KiCad 6 VCC & GND pins. I do not want all the VCC pins connected

I have a board with 5 different GND and VCC areas that are 1000V apart. As soon as I added digital parts all VCCs and GNDs are now connected together.
Last time I made parts without names on the power pins. I think there is a way to edit the parts in the schematic, but it is not working for me.

Ideas please, thanks.

don’t use symbols with hidden power pins.

1 Like

Good advice but for me using such symbols not explains a problem source.
Why without them 5 GNDs were not connected and this symbols made them connected?
If all GNDs were the same net than they should be connected even before and if were different nets than digital parts should connect (depending of net names) to none or only one of them.

Say there is a small circuit that sits on the power line-1, line-2, line-3 and Neutral. (three phase) Then through isolators, signals are sent to a circuit sitting on earth ground. The isolators (I made) have the power and ground pins named 1, 4 & 5, 8. PLgnd-1 does not connect to PLgnd-2, etc.
I am using a part 74LVCT1G08, small AND gate, with “VCC” and “GND” pins that force all the nets they connect to, to become VCC or GND. Once the AND gates are connected all PLgnd-X become GND, across all pages of the schematic.

OK, I think I need to copy any digital gates I am using to my LIB and delete the pin names. (or maybe change the power pins to inputs) Maybe I need to study why an OP-AMP with VCC & VEE does not have this problem, but logic does.

Depends on how you read OP’s wording. It could be that OP thought of the 5 areas (that’s the word used) as “ground” albeit a local one before attaching a power symbol, global label, or a part with a hidden power pin, to each of them.

OP, sounds like you are using the older digital symbols which have hidden power pins. The recent ones have power pins in a separate unit.

You are right. Go to every logic gate, edit, edit symbol, select the power & ground pins (hard) and mark them visible, save every time. This only saves to the schematic not the library. Now the pin will not rename the net.

The better is to edit library once than edit each symbol at schematic.

For me it is still not clear.
Placing part with hidden power pin can’t make automagically this connection, I think.
If PLgnd-1 is not connected with PLgnd-2 than placing 1G08 with hidden GND pin at both sheets not connect them. But when you want these 1G08 to be connected to these isolated grounds you need to add GND symbol and connect it to PLgnd-1 and at other sheet you also need to add GND symbol and connect to PLgnd-2. But in such case it is you who connected both PLgnds to common GND. I simply can’t imagine how it is possible that “As soon as I added digital parts all VCCs and GNDs are now connected together.”.
In my opinion you had not only to add those digital parts but also add GND symbols and do the connection of your isolated GNDs to common GND (trying to connect it to 1G gnd).

This suggest me that 1G symbol used has a way to be connected to PLgnd-X so it is not what we suppose a symbol with hidden GND pin. But if it has not hidden pin than it should not connect to global GND net. At least I think so, but I have never used any KiCad digital symbols library.
If symbols you used has GND pin visible and it connects it to global GND net than it is certainly wrongly defined symbol. I didn’t expected such bugs in KiCad libraries.
I use only my own symbols and have full control on what is going on.

All hidden power pins have now been removed from the libraries, this was done before the v7 release. We strongly recommend upgrading and then updating these parts from the libraries because of exactly this issue. Many discrete logic parts used to have hidden power pins causing exactly this problem.

Background: A long time ago, a very poor decision was made to turn all hidden power input pins into global labels named by the name of the pin. For backwards compatibility reasons, we need to support these in order not to break older projects. As a result, hidden power inputs automatically connect to all other global nets of the same name. Over time, we’ve slowly been removing parts with such pins from the libraries, specifically for this reason. This work was finally completed for the v7 release.


We all the time don’t know where from OP took symbols he used.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.