How to invoke and separate power pins?

Hello,

Another Eagle user question :slight_smile: - how to separate a power pins to make a layout more readable? So basically, I want to move outside a power pins from an LM741 footprint.

Thanks J

Do you actually mean schematic and symbol, rather than layout and footprint? Layouts are usually not intended to be readable, and you can’t move the pins from their positions because they are part of the package.

Yes, I mean the schematic symbol - V+ and V-. Normally, I can do this in Eagle just using the “invoke” command, than it shows all of the parts of the package I can use (eg. PWR pins).

J

You’d have to edit a copy of the symbol to change the positions of the pins.

1 Like

In KiCad the LM741 has all pins defined in a single unit:

image

And so do the other single opamps.

It’s only with dual and more opamps that the power pins get separated in a separate unit. With the TL072 for example (see below) Units A and B are the regular triangular opamp symbols, while unit C are the power pins. This unit is designed to fit on top of one of the opamps, so you can use it either with similar looks as a single opamp, or collect them with other power symbol units in some power supply section.

1 Like

So basically, I want to move outside a power pins from an LM741 footprint.

To have the power-pins on a different position or on a different unit you have follow retiredfeline: copy the symbol to your own library and modify it. As example for a multi-unit-symbol with dedicated power-unit look at LTC1519. You could use that as starting point for your own multi-unit symbol.

Also please use the correct description - symbols are used in the schematic, footprints are used in the board-editor. Mixing these terms could make it difficult to understand you.

Normally, I can do this in Eagle just using the “invoke” command, than it shows all of the parts of the package I can use (eg. PWR pins).

Kicad has no invoke-command. If you want to “invoke” (==get more units from a symbol onto the schematic) a symbol:

  • just copy the existing symbol (maybe unit A)
  • now you have two symbols with same unit “A”
  • doubleclick second unit → you get symbol properties dialog → on the left there is pulldown-menu: General–>Unit. There you can select the desired unit. (see picture)
  • with v6 you are selfresponsible that you add all units to your schematic
  • v7 added a additional ERC-test to show you missing units
  • you have to take care of the unit-annotation. The individual unit-symbols are not as tight coupled together as in eagle - so keep an eye on the refrence-designators so that units which belong together get the same Reference-designator
  • In the symbol-chooser you could activate two checkboxes: Place repeated copies + Place all units. Try that (see picture), it will place all units directly at adding the first unit.

2 Likes

Thanks a lot for the clear explanation. I have already check some options and have solved the problem. I love KK more, and more. I’m long time Eagle user and boy… believe me :wink: some things are simpler and more straightforward with KK. Just finishing my first design in KK and it was flawless. Key commands are amazing. I will dive into my own footprints soon. during the years with Eagle I made some nice and big library of my own devices and footprints, I would love to import them if it’s a simple way to do it (?). And sorry for an incorrect description. J

1 Like