I have installed kicad 8.0.1. But i found something interesting. Every net with no name is shortcircuit together.
For example, you place a battery, one resistor and one led, all path is in short circuit.
For example this is a piece of a schematic that i am creating. I highlight one unnamed net, and a lot of traces becomes pink.
This is looking weird. Also named nets are highlighted (going to the output connector) and also the vertical bus on the left side.
in the case of named and highlighted tracks i do the following. I put the labels before to draw the tracks, because i know where the tracks will pass.
In previous version of kicad, when the track pass for the label the track get the name. But when i move the label one step left and one step right, the track is named and the pink go out.
Another thing that i note some interesting. Y copy and paste 3 times one label, as is expected the 3 tracks become the same. So i edit the name of the copies 2 and 3 ( 1 is the original)… and the track STILL is the same (in short circuit).
The kicad dont recognize the new name until i move the label.
Be a little bit careful with the highlighting command. There is still a bug in Kicad regarding the connectivity/highlighting for new added wires and/or copied/modified labels.
If you want to rely on the highlighting tool: save, close schematic, reopen schematic, use highlighting.
This affects also the new added net inspector panel, which is also not 100% reliable after adding/modifiying wires/labels.
See gitlab issue Net navigator panel is missing sheets after connecting local label to global nets (#16836) · Issues · KiCad / KiCad Source Code / kicad · GitLab and all mentioned sub-issues (16818, 17713, 17891).
The vertical bus line on the left being highlighted also suggest there is a bug in the highlighting tool itself. If you want to check real connectivity, then use: Schematic Editor / Tools / Update PCB from Schematic [F8] and use the ratsnest lines on the PCB.
If i close, and reopen the “short” still there.
The schematic is in very early stage with 120 errors and not annotated. Only appear few components, and very less connections
This seems like a variant of bug Incremental connectivity fails to update subgraph when removing power symbol? (#17984) · Issues · KiCad / KiCad Source Code / kicad · GitLab
One possible workaround (until the bug is fixed) is to disable incremental connectivity. You can do this by creating a kicad_advanced file (if doesn’t already exist) in your config folder (%APPDATA%/kicad/8.0 on Windows, ~/.config/kicad/8.0 on Linux) and adding the line below:
IncrementalConnectivity=0
Can you try that and see if it fixes your issue?
I dont think that the bug is inside of highlight tool, because i can fix moving the label one dot to the right or the left.
I dont know how work the code of kicad, but i imagine that kicad have a “net_rescan()” function and this is not called when i change the label name or if i place a wire over an existing label. The result is that the wire dont recognize their new net association.
a possible workaround can be create a automatic net name the according the first connection. For example: NET_C1_1 ( net connected to pin 1 of C1). This will create a unique ID for default.
I create the file with the content, but the issue still is there
Yes, as I mentioned I think this might be an issue with Incremental Connectivity. You could try disabling it and see if it solves your issue.
There is no hard rule for a 50mil grid. 0.635mm is half of 1.27mm, and thus it’s 25mil, and that should work too.
Some background:
KiCad builds up connectivity from the coordinates of pins and line segments. The coordinates have to match for KiCad to recognize a connection. All of KiCad’s symbols are designed to have the pins on a 2.54mm (100mil) grid. This grid is however not practical to use, because when capacitors and resistors get inserted, they have their pin offsets 150mill from the attachment point of the symbol. Inserting them on a 100mil grid will therefore put the pins off-grid. This makes 50mil the coursed practical grid in KiCad. Finer grids can be used, as long as it is an integer division of 100mil. With finer grids (<10mil) the grid becomes unpractical again.
Yes, my girds are on 0.635. The origin of this schematic was one created on kicad 6 and i need move a lot of components and tracks.
The origin was a single page, and now i s a 6 pages schematic.
I do:
wolf@localhost:~/.config/kicad/8.0> cat kicad_advanced
IncrementalConnectivity=0
wolf@localhost:~/.config/kicad/8.0>
close and reopen the kicad program.
New Update. Seem like was fixed automatically.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
