Greetings - Back when I started this board, I made a copy (named C_0805) of the standard capacitor symbol and put it in my project component directory. I then added some property fields that I wanted uniformly named throughout the project. When I run the DRC, I get a warning “symbol C_0805 has been modified in library AL200_Symbols” followed by the device’s reference designator. There are TWO warnings for each symbol, one pointing to the body of the symbol and one pointing to one of the pins.
As an experiment, I deleted several of those and replaced them with the original capacitor symbol. This now produces a warning: “Library symbol issue” and (deleted symbol) where the reference designator is, in the previous warning. There are still TWO warnings, of the same class, one pointing to the body of the symbol and one pointing to one of the pins.
There are lots of capacitors behaving this way! As one of those designers who strives for zero warnings, I would really appreciate some help. Does anyone have any idea what is going on and what to do about it?
Before going deeper into this, please upgrade to 6.0.11 (if you want to stay with V6).There were lots of issues with the early releases of 6.0, but 6.0.11 is well-behaved.
This is getting stranger and stranger. Updated to V6.0.11. Now getting modified symbol warnings for ground and power symbols in the power library (which I have never touched). All power supply and ground symbols seem to have this warning. The specific warnings are:
Warning: Symbol ‘+3V3’ has been modified in library ‘power’. Symbol #PWR0123 [+3V3]
Warning: Symbol ‘GND’ has been modified in library ‘power’. Symbol #PWR0124 [GND]
The warnings related to deleted symbols are gone. The original warnings about a change to my version of the C symbol are still present (two per symbol). And I am now getting warnings about changes to symbols I have created in my own project library.
Of course, I can suppress those warnings and just go on with life, but if it is possible to deal with them, I would like to do that. Many thanks!
Hehe… been there. It’s a pain.
The last two warnings are easy to deal with. Open the symbols’ properties and select “Update from library”.
Is your project called “AL200”? If so, there’s another personal library in play.
On themselves there is no error in your schematic symbols being different from the Library symbols. Having a warning for this, is only useful for a part of the KiCad users, for example when using the (new) Database Library system, so it can be ensured that all used parts comply with the way they are specified in the database. Just imagine what what a mess it would be if on the schematic the value of a resistor is (accidentally) changed to for example 10k, while the attached order number in the database points to a 2k2 resistor. For such reasons, KiCad has to have an ability to flag the discrepancies.
For users who like a simpler workflow, you can either disable the warning, or make sure the library symbols are the same as the symbols on the schematic. One way to do this is:
Schematic Editor / File / Export / Symbols to New Library
Make it (very likely) a project specific library.
When KiCad prompts you with: Update symbols in schematic to refer to new library? answer with [Yes]
(This works in KiCad V7. I am not completely sure if this works in KiCad V6).
After that, all symbols on the schematic match with the library you just exported. If you want to modify a schematic symbol after that (but not all instances), the best workflow is probably to first make a copy of the library symbol with the Symbol Editor and give that copy a new name, and then put that new symbol on your schematic.
At the very least, you can do the same in KiCad V6. At most it will be a bit more work but I guess the difference is minimal. Can you verify how this works in KiCad V6? Or else, I’m confident that j_wagner can compensate for small differences.
Well, the first thing I probably need to do is just update the symbols. As I think about it, those warnings must be telling me that there is some difference between the library and the schematic symbols. Will report.
Report:
I selected ONE power symbol and chose Tools>Update Symbol from Library … Chose “Update selected symbol”.
Reran ERC checker (yes, you are correct). Same error on power symbol as earlier. When done on a symbol in my library, the error on that symbol goes away.
Looks like I can finds some resolution, hacking through things. Thanks for the ideas!
While this is annoying, I recognize, as a sometimes programmer, that this is really complex software and I commend the dev group for what they have been able to do.
Indeed, that is all.
It is good form to keep your libraries and schematic symbols in sync with each other but you don’t strictly have to do that. I see you already have a custom AL200_Symbols library. It’s up to you whether you sync the lib with the schematic or the schematic with the lib.
Yep.
The libraries have been updated, though not by you.
The upside is, that it’s only warnings. The big leap from 5.1 to 6.0 was that the involved symbols are now stored in the project.
