Question about multipart symbol

[sugenganthos]

Good morning,

Here I have questions about symbol. Example is TL084 : quad jfet op-amp. So I have 4 alternatives for creating library.

1. Using single part. Drawing A square with 4 opamp inside. Some documentation use this. No question.
2. 4 parts, one of them has power pin. I can’t use option “all units all interchangeable” because one part which has power pins can’t changed. Or the power get disconnected.
3. 4 parts, all has power pins and marked “common to all units in symbol”. This can use “all units all interchangeable”. Question: do i need to connect every power pins in schematic or just one of them is enough? (Others keep unconnected, without additional no connect flag). Also not trigger ERC error.
4. 5 parts: 4 are opamp, 1 is power pins. This can’t use “all units are interchangeable” because of power part.

So, please answer question for alternative no.3.
Also, which preferred alternative for creating library (between 2,3,4)?

Thanks

[ML9104]

KiCAD 7 Creating Schematic Symbols with Multiple Units

The KiCAD Symbol Library contains many multi-unit symbols. The simplest way to visualize units is to think about something like a quad op-amp, eg, LM324 as the symbol, and each of the four op-amps as units (A, B, C, D). Important to know is that the units do not need to be the same! As always, creating or editing symbols is only possible in your personal libraries, the standard libraries supplied with KiCAD are read-only. More information in this FAQ: Additionally, it’s a very good idea to k…

It makes sense to check the FAQs and consult the KLC.

[Claudio.Lorini]

Good evening,
i’d go with 3. You can connect power/gnd to just 1 instance, afair the ERC does not complains.

[tryitagain]

It is not unusual to flip an opamp top to bottom (keyboard shortcut ‘y’) for company convention, flow, and/or schematic readability. If power and ground are attached to that instance then they will be flipped as well with power being on bottom and ground being on top of the symbol. Electrically it doesn’t matter but it hurts to look at it.

Having dealt with that issue a few times I now keep the power/ground connections for opamps as a separate instance.

[ML9104]

@sugenganthos

5 parts: 4 are opamp, 1 is power pins. This can’t use “all units are interchangeable” because of power part.

I think you are misunderstanding unticking this. It does NOT mean that you can’t swap the opamps as you llike. Of course you can.
It’s there to make it easier/faster to create multi-unit symbols.

[ML9104]

@tryitagain

It is not unusual to flip an opamp top to bottom (keyboard shortcut ‘y’) for company convention, flow, and/or schematic readability. If power and ground are attached to that instance then they will be flipped as well with power being on bottom and ground being on top of the symbol

That pain has a solution in another FAQ:

KiCad 7 Alternate Schematic Symbols: How to Create Them

This FAQ is about regular and alternate schematic symbols in KiCAD, a feature that can be extremely useful. It is only possible when using Personal Libraries, the reasons are explained in this FAQ: Read it first. Is there an alternate symbol functionality in KiCAD? Yes, it’s there, but it has a non-obvious name: De Morgan. Originally made for logic gate transformations, it’s universal enough to be used in a general way, which is nice. The official documentation does not really address this…

[Piotr]

@sugenganthos

Good morning,

It is 21 here

@tryitagain

It is not unusual to flip an opamp top to bottom (keyboard shortcut ‘y’) for company convention, flow, and/or schematic readability. If power and ground are attached to that instance then they will be flipped as well with power being on bottom and ground being on top of the symbol.

Since ‘always’ I used for it De Morgan but if I were needing such symbol now I would probably consider having 5-th part with power pins made such way that I would be able to place it at anyone of OpAmps making it looking like power pins were part of OpAmp symbol.

[mf_ibfeew]

Also, which preferred alternative for creating library (between 2,3,4)?

You have to decide this for yourself. The good thing is: all options work, so no decision is really false.

In my normal workflow I mostly use option 4.
And yes, the “all units are interchangeable" checkbox must be unticked.

[sugenganthos]

So, that option just for remainder to engineer of that symbol is “safe” to swap. And no additional function on schematic (ERC, or perhaps auto populate). The real function is on symbol editor. Is that right?

Then I go on alternative no.2, with DeMorgan symbol for swapping in+ and in-.

[ML9104]

Options 3 and 4 are “safe” in your case. For option 2, you’ll have to reroute power for the opamp having those pins.
It’s in no way ideal, and I have my issues with it as well.
I use the KLC way, and if it gets too dense, I stick all the “unit 5 symbols” (power units) in a hierachical “Power” subsheet. I generally do that anyway for the power supply circuit.

[retiredfeline]

I prefer a separate power unit. That gives the freedom to place it anywhere and not clutter the circuit around the opamp.

[sugenganthos]

Aha, another way to use “power” sub-sheet. I had separate power pins also. And usually placed on one of the op-amp. So I can swap the opamp pin while keep power pin keep ‘up’. Then hides the ref & value text.