other end of fuse connected to +5v, but no power flag
So, you have everything ‘connected up’ ok, but DRC isn’t recognising the ‘5v’ as being driven by a power output. DRC expects ‘inputs’ to be driven by ‘outputs’, and power is no difference. The two ends of a fuse are, I have no doubt, deemed to be ‘passive’, so the poor +5v isn’t deemed to be fed by an ‘output’… so it also needs a pwr flag to keep DRC happy.
In KiCad, every net that has a pin that is defined as being a Power Input has to be connected to a pin that is specified as being a Power Output (for example the output of a voltage regulator).
Each net can only have one Power Output pin. You can’t short different power regulators together. There are rare cases where outputs are being connected to get more current, but even then there are often balancing resistors in between (See some old application notes of the LM317 for example).
Because each net can only have one power output, the power symbols have to be defined as being a Power Input. Many of them are often on the same net.
And finally, the use of the PWR FLAG. This is used when a pin which is defined as being a Power Input is not connected to any pin with a Power Output. For example for connectors through which the power is delivered to the PCB, the pins are normally defined as Passive. KiCad can not know how the connector is going to be used, and passive is the most permissive pin type.
Me, too. There’s something the original poster doesn’t understand, but also something we don’t understand so that we could explain things clearly.
IMO the original schematic design should be redrawn, like the following. Not only because it looks tidier, uses de facto “good practice” rules of thumb and is easier to read, but also because it helps finding the root of the problem.
If delete your existing wires, delete power symbols etc., move the old symbols, rewire and then update the PCB from the schematic, it should work.
First rule of thumb: source left, sink right. Input left, output right. If I have understood correctly, there’s a buzzer which is driven by logic.
Second rule of thumb: high potential up, ground down.
Third, suggestion: no separate sections. They just aren’t needed, this (small and simple) design is clearer when everything is connected with wires.
Why no power symbols/flags? Because they aren’t needed in a simple design and in this case they may be the part of the problem and cause misunderstandings. The ERC error is caused by power pins/flags and draws attention, while it’s just a technical detail of KiCad which isn’t necessary for a successful design, especially for a simple one. (The more I think about this - over several years - the stronger is my opinion that this power flag system or even the whole pin type system should just be ignored, by default set to be ignored in KiCad.) In any case, if you start with the most simple representation possible, it may be easier to notice what went wrong, and then change to more complex one.
At first I was tempted to suggest to use normal local net labels. But even that could be a mistake. Let’s see how a fuse would be added:
And this would only repeat the original problem, as far as I can see.
The left and right side of the fuse shouldn’t, don’t and can’t belong to the same net!
No matter if you use the +5V power symbol or just ordinary local net labels. They both connect everything with the same name together, like this would connect the two sides:
What this does is shorting all those pins together. Basically, you did this, and it caused the error. Unfortunately you deleted your old messages (please don’t do that!), but in the screenshots by Paul we can see that you added the same power symbol to both sides of the fuse. This doesn’t work.
You shouldn’t insist using power symbols if you don’t understand how they work. The most important thing to understand seems to be that electrical connections – physical connections in a real circuit which can be functionally thought of having 0 ohm resistance – are NOT nets in KiCad. Nets are only connections between symbol pins and then component pins/layout pads. All pins which belong to the same net must be explicitly connected with copper in the layout.
The ERC error is still a red herring. It’s a kind of a problem, but it’s caused by another problem. Also, there’s no error or problem in KiCad itself. This doesn’t depend on the used KiCad version or something like that. If you share your other, old design which have worked, and this new one, we can find the difference. You have done something differently before. I’m pretty sure it’s exactly this misconception about connections and nets.
I think this all has been said many times in this thread. At leas Retiredfeline saw the same problem, in different words:
Also Piotr and JamesJ among others.
The last message by Paul, about power flags and power input, should be read only after you understand the more basic thing about nets and connections, otherwise it just confuses more.
