I have this in my design
but the bus’s nets are not connected together even though they are all in the bus alias definition
but the bus’s nets are not connected together even though they are all in the bus alias definition
How does the bus alias look like?
You may need an extra label and connect it to the blue bus, since your bus enters just 1 sheet. Im gonna test this theory out
I tried giving it a label {BMC_VDOMAIN_SOC_JTAG} as well as simply BMC_VDOMAIN_SOC_JTAG but it did not fix it
I cannot duplicate it. I made a simple bus with shorter names, one side goes in the sheet, and the other side has wire entries just like in your schematic. But this connects just fine. So from the looks of it you don’t seem to have made an obvious mistake. I could not find typos or missing {}
At this point I would try to use shorter names? For all I know there might some kind of character limit related bug?
I tried longer names than you, but it still works on my end 
I forgot to say something. For me it tells nothing but it can tell alot to others:
Please post your kicad version, it may be a new bug or an old bug?
I’m on version 8.0.2
I unfortunately cannot tell you. I am still sitting on V7.
Have you tried redoing all relevant labels, lines and bus? Try to use the unfold bus option (default hotkey c) to prevent accidental typos. (I once managed to get a bug in some software because of an invisible character)
Doesn’t the ERC reveal any clues?
I’ve never actually used ERC in schematics before, only in PCBs, so I ran it and it did
but this looks a bit weird since it says that labels are not connected to anything, yet when I jump to pcb editor pads on the IC that they are attached to are labeled
I notice something
This sheet hierarchial label is not dark blue like the others. But I can’t tell why. I triple checked the spelling like 5 times now 
.
It does indicate there is some issue with the bus label inside the sheet or the connection between the sheet in the label and on the label.
Can you delete the hierarchial label which you can see on the sheet, and re-import it?
This one contains typo
This one does not
Also, if I only ruin the alias and run DRC I get also warning and errors. Obvious. It is worth noting that the the label itself (which no longer has an alias) remains deep blue.
So my conclusion is that your label which is not blue, is not recognized as a bus label.
If I change the label name on the sheet, it loses it’s connection with the label in the sheet, but it still remains dark blue. Even typing spaces before or after does not change anything.
Honestly, I think we are looking at an actual bug.
What also does not help your schematic is that the ERC is telling you have 368 errors next to your 261 warnings. What the heck 'd you do? 
I deleted and reimported it but although color was changed to dark blue, it didn’t fix the issue
I tried again addaing a label but then after exiting pcb editor label’s color again changed from dark blue to cyan
I don’t trust coloring of those labels since I noticed these inpredictable changes throughout the entire schematic design process up to this point
I’m in the process of switching from flat to hierachical schematic model, but I still haven’t finished the schematic yet, so propably just a lot of missing connections
I do have Kicad 8 installed on this machine, but I haven’t use it yet. can you upload a zip file of your project? See if I can duplicate it
Unfortunately can’t directly upload it here because my account is too new
Also don’t mind the annotations for component’s with multiple symbol parts on different pages. I’ll manually fix it as the last step since auto annotation breaks them anyway
I was toying around. I moved the labels left and right a bit and I redid the alias. And that seems to have done the trick. I double clicked the label with BMB_VDDMAIN_SOC_JTAG. Copied it to clipboard and pasted it back into the alias. I could not really check the board, because it was missing from the zip.
All arrows dissapeared. I had the same ones like you when I ran ERC at first. But after my toying around… gone
I do see green and blue bus labels. The randomness of those colors…it seems total buggy to me.
I added the zip file, but it was somewhat huge with step files and back up things and things in sub folders, so those I deleted in order to be able to post it. You could replace the kicad schematic files
Constructor.zip (2.2 MB)
1 Like
In the thread below I created posted and posted an example with a bus. It also has a truck and music. It uses two instances of a hierarchical sub sheet, and the bus is routed to different parts on the sub sheets through the hierarchy.
I had the same problem with other busses, moved it left and right, but that still wouldn’t fix the issue. So i decided to do the last step you did and recreate the bus definition alias, but as I was about to do so and selected the name to copy and noticed that selection was a bit wider than the text. I have now realised I had a space at the end of alias name 
. So yeah, lesson learned to check for space, because it might not matter in the schematic, but it definately does in the definition. Now that I deleted that space everything works as expected.
1 Like
I am glad you found it 
. My next advice would have been to smack your computer. That always worked with old TV’s… so it is only logical to keep doing it 
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.