That’s how I do it:
Symbols are all as small as possible and custom.
I asked the electronics engineer I work with which way he preferred it, and he chose this over the other, where you don’t see the power pins.
1 Like
Sorry, I wanted to post a description and example how I solved it.
But the post got censored by KiCad.
Hm… sure?
I’ve seen spam here, no such thing as real time censorship here, really.
Maybe the forum was busy or something, had that happen a couple of times lately…
Anyhow, would still be interested to read how you solved this, might learn something from it 
They say I’m a ‘new user’, but don’t tell me how to get old.
I’m not allowed to post an image etc.
Well, I just retired - and seen in geological dimensions - this is new.
Got it through the Design Rule Checker error free!
A good description how to do will take some time, letters and some images.
If you send a mail to dieter.kunkel@onlinehome.de, I will send you a pdf within some days.
You just gotta scroll down a couple of threads (read them) and post some… restriction lifted for me after 1-2 days I think.
If you click on the top right and your logo and then on ‘Profile’… there is a pane to the left… go to ‘Badges’.
If you click at one of those badges, you’ll see a list of people on this forum who got that too… click on the badge symbol at the top left to finally get to a page which explains how this forum works.
Or just click on this link:
https://forum.kicad.info/badges
Yeah, I wasn’t told either… just being curious and click-happy does the trick usually 
OK, checked that.
In simple words:
The power symbols are all inputs. A net with only inputs requires one single output connected. Could be a power output or a simple output from any component.
Got a working design with 3 insulated logic supply grounds and 4 logic supplies done. Well - and an own library of the logic devices and one of the powers I used.
1 Like
I’ve had the same problem, I had 2 x 4050 gates, I wanted 1 to be powered from 3.3V, and the other 5V. As the gate power pins are locked to Vcc, Vss (invisible pins) I couldn’t separate them. I had to do it manually in the PCB. This caused further problems, as every time I updated the schematic and updated the netlist in the pcb it would reset my hard work.
I’d suggest creating your own symbol with all pins defined
2 Likes
I have my own libs for logic devices, microcontrollers, etc. now.
Updated when something new comes by.
This way I also get a common style for the components in the schematic (everybody making a device seem to have his/her own style).
Open the ‘source lib’.
Get the component and modify to your need (power pin visible and defined as inputs)
Open the ‘target lib’ where it shall go in.
Press ‘save component’
Just some minutes for each component.
1 Like
Thanks for the tip. I’ve only just starting getting used to the library editor and copying components, and your right its not that slow to do either. It’ll definitely save me time in the long run with re-imports of netlists. Cheers.
Probably the best thing to do. Twenty years ago when an entire board of TTL logic ran at 5V, hidden power pins made tidier schematics. These days it is normal to see three or more logic supplies on one pcb and I would question if it still makes sense
1 Like
I’m often ask for parts replacement in system designed in the late 70s. And all these new high density electronics do not survive long if you go high off the ground. Radiation destroys these small structures.
Sold some ceramic 80286 to the NASA not long ago.
There are also components that look like an ‘normal’ ic, but the logic inside is built of small Tetrodes.
The lifetime is another problem if you have to think in decades. Bad with that ‘new’ stuff.
1 Like
It definitely does but needs to be done right. See how it is done in EAGLE for a good example. It makes the schematic much tidier and allows e. g. creating separated decoupling sheets with ease.
Something as described in this tutorial?
In short: multi unit symbol with an extra unit for power pins. (Has drawbacks in the current library file format that will be fixed in future versions. We hoped it will be included in v5 but this seems very unlikely at the moment. Most likely in v6 or in the worst case even later.)
We library maintainers see this as the best option with the current symbol library format. In fact, new symbols are not accepted with hidden power pins. (Sadly nobody volunteered to fix the current 74xx lib. Are you prepared to do it?)
Could it be scripted? A chance to practice my Python-fu…
We need a new symbol name or risk havoc with existing designs
old designs could use the rescue feature. (Or do i understand this feature incorrectly again?)
The library is also only rolled out with a new release (The next one would be 4.0.7). The current symbols live on in the commit tagged as 4.0.6.
This way one could download the old lib and use it to rescue old projects manually if the rescue feature does not work as intended.
If this rescue feature does not work as i think, we librarians might be screwed any ways. Especially after the recent major updates to the opto, regul and linear libs.
Of course. The lib file is text based, so one could write a parser for it and change the symbols in the desired manner this way.
I’m just not sure if it would be less work than doing it manually. Simply changing the visibility of the power pins does not correct these symbols.
- The power pins need to be moved to a separate unit
- The symbol needs to be given the property of “all units are not interchangable”
- the unit count needs to be increased.
- All graphical elements need to be copied to all units that are logical units. (the shared for all units property needs to be removed for them of course.)
- This needs to be done for the normal and the de morgan representation. (or we romove the de morgan representation.)
- The symbol body should be colored by the background color. (light yellow in kicad out of the box)
- Maybe something else needs to be done to them such that they fulfill the current KLC. (I have very little experience as a maintainer. But i think if all the points listed above are done the lib will be a lot better already.)
In short - yes. In a more elaborate way it is slightly more than only “extra unit for PWR pins”. It is also about making a subtle distinction between that “extra” unit and “regular” units. In EAGLE the supply units with their pins are hidden from schematics by default but automatically connected to their respective nets. Similar to what KiCAD does with power pins. Yet, unless I am mistaken now, the unused (not invoked in EAGLE terms) units are not automatically connected in KiCAD? Once this is solved I can imagine “fixing” the lib(s).
Is this a new feature? I never knew this was possible in eagle. (I used version 6.5)
I’m personally not a fan of auto connecting anything. Everything should be explicitly shown in the schematic. (Everything else is too error prone.)
As stated above, currently we don’t have much options. What can be done with the new library format remains to be seen.