My thought was (again using +5V as an example), the +5V_Source symbol with the hidden power output pin named +5V would only be used one place, ideally where both you and I suggest using the PWR_FLAG symbol. Everywhere else the regular +5V symbol would be used. What would show on the schematic is the symbol name (+5V_Source vs +5V) so it would be obvious if the source symbol would be used multiple times. If the designer does accidentally use the source symbol more than once ERC will flag one of them, telling them to fix it.
I don’t know if I’ll have a chance to experiment with this in the near future, but I thought I would throw the idea out before I forgot it.
I think the use of multiple symbols breaks down for such a usecase. Something similar to the not connected on purpose marker might however offer a more flexible solution (That tool could then have a property for the voltage level for example)
It is true that my suggestion would basically double the number of power symbols instead of only having one extra symbol as it is now. But it might be more intuitive to the new KiCad user (or the non-KiCad user reading a schematic generated in KiCad) than the inscrutable PWR_FLAG symbol. Honestly, my intent isn’t to give the librarians more work. You and your team have done an incredible job tackling the Sisyphean task of library management, all in your spare time.
While, yes, something similar to the not connected marker might be more flexible, that doesn’t exist (yet). So my idea is how to handle the ErrType(3): Pin connected to some others pins but no pin to drive it a little more elegantly with the tools that we currently have. How does something called “FLAG” drive anything… Having a power source type symbol that links to regular power symbols conceptually makes sense to drive other pins.
But this is all academic unless someone is able to prove that this idea does or doesn’t work with the existing KiCad stable release. As I mentioned above, I don’t think I have time to experiment with it. But if anyone else wants to take up that mantle…
Though, of course, the counter argument is it may not be intuitive to someone who doesn’t know how KiCad does things that a power symbol called +5V_Source is on the same net as +5V and might think that they are two separate power nets… More thought is required…
There is no getting around the fact that some item must be the source. KiCad, now with V5 has a separate field in the symbol library called “Symbol Name”.
If it becomes allowed that power symbols were to also be tied to a net, then all that is needed is for the duplicate Pwr Symbol to have it’s pin as Power Output.
The text does not have to be different when the symbols are placed, and a menu toggle similar to Show Hidden Pins could show the Pwr Symbols pin description.
There is going to be some ambiguity no matter the solution, and this does not seem to me like a bad solution. And, I think for some, 5V_Output and 5V_Input makes sense in a basic logical way.
I read threads on this forum to learn about KiCad since I am a very new user and know very little about electronic circuit design so I know I am not an expert by any stretch of the imagination. I have only posted a few times so I don’t want to step on any toes here but I think it needs to be pointed out that the screenshot in the first post of this thread is not a circuit created by the original poster. It comes from section 6.5.4. Power ports connection in the Eeschema Reference manual.
Since the very first response states that “The way power flags are used in your screenshot makes them basically useless…” then isn’t the first thing that needs to be done is to correct the documentation?
The way hidden pins work electrically is they connect to the net that shares the same name as the pin name. That’s why the existing power symbols use them. So having the pin names different between the two symbols won’t work. (The PWR_FLAG symbol works on any net because it doesn’t use a hidden pin trying to automatically connect to a net name.)
I’m not sure what you are getting at. KiCad symbol libraries have always had a field called “Symbol Name”. That is how you choose which symbol to use out of a library. And because of this, symbol names within a library must be unique. (And I just checked, the value field and symbol name field are linked together in the symbol editor in v5.1.) My first thought was to have two symbols with different shapes with the same name. My second thought was that wouldn’t work unless they were in separate libraries and I didn’t even want to consider suggesting that. Doubling the number of symbols in a library is bad enough, suggesting two separate libraries with one just a modification of the other is worse logistically.
And again, we get to the point that I’m trying to think of a work flow that works within the existing tool set. Not a program feature wish list item.
Edit: Oops, quoted the wrong paragraph first. Corrected.
Just tried that method again, and it did not seem to work. I don’t have time, at the moment, to work out what I probably did wrong.
There has to be either, PwrFLags, Custom Symbols, or specialized Power Ports that are allowed to act as Power Output. I like idea of the specialized Power Ports because it would eliminate the weird PwrFlags from the schematic and still comply with the ERC.
I am fine with any, and all, suggestions to get rid of the PwrFlag on printed schematics.
Only hidden power input pins are labels! any other hidden pin is just hidden.
See my FAQ article about how to make symbols (section custom power symbols) Tutorial: How to make a symbol (KiCad v5.1.x)
I think you overestimate your knowlede about kicad right now.
Ah. Well, I did claim that I hadn’t experimented with it. That is the detail that kills the idea.
That’s what I get for spouting off before trying something out. I did slightly misspeak my assumption, which was hidden power pins. I just forgot that it was specifically power input pins only.
@Sprig This explains why your experiment didn’t work.
As a new user of KiCad, I must say that the power flag thing is the most incomprehensible part of KiCad! Nothing about it makes any sense. The symbol used doesn’t make sense. None of the discussions nor questions and answers about it make any sense. There are no sensible examples of how to us it. IMHO it should be gotten rid of as it only seem to be some inconvenient hack in order to do something that should be an editable option of any of the already available power parts. Adding these horrible things to you schematic only confuses the reader and clutters multi source circuits. Look at any professional schematic (i.e. from Samsung, Qualcomm etc.) and you will…guess what? Not find any!
Please rid this nuisance or at least put some proper effort in explaining how to use it. Yes, lots of example pictures would be helpful.
Reading through the forums, it is also clear that this is an issue that is both overwhleming and will clearly not go away any time soon.
How is a ‘power part’ defined? On my board I have an RJ-45 connector (symbol from outside of the KiCad library, as well), where power and data connections arrive. Short of editing that connector’s symbol to mark the relevant pins as ‘power output’, PWR_FLAG is the only solution, since this part is not a ‘power part’ by any reasonable definition.
That is a good point, but my point is that you should not have to edit the part in your library to be able to set one or more of it’s pins to be a power source. So in this regard, I suppose there are only 2 solutions, either:
rewrite the part libraries
or make part pins editable so that they can be marked as powersource
Anyway, what do I know. I’m just re-new’ed to KiCad since >5 years.
The concept of a Power Flag on my schematic bothered me at first also; and while I do think some things could be done to improve it, it makes sense once you understand the basics.
The Power Flag allows for ERC checking while using generic Symbols. If you want to remove the Power Flag from the schematic you can create something KiCad users typically call an “Atomic Part”.
Every EDA program has it’s own individual quirks.
Realize that you can become a Developer and make the changes to make KiCad what you want it to be.
One of the main points of confusions might be that a normal symbol is used to communicate this sort of thing. If it would be similar to the no connect flag then i think it might be a lot more intuitive.
Atomic part might not be the correct term here. A fully specified symbol represent exactly one part number and has all its fields filled out accordingly. But it still points to a generic footprint. Only if the assigned footprint is also only meant to represent that same component can the pair be called “atomic”.
Nothing suggested here would require even a fully specified yet alone an atomic asset.
The term you are looking for is a “project specific” symbol. This is a symbol of any type (generic, fully specified or atomic) that is changed to represent special requirements for the current project. (Non standard use of a rj connector, pin setup of an mcu representing how it is configured in software, …)
Each pin should have an option to add attributes. Like symbols now have where you can add custom fields. Then we could standardize a few of the attributes for this purpose. This would enable automating DC power analysis using FEM.
Hopefully the option to add attributes to pins will be added in V6.
