started as a circuit review has gone down the lecturing road but as I said on the initial post, this is a KiCAD learning journey and sometimes it’s hard to proceed unless you understand what’s going on. Anyway, I hope I am not misusing the forum, I guess some ops will close it down if so.
Here is a guitar pedal project I did some years ago (on eagle). It fits the classic metal Bud box and is comprised of a base pcb with power, signals in/out etc, and a plug-in upper board with an effect of your choice (a 2x5 header/socket connection). I did a simple back-to-back diode clipper as a first test module. Maybe there are some ideas here. Yes, center-negative is standard for pedals.
190-8002-A-pedal-SCHEMATIC.pdf (188.3 KB)
@teletypeguy thanks for the input. I also think about making a version with all parts on board but I am pretty sure it’s too early for this.
Until now I’ve been trying to squeeze things together, but this post has shown me that I should not worry too much about the size of such a circuit. So, next version will be a bit more spacious to fit jacks, switches etc
