How to define symbols for individual components inside one chip?

[max.wwwang]

New user of KiCad here.

How can we define symbols for the components (such as a logic gate) of one physical chip (such as a quad 2 input and gate chip), so they can be used in schematics conveniently and intuitively as standalone components, but they are still 'associated' with the chip information (maybe footprint? I don't know), so will be 'integrated' into one single physical chip at the PCB stage?

Thanks.

[golden_labels]

In the symbol editor, when you create a new symbol, the dialog has a field labeled “Number of units per package”. If you choose a number greater than 1, the symbol will have multiple separate units — similar to what you see with gates from the standard KiCad libraries. Then you can edit units separately, by choosing the currently edited unit from a dropdown menu in the toolbar (towards its end). The next icon in the toolbar controls, if pins are copied and synchronized to all units. In some situations you do not want that.

[LazyJack]

Also don't forget to assign power pins to either one of the units or create a separate unit with just the power pins. Provided of course the package has power pins, such as an IC and not a resistor network for example.

[max.wwwang]

Beautiful. Thanks!

Also don't forget to assign power pins to either one of the units or create a separate unit with just the power pins. Provided of course the package has power pins, such as an IC and not a resistor network for example.

If I define a separate unit for the power pins (say Vdd/Vss), do I need to include this unit in the schematics for each chip of the same type (each will have its identical component number, except the suffix for the units such as "A/B...")? If there are multiple identical chips, this seems a bit redundant (because there will be multiple copies of power units, which look a bit boring). Probably there is a smart way to make the presentation neater?

[LazyJack]

Well, in theory you could make hidden power pins, when the pin is hidden on the part and labelled and thus automatically connected to VCC, GND, etc. This used to be the setup with old <V.5 KiCAD libraries. However, this is now discouraged (I don't like it either),because it can cause more problems than the small inconvenience that it solves. First of all, you are now bound to the power lines defined in the part and it makes things like having separate GND for different parts of the schematic, etc. I think it is a good thing to have every connection visible on the schematic and not having nets automagically connected in the background.

So in practice, yes, you will need to list all the power pins. This is not unheard of, seen t on many schematics. Or alternatively, you could add power pins to one of the identical units, so say unit 'a' will have two extra pins for power. 

[Doctorandus_P]

Yes, you need to connect all power pins of each IC.

In the old days when Big PCB's were made with 100 or more TTL IC's, it made some sense to implicitly connect the power pins. But in modern times and multiple (and sometimes isolated) power supply rails and different operating voltages for IC's it makes more sense to just put everything on the schematic explicitly.

If you have a bunch of IC's, then I usually make a simple two sheet hierarchical sheet schematic. In that case I put the power supply section, all decoupling capacitors and power pins on the second sheet. You could add a text note of where to put the decoupling capacitors, but as I know the engineer who draws the PCB for my schematic (also me) is capable, I just draw "enough" of them in a row and tug them away in a corner.

Also:
But why ask?
Just draw the schematic, depress >[F8] to port the thing to the PCB and you'll see soon enough which connections are recognized. Especially for beginners I recommend to do this multiple times as your schematic grows. It gives you hands on experience and verification whether the things you do work as expected.

The "extra sheet" can also be used as a placeholder for other extraneous things such as mounting holes. I do include these in the schematic, because it's an easy way to be sure they don't get deleted "accidentally" during the PCB design phase, which usually has many update cycles.

[max.wwwang]

Thanks. I'm ok with making everything explicit and under my control without business going on under the table. It's merely a matter of copy and paste, or at most, an extra sheet. Asking just in case there are smarter ways of doing things (which is almost always the case) and didn't want to waste time on bad practices and would rather stick with good ones.