CD4051 power pins not available in schematic symbol

[zenseidk]

Hello friends,

I’m building a circuit where the CD4051 analog multiplexer is used, but I’m not able to connect VCC and ground in the schematic. I tried making a new schematic symbol with pin 16 VCC and pin 7 GND, but when I choose that symbol, it just adds the old one to the schematic, even though I can see in the preview that it’s the right symbol I’ve chosen:

Am I missing something here or is this a software glitch?

Any help is much appreciated, as I am unable to connect power to the chip as of now…

Thanks

[zenseidk]

When the symbol is added to the schematic, the VCC and GND pins are still missing:

[Rene_Poschl]

Sadly the 4045 lib still has a lot of symbols that rely on invisible power pins.
I would suggest you copy this symbol into your own lib, rename it to something that makes sense to you. (to avoid name collision)
After that edit the vcc and gnd pin of the symbol to be visible.

You can use the invisible pins if you want. (Be aware that they are dangerous, especially if you have multiple power supplies.) Just place a power symbol with the same name as the pin names of the symbol and it will be connected.
(Invisible power pins are global labels.)

Invisible power pins do not allow for a usecase where you have multiple ICs on different power supplies. It is your decision what route you go.

[Joan_Sparky]

They are hidden.
See several threads about this on here:

New symbols for 7400 library

I have been working on new symbols for the 7400 logic library (74xx.lib). One major goal is to remove hidden VCC/GND pins, which are now considered “old hat”. Additionally, the current symbols lack consistency and most are not conformant to latest library conventions (KLC 2.0.4) Therefore I have extracted data from the current lib, and regenerated the symbols using a script. Some of the existing symbols already have visible power pins, so I have not included those in the new library, which for…

Problem with hidden pins

Hi, in my circuit I would switch on and off a schmitt hex inverter with a transistor. So I switched on the Show hidden pins icon and connected the transistor to the GND pin of the 74HC14 (ERC doesn’t give me errors). But in PCBnew it doesn’t works as expected: it grounded both pins of the transistor and the pin 7 of the 74HC14. I’re read somewhere that, if I make a direct connection to an hidden pin, it overrides the automatic rule of attaching the pin to power rail. But looking at PCBnew it …

Is this a bug in Kicad? (Later discussion how to add libs if github plugin not compiled)

While working with Kicad I’ve noticed some peculiar behaviour. Although the schematic clearly shows there’s no connection between any pins on a DIL16, it still connected both power inputs (Ucc and GND) in the rats-nest in PCBnew. I can manually correct it by editing the .net and .xml files, but it shouldn’t happen, IMO. I didn’t test it with other sockets. Version info: Application: kicad Version: 4.0.6 release build wxWidgets: Version 3.0.2 (debug,wchar_t,compiler with C++ ABI 1009,GCC 5.3.…

Dual and Quad OpAmp symbols (solved)

Hello, I need some help with the use of multiple-part components. I want to use a quad opamp (TLC074), but I couldn’t find enough information on how to properly create a multiple part component. Also, when I insert, in Eeschema, a dual or quad opamp symbol, I only get ONE opamp symbol. I have already managed to create a PCB and also a custom component, but here I’m lost. Could anybody put me in the right direction ? Thanks in advance ! Franz

[zenseidk]

Thanks for your replies.

I tried making a copy library, saved to the project folder and added Vcc and GND pins so that they should be visible.
But when I add THAT library, there are still no power pins.

That is what I was trying to convey in my previous posts.

[Rene_Poschl]

You need to move your personal lib to the top of the priority list.
In kicad symbol names need to be unique over all libs. If kicad encounters multiple symbols with the same name it will only use the one of the lib with the highest priority.

Above i suggested to rename the symbol to avoid this problem
More details:

Any conflict with names of modules and libraries?

Newbie here, slogging along the learning curve. Managed to create some new footprints and libraries - happy camper. I have questions about good file management practice. Here’s my setup: I have a folder (“librariesAdded”) where I put all the new libraries I create or download. Inside that folder I have another folder (eg. “arduino-1”), and inside that folder I have arduino-2.lib and another folder (“arduino-3.pretty”) and inside the .pretty are the kicad-mod footprint files. Like this: Librarie…

[thawkins]

For many packages such as quad or hex device packages, i discovered that there was an extra “Unit”, for example on the 7407 library symbol which is a hex buffer, there was a unit “G”, which is a 7th unit on a hex package. Selecting that just produced a box with a pin 14 and pin 7 on it, for connecting up the power.

[Rene_Poschl]

This is new in the version 5 library. Sadly still not for all symbols.
The version 4 lib (which was the topic handled in this thread) did not come with this. There the pins where defined as invisible power input pins which makes them global labels.

[davidsrsb]

And breaks your design if you have one chip on 5V and another on 12V. You end up with the two power supplies shorted