Why are certain relevant pins hidden in some schematic symbols?

Take for example, 4053 analogue multiplexer in the cmos4000 library.
VDD is set to hidden, which means it doesn’t appear in the schematic.
This seems an odd thing to do, since it is the positive supply for the IC. Is it somehow automatically connected to the power source (In Part Library Editor I see it is has electrical type:power in)? Even if that is the case, how do I know which supply it will be connected to, and what if I want to attach a bypass cap. Am I supposed to edit the component to make it visible?
I’m not complaining BTW, just not sure what I’m supposed to do :slight_smile:

The logic libs use a very old feature of kicad. If you hide a power input pin it becomes a global label. More details see FAQ

A long time ago some contributors thought it would be a good idea to make the logic symbols that way.

The reason as to why this is a bad idea nowadays is that you can no longer say that most pcbs will have only one power supply.

The new library convention would not allow that. The lib that will be shipped with kicad version 5 will no longer have this problem.

That is very helpful, thank-you. Another reason to look forward to version 5.

Meanwhile I will edit the symbol to make the pins visible

The problem is that you then have these pins more then once. This can result in invalid netlist creation.

Have a look at this: IC footprint VCC+GND

Here i explain everything in more detail and even add a tutorial as to how you can make correct symbols with a separated power unit

Ah yes, I see. The explanation of the problem and tutorial is very clear. Thank-you.

That long time ago was from a time it was common to have 200+ TTL chips on a PCB which all had the same GND and Vcc connections. (PCB’s were big back then, really big). And it did actually make sense back then to hide the GND and Vcc pins.

Fast Forward 40 years and we have multiple power rails with different voltages going to the same chip.
Not only for the big guys (FPGA, Multi GHz CPU’s) but also small uC’s with an USB interface often have 5V and 3V3 power connections, and onboard voltage regulators are also common.
The occasional TTL chip still used is often for interfacing or level conversion and then you really want to know to which power rails to connect the Vcc pin(s).

Thanks again for that tutorial. I’ve just tried to follow it using the same 7400 component. All seemed to work OK, but I’m a bit puzzled about the result. Now when I try to load the modified component in Eeschema, I have a list of Units A-E, with E having the power pins. So am I meant to load for example Unit A and then also load Unit E, and place it on top of Unit A? If you can clarify how to load and use the new component with separate power unit that would be great.

To use the component you will need to add the unit containing the power pins and connect it to the appropriate power levels.

You also of course need to at least add the logic unit you want to use. (Ideally you load all units and connect the unused input pins to ground.)

If you want you can put the power unit on top of one of the logic units (If it is designed that way.)
But you can also put it on a separate sheet with all other power pins, next to the logic stuff, …
This is all dictated by your personal preferences. (The new symbols in the kicad 5 lib are not designed such that you can overlay the power pins with the logic parts as the power pins are encased in a rectangle.)

1 Like

Aah I see. I misunderstood the purpose of units (silly me). They are to encapsulate parts of a component and allow separated symbolic representation of the units in the schematic.

I’m used to seeing components represented as as a single package in the schematic. I’ll have to read up and look at some examples.

It is quite common to have one page just with the power blocks and decoupling capacitors.

1 Like

Interesting, thanks, I can see that would keep things tidy.
I have a follow on question about using components with multiple units:

If I use a component twice (say I use a pair of dual op amps like OPA2340) and that component has two units, then how can I associate the units of the same chip with each other. Or in other words, if I load two unit As and two unit Bs, how do I know which unit belongs to which IC. Hope the question makes sense…

When you place the components you choose which gate (A, B, or C assuming you have the power pins for the opamp in gate C). Then when you auto annotate the schematic, eeschema will make a guess based on the order that it finds the gates based on the scanning direction. It’s up to you then to verify that the right gates get paired together.

Before annotating you would have two U?A, two U?B, and two U?C. After annotating (I’m making up numbers for illustration) you would then have U2A, U2B, U2C, U7A, U7B, U7C. It is then up to you to make sure that the sets are correct. Which gate C is which probably doesn’t matter unless you are providing them with different power rails.

1 Like

That makes perfect sense, thank-you.

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.