Floating DC to DC IC ground connection

I am trying to insert a symbol of type XP_POWER-IAxxxxS_THT specifically 0512 (5vin ±12V out fully isolated). So, I connect the input to 5v, the input ground to ground. But, when I try to connect the 0v output to ground I get an ERC error telling me that an output is connected to ground. That is not unreasonable given that the model is defined with +12v, -12v, and 0v as “w” - outputs. Since outputs cannot be connected to outputs for ERC, that is perfectly sound advice. Now, I could make another model with 12v labelled as “W” (input) but of course someone else might want to connect +12v or -12v to ground, not 0v.
So on to my question - is there any more elegant route to connect 0v to ground that inserting a zero ohm resistor? I tried “net-tie” but that gives the same ERC error.

Please post your schematic (or a screenshot).
It’s not clear (at least to me) from your descriptions what other “grounds” of power output type you are connecting together. Note that a “GND” power label is technically a power input, specifically to avoid this kind of DRC error.

Here goes, but this is a first for me.

The PWR_FLAG in the bottom right is the culprit.
If your “ground” net is actually being driven by a power output (in this case the converter’s 0V pin) as opposed to, say, a terminal block with only passive pins “supplying” your schematic, you don’t need that.

Another note: Using the same ground on both sides defeats the isolation. Is that on purpose?

I don’t need isolation - just ±12v in a circuit originally being supplied from between 12v and 28v DC which then produces +5v. The IC is just to get ±12. I will remove teh pwr-flag and see what happens, but I think I recall many other errors.

I took the IA0512S from the default library and all three secondary pins are defined as power output:

while, if you take for example an 7805, the GND pin is a POWER INPUT".

Removing the PWR_FLAG from the GND net should not matter. The Net tie (Which is a real PCB Footprint, consisting only of copper) should isolate the nets.

As the net-tie option should work and I think the problem is elsewhere.
Without the net-tie, the current solution / workaround would be to copy the DC-DC converter into a custom library and change the electrical type of one of it’s pins.
KiCad V6 will have improved upon this, with options to suppress specific ERC errors.

In this case, the net tie is “shorted” by all the GND symbols.

Edit: nonsense, I was confused

Any chance your LM78’s GND pin is erroneously a power output?
Something’s amiss in that schematic and it’s not the DC/DC converter.

If you zip and upload the whole project (or at least the .pro, .sch and -cache.lib files) I’m willing to have a look at it.

But start with reading the output of the ERC check. It’s possible that a single error causes lots of error messages, and maybe only one of the messages has a clear hint to the root cause.

On top of that, pins 10 of your “Dongle1” seem to be connected, and it looks intentional, but I’m not sure.

Those small SMPS modules also often rely on external (electrolytic) capacitors. Check the datasheet of your IAO512S.

I have to stop tonight. I will try to reduce the circuit to some essential components to see if the symptoms change. I apologise for showing the net-tie - that was my attempted “fix” to the error when it was linked directly to ground. I am an amateur in grounding in kicad although I read somewhere that grounds are normally “inputs” not outputs. I think what I will do is to put in several isolated power supplies and configure them in innovative ways such as putting connecting the -12V to the +5v supply to give me +5v, 17v and 29v supplies and see what happens.

There is no need for this:

Pins are defined as power output, and therefore they WILL generate ERC errors when connected to each other.
See the error matrix of the DRC check:

I will try to simplify the circuit. I think that the dongle is just confusing since it isn’t a known component and has been artificially handled using two single row sockets - it has no model of its own.

I have not yet figured out how to post the output of the ERC check since copy/paste is not permitted. I tried to save a copy but got mixed up with finding text editors so I gave up for the moment.

The use of the 5 to ±12v module has been in use for some years in a circuit much like this - I am trying to change over to Kicad from software obsolete since the late 80s. Most of the circuit isn’t new, only to Kicad.

Ah, I sort-of suspected as much despite it being technically possible to do with an isolated supply.

There is a checkbox in the ERC window with:
" Create ERC file report"
and if you check that before ERC, it asks for a file name to save the ERC errors.

If you want to “stack” the outpus of such modules, it is a perfectly legal thing to do. One of the many tricks you can do with such isolated modules. But it does confuse KiCad. Your options are:

  • Ignore these ERC warnings (can be suppressed in KiCad V6)
  • Make copies of the symbols to a custom lib and change the Pin types.
  • Use net-ties or similar.

Well, I was in a hurry but I tried that and it started asking me for an editor - I will get on to that tomorrow.

The point is that every power net should contain exactly one power output (which is either a power output pin on a symbol or a PWR_FLAG).
This means that every GND pin that’s not unequivocally an output (only the DC/DC converter in your case) should be of power input type (all GND pins of your components and also the common GND on the LM78L05).

You may be able to suppress the DRC error by changing the converter’s output pins to power input but that’s a crutch, not a solution.

Maybe I should have added that without linking the 0v to ground (just nc) there are no ERC errors reported for the remainder of the circuit.

I think that the reason that the writer of the converter labelled the 0v an output, is that it can be. There is really no inherent reason why any one of the 3 terminals should not be the “input” as I hinted with my proposed experiment. I suspect that without the crutch, there is no way of suppressing the error i.e. once a pin in labelled as output, Kicad has no way of knowing that it could also be an input i.e kicad willl treat +12v, 0v, and -12v identically. If I am not able to link +12v to ground then I will not be able to link 0v to ground for exactly the same reason??

The reality is that the rule for this component is that “any one of these 3 pins can be an input, but only one, the other two are outputs”

No. I don’t think we’re on the same page here.
Power output/input is not current source/sink, ERC-wise. Regard it as power output meaning “supply” and power input meaning “demand”.

Simpler example: A battery in a KiCad schematic has two power output pins. You connect those to a random IC’s Vcc and GND pins, which are both power input. Add GND and +V symbols (also power input) if you like.
Result: ERC is happy.

What I’m saying is: your schematic above should be fine without adding a net tie nor changing the 0V pin type. The error is caused by something else. Stacking isolated converters is a different story.