I am designing the schematic for a board and have a single remaining error in the ERC Checker. Please can you take a look and help me understand what the problem is.
I have 4 identical scart bus connectors, each driven from a 5V rail, see here:
Pin 17 is the 5v Rail connector, and in each of the 4 chips, it is connected to the same rail, as per this image(note the right angled wire on the right hand side is the wire from A4 pin 17:
ErrType(3): Pin connected to some others pins but no pin to drive it
@ (328.93 mm,344.17 mm): Pin 17 (Power input) of component A4 is not driven (Net 167).
My logic suggests if A1 - A3 are connected to this rail fine, why would A4 be reporting this error? Component A4 is the bus on the far right hand side…as far as I can see, the wire from pin 17 correctly joins up to the 5v Rail.
Can somebody help me get to the bottom of what is causing this error?
I also notice that in your second screenshot there is a little rectangle on the “5V” net label. That means that label isn’t actually connected to any nets. Move it so the label is on the green connection lines (any where on the green) and the rectangle will be gone. If there are no other labels on that line then when you import that netlist into PCBnew the connection network (i.e. 'net) will be labeled “5V” instead of a seemingly random auto-generated name.
See Sprig’s answer for the short answer of how to resolve your ERC issue (my observation is separate from your ERC issue). The reason why you aren’t seeing the same error for the other pins on the net is because KiCad will alert you of an issue on one pin of a net instead of ALL pins on the net for brevity. Unfortunately, the indicated pin may not be near the actual origin of the issue. (Sort of like how a missing semicolon in a program can pop an error tens of lines of code later.)
The power flag is in the power lib.
It tells kicad that a net is powered by being a single pin device (pin is of type power output) So place this carefully to still get the benefit of the ERC.
Directly at the connector that powers your pcb. If you have a passive device in series (Fuse, inductor of a filter, …) then after this device (But again as close as possible to it.)
I am not sure sure about the polarity, I thought that was right! What should it be?
It has now been resolved - I was looking for a “PWR_FLAG” element as per :
I don’t understand why there are 3 pins on the jack though. I believe it is to do with a battery – but my device will not be powered by battery at any point, so I am kind of just ignoring the middle pin for now!
I am not sure of the advantage of the 5v label, what do you mean by easily connect it up elsewhere?
Yes - you can use the switched pin 3 to connect a battery. When unplugged, power will be supplied through the switched contact. When plugged in, the contact is broken.
You use labels to connect two or more distant points without the need to draw a line between them. So you can put a GND or a 5V label (or whatever) elsewhere on your schematic sheet as a connection to another component without your schematic turning into a birds nest of crossing wires. Labels can be local to one sheet or global to the whole project.
