I am new to KiCad and finishing up my 2nd schematic. I have an annoying problem that I can get around (I hope), but want to understand what is happening. I have a power supply (isolated DC/DC converter) with 2 power input pins (+Vin and -Vin) and two power output pins (+Vout and -Vout). The +Vout line is +5V and the -Vout is COM2. There are three capacitors between the those two lines.
When I run the Electrical Rules Checker, it informs me that Pin 3 (+Vout) of component U2 is connected to Pin 4(-Vout) of component U2. I don’t understand why.
I have discovered that if I open the symbol editor and change the Pin 4 to be Passive instead of Power Output, the error goes away. The error will also go away if I move the +5V and/or the COM2 power ports off of the ends of the lines. I have to have those ports connected, but don’t mind re-labeling the Power Output Pin as a Passive pin, but would like to understand why that is happening.
Can anybody clarify?
I am attaching a copy of that part of the schematic. It is passing the electrical test now, but only because I changed pin 4’s designation from power output to passive.
You have a short between those two nets somewhere else on the schematic. The error isn’t always flagged at where it happened only somewhere in the same nets. Don’t change the pin type, the system did you a favour by pointing out that an output is connected to another output.
If the error goes away if you remove the “+5V” or “COM2” symbol, then that suggests the error is “elsewhere” in the schematic.
However, you also write the error goes away if you change the pins of your DC-DC converter and I do not understand why that would change anything.
One way of determining if there is an error “elsewhere” is to make a copy of the project, then delete a part of the schematic and doe ERC again, and repeat. When the error goes away, the last part you deleted has the error.
Or if you zip the project and post it here then I (and probably some others too) are willing to have a look at it.
I think most of users (me too) when starting to use KiCad encounter an problem with power symbols.
If you change power symbol name at schematic it don’t change the net it is connected to (that is hidden in the pin settings in the symbol).
I have placed VCC and in another place once more the VCC and renamed it to VCC1 (another net after 0R). When designing PCB I noticed that he wants me to short my 0R with track because for KiCad both my power symbols were connected to VCC net.
So I have defined my own VCC power symbols (VCC1, VCC2, VCC3,…).
If at your schematic +5V and COM2 were looking the same I would be pretty sure it is the same case and you made one of them by renaming the other. But as they look different than may be as you were told you have the short somewhere else.
KiCad reports that two Power Output pins (of DC/DC) are connected together. If one is changed to be passive than everything is OK - it can be connected to power pin.
Duh, indeed. If you set one of the power outputs to “passive” then KiCad does not warn anymore about the short circuit, even though it is still present.
ERC is a useful tool, but it has it’s limitations. If ERC finds an error, then it knows something is wrong between some nets, and it shows that somewhere on the net. The ERC arrows for the errors are not always near the problem itself, but they are on the right net.
Paul, Thanks for the advice! You were correct. Deleting sections of the schematic helped me find the error in no time. Somehow a line got crossed, probably when moving things around and it automatically put a connection between two unrelated nets. It had absolutely nothing to do with the section or part that the error was indicating. Not very helpful checker if it doesn’t even get you close to the problem! However, now that I know this trick, it should really help me out in the future until somebody can figure out a better algorithm for that test. I think I am finished with my schematic now and now get to work on the PCB !!
The thing is the short was only detected because two outputs cannot drive the same net and a net like power or ground is far reaching. You as a human would have the same difficulty if say a board developed a power short somewhere and it shut down the power supply without any smoke or burns.
Yep… Exactly. It is like saying Hey you made a mistake, but I’m not telling you where. The more complicated the schematics get, the more you need this thing to at least flag the correct area to look in. I am not saying I am not glad it flagged an error, I am just saying it should be better at pointing out the real connection issue.
If you can figure out an algorithm that KiCad can use to figure out where you made the error, then one of the KiCad developers is probably happy to implement it.
A schematic is a symbolic representation not a spatial one, and a net can cover a lot of “area”. All ERC knows that you connected two power outputs together, but not whether this is legitimate or an error. Here is a situation where I deliberately ignored it.
To be smarter, the ERC would need more information. Perhaps it should be possible for the user to label power nets and connecting them should be flagged for scrutiny. But then you would have to be able to filter out legitimate situations where say GND is connected to GND1 on purpose.
Have you think about what you are saying? There is connection from one power output to the other so it is simply one net. ERC sees two power outputs connected to that net. There are a lot off connections at that one net. Which one was not intended? KiCad isn’t in your head to know it.
