Is this intended behavior that a power input GND pin will automatically connect to a global GND net? If so I don’t understand why this would be the intended behavior.
I’ve been struggling to understand why my GND and GNDPWR nets were shorted together, and finally managed to track it down to a symbol with a pin called GND with the “power input” pin type.
Maybe I misunderstand the “power input” electrical type, but GND automatically connecting to a global label seems very counterintuitive to me. When I have split grounds, I can no longer use the GND symbol or I have to change all the “power input” pins to “input” pins.
Does anyone have insight on to why KiCad does this?
In KiCad all power symbols are not much more then glorified global labels with some extra graphics to make it look fancy. This is for the power symbols, not for regular schematic symbols, in which GND is (nearly?) always a power input. (It has to be a power input, even for voltage regulators, because multiple voltage regulators can share a common GND wire.
No. Not true. You can leave the symbols as they are, but you do have to connect the GND pins to different GND nets.
But this still does not explain:
My best guess is that your LT1161 is defined as a power symbol, and not as a regular symbol. LT1161 is not in the default libraries. Libraries from external sources tend to have more errors. “Normal” symbols should never be defined as being a power symbol, even when they are a voltage regulator.
In 80s all digital ICs were powered by 5V and there were symbols for all TTL family that you need not to show at schematic their supply connection as it was done automatically in hidden way.
I have never used KiCad libraries, but I remember from forum discussions that KiCad had some libraries made that way (KiCad V5 times). I don’t remember how it was done (pin made like in power symbol and hidden ?) and I don’t know if such libraries are still among current KiCad libraries.
From what you write it looks that KiCad still have such libraries and you just found one of them.
@George_Sleen
You’re quite new here, Probably also new with KiCad. Can you share a (small part?) of your project? This allows us to make a better diagnosis of what’s really going on and determine if it could be related to some bug in KiCad.
You’re still a “new user” and due to the automated spam bot you can’t upload files yet. For info on how to fix that, see: New Member Information
Yes that did seem to be the issue, thank you for the fix!
There were two pins named GND, and I followed some of the KiCad symbol libraries when designing the symbol to set all but one of the GND pins as invisible and stack them on top of each other. I checked again though and it seems that all the libraries have the invisible pins set to “input” rather than “power input”
I had a look at the manual, just to see whether it was clear, and it does not only write it down neatly, it also has an extra note warning for exactly this situation:
2.8.4. Hidden Power Pins
Note:
Care must be taken with hidden power input pins because they can create unintentional connections. By nature, hidden pins are invisible and do not display their pin name. This makes it easy to accidentally connect two power pins to the same net. For this reason, using invisible power pins in symbols is not recommended outside of power symbols, and is only supported for compatibility with legacy designs and symbols.
