Had you try add PWR_FLAG for the GND net? It may just because the ERC stop there since Pin 7 are actually the identical event it draw on two location.
Hi!
As the OP I can confirm that I used the standard library. I can also confirm that in desperation, I tried the pin definitions in all flavours (power input and output) to try to find a solution (and in fact ended up defining the pins as “passive” to prevent the error - I know, not the intention, but it was a clunky solution to an annoying problem). I also changed the layout of the pins to be (for me) schematic friendly).
Goz
Also, I never/rare use Power Output pin for symbol, event with regulator output IC. ERC will not understand the circuitry that well. So any 2 or more power output pins get on same net it will yell. Event the power symbol. This is why, it very hard to find the reason for using this Power Output type.
I thought GND was a PWR_FLAG by definition? No?
Goz
I don’t think so. No exception for any power symbol including GND. Sofware treat all the same kind of symbol.
No it is different as explained above.
I simply think the benefits of having power pins on a separate unit outweigh the downsides. If you design such a part properly then you can overlay the power pins with your normal unit and get the same result as if you have it on a single unit. But you gain the massive advantage of being able to have all of your power stuff consolidated in a particular place.
The main downside is that kicad does not check if you have all units of a multi unit symbol placed.
Hopefully the new file format will be more flexible in this regard.
Oh dear, now I’m confused. From your “above” Rene, I’m assuming you mean the link you sent. Well there it states the following:
So the GND flag is actually a “power input” meaning it could be able to be connected to a “power output” OR a “power input”, which makes sense. As such, I think my problem lies with the fact that EEschema can’t deal with two modules having the same power input and ground pins for both modules, as both you and SembazuruCDE have both commented.
However not connecting the power and ground of one module, brings yet more problems:
Goz
Got it. Thanks. I’m using a duff schematic from the standard library 
Kann mal passieren.
Thanks again.
Goz
I would say depend. I had try both styles, I end up that conclusion. It help my coworker review schematic much easier. When I have about 10+ such part on the schematic, I very hard to not make a dump mistake (not connect power to the part). So I like to have power pins on every units (there are always exception to this).
@Rene - so I’ve now included a third unit for power only and superimposed it over the first unit and connected it all up and now have the following:
So I connected the grounds together and defined the GND pin as a Power Output and got the following:
Success! So the GND Pin needs to be a Power Output, right?
Goz
which gnd did you define as power out? I hope not the one of U1!
Place a power flag near on the gound net near where you connect ground to your external power source. (Most likely a connector)
Do it this way to ensure that ERC can detect if you have connected the ground pins of your symbol to where you get power into the PCB
@Gozzle: I hope you not ignoring my response. I were telling you to add PWR_FLAG for the GND. And should not try to use Power Output type for any symbol as much as you can.
GND is a PWR_FLAG according to my KiCad. Or which PWR_FLAG do you mean?
there is a symbol called PWR_FLAG.
It is in the same library as the GND symbol but it is for a very different purpose.
The PWR_FLAG symbol has a single pin defined as power output. It is intended to mark the place where you supply power. (The connector where you connect to your external power supply, after a passive device in the supply line like a fuse, …)
The GND symbol has a single hidden power input pin. Such a pin is a global label (yes this is hacky). Such a symbol is called a power port or power symbol.
More details see: ErrType(3): Pin connected to some others pins but no pin to drive it
Please go down to section #43, or search for “PWR_FLAG” in following page:
http://docs.kicad.org/4.0.5/en/getting_started_in_kicad.html#using-eeschema
I don’t like the way they use it in this tutorial. By connecting the power flag directly to a power symbol you loose the reason to have it. I would suggest to place the pwr_flag symbol as near as possible to the place where the board is supplied.
2 Likes
YIPPEEEE!!
I’ve got a three module LM556 and the Vcc and GND pins are “Power Input” pins. I flagged the GND input pin to my board as a PWR_FLAG and it all works!
Thanks to you all for your patience with me. I’ve learned so much about KiCad just because of this one single problem.
Time for bed…
Goz
A PWR_FLAG is virtual schematic element with the pin set to Power Output.
How many different ways can a multi-pin connector have power applied to the PCB from the Outside World?
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.