Symbol with multiple units

Hello members
I created this AD8608 IC which has 4 units…As it can be seen that pins 4 and 11 are common to all the units…but i am confused,how to connect these pins.should i provide voltage and ground to one of the units or what…please suggest.

Those pins should not be common to all the units; you should create an additional unit with only the power/ground pins. That’s how the symbols in the library do it.


You did not create that from scratch did you?

This is the default library symbol for a TL074.
Pin assignment for the majority of opamps is interchangable, so you can add an alias for your AD8608, or copy one of the other quad opamps and give it an AD8608 name.

Note the separate ‘E’ unit for the power pins.
This is usually hidden in some corner of the schematic, or even on another sheet, together with the power supply circuit and the decoupling capacitors.
It’s there on the schematic when you need it (and gets imported into the PCB) but for the circuit itself you can concentrate on it’s function and not be distracted by the power connections.



As others have suggested one option (that i personally prefer) is to have the power pins on a separate unit. Downsides: you lose the exchange units feature (which i personally do not really use anyways) and ERC will not report that you did not place the unit holding the power pins. (ERC never reports unplaced units but if you have the power pins on all units then it will report that you need to connect them.)

But you can keep the symbols as they are. You can then (since version 5) connect the power pins on any of the units. KiCad should even report an ERC error (since 5.1 or possibly 5.0) if you connect the same pin to different nets this way. Downsides: You will have open connections on your schematic that look like a mistake (and i am not sure if KiCad might not even report them as a mistake)

By the way i go into great detail how such a symbol can be made in Tutorial: How to make a symbol (KiCad v5.1.x)


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