ERC Checker problems with power line

Hi,

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:

The ERC checker reports just 1 single error:

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?

Short answer, adding a PWR FLAG to that net will likely clear ERC.

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.)

Ahh wonderful - very useful.

Can you explain how I add a ‘PWR FLAG’ to the net?

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.)

You might want to take a look at this FAQ article: Electrical type of schematic symbol pins (KiCad 4 and KiCad 5)
Especially the section about power input/output pins.

I am not sure if I am doing something incorrectly here. I have added a power flag at the connector which powers the circuit.

24

Now A3 pin 17 reports the same problem, when before it was A4, Pin 17? Thoughts?

Have a read of this FAQ ErrType(3): Pin connected to some others pins but no pin to drive it
It has a good explanation of power flags. You have added a label not a power flag. You need to add the flag in addition to the label.

Are you sure you want the polarity of your jack that way round?

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 : 49

Yes - but you can also leave your 5v label there too so that you can easily connect it up elsewhere on your schematic page.

[Edit] If you are using a Barrel Jack then your connections are correct. I have just been using a 3.5mm jack with the same symbol.

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.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.