Hello all, I made a simple project - an adaptor board, with one common bus. I got multiple warnings “Net /XX is graphically connected to bus / but is not a member of that bus”.
Where exactly the problem is? Thank you in advance!
First, Starting with a project as big as this is not a good idea for a beginner. With a complex project, it takes much longer before you discover you’ve made a mistake, and correcting mistakes is also much more work. When you want to get familiar with features that are known to you, it’s much better to start with it on a small scale.
In KiCad V5 and earlier, the thick blue bus line was just a graphical item and had no meaning beyond visual. In later KiCad versions connections to buses has become more strict, and you also have to label the bus itself, and all it’s members. In short, KiCad has “Vector buses” and “Group buses”, and those can be combined too. With a bus like this, you normally put all the bus members in Schematic Editor / File / Schematic Setup / Project / Bus Alias Definitions, and then put the name of the bus itself as a label on the bus. This is all explained in more detail in the manual of the schematic editor. https://docs.kicad.org/8.0/en/eeschema/eeschema.html#electrical-connections
I suggest you start a new project, with a bus of maybe 5 or so members, then read the above linked to chapter of the manual and experiment with it until you understand how it works. Then you can easily fix your bigger project.
Thank you for the info! Indeed I did not touch KiCAD for a very long time and my assumption was that the bus is a just a graphical line, that’s it.
Yes, I will split the buses per logical groups
I’m surprised. I was sure that using buses as only graphics is still acceptable (if you label bus it have to be correct, if you don’t than it works as previously).
I am in V8. I have never labeled buses. I have never noticed any Error/Warning about it.
Is it possible that it is because I start each project from copying a previous one so all my projects have in their history V5 and in some moment in past KiCad took care about it when upgrading old projects?
I am writing from home where I have Win7 so only KiCad V5 being installed here long time ago and not used.
I was surprised too. I did a very brief test, before I wrote my previous post. I connected some wires to a bus without naming the bus and KiCad complained about it. My expectations were also that KiCad would still accept this, but apparently it does not. I have not looked into details. This particular project has 6 instances of the hierarchical sheet this is on,
Yep. It looks like the bus label should contain all bus member labels, with some syntax applied:
I’m fine with it, it should improve the reliability of the project
Traditionally, buses on microcomputer boards are divided into three. An address bus, a databus, and a control bus.
If you start making lists of bus member names:
Then it’s also getting time to look into how the Schematic Editor / File / Schematic Setup / Project / Bus Alias Definitions list works I mentioned earlier. If you want to put it all on one bus as you did before, you can also add the data and address vector buses to the alias list.
In my case, the control bus is separated between two bus connectors with jumpers/inverters between the signals, so I have to keep signals under separate names. This is acceptable to me, except that the bus label becomes too long and unsightly. Is there a way to ‘hide’ it under Schematic Editor / File / Schematic Setup / Project / Bus Alias Definitions ?
yes
And some silly )(*&^%$#@! because this forum software does not accept posts shorter then 20 characters.
1 Like
How stupid I am! 
I had to sit at PC once more to suddenly get my eyes open. It it obvious why I didn’t sow any error regarding buses. I just have never run ERC. Any errors I have ever seen was DRC errors and what I had in mind was that I have never seen there (in DRC) any bus errors 
And buses used old way (no labels at buses) still work correctly so I have never noticed any problem with it.
Yep, I was able to hide that mess from the bus label under the Schematic Editor / File / Schematic Setup / Project / Bus Alias Definitions, now it looks much better:
1 Like