The PCB Editor window is reporting that I have one item unrouted.
If I run DRC, it also reports a Gnd pad as not being routed to the Gnd zone.
The pad that’s highlighted (Gnd pin on a LCD) as not connected is close to 5 other ground pads (2 each on 2 push button switches and an LED), none of which are reported as unrouted, and there is a continuous ground zone between them.
Any idea what problem I’m not seeing here and how to resolve it?
Is that GND zone an island and not connected to the larger GND zone ?
Can’t tell from your screenshot, but note that the message can be a red herring. The message doesn’t say that the problem is near DS1 pin 1, it just says that DS1 pin 1 (and all the other stuff on the same island) isn’t properly connected to some other zone island on B.Cu.
Try to double click on the bottom (Zone [GND]) item, see where it brings you and try to find a path between that and the mentioned pad.
If there a GND fill on the top layer? If yes you probably want to add more vias to create a mostly uninterrupted GND fill.
try to left-click on the ERROR-line (missing connection between items). This should pan the pcb-view to the corresponding error marker, which is normally placed at the smallest distance between the different GND-islands.
All the tracks and zones are on the bottom layer
The circuit is battery powered and the zone that the error indicates is attached to is connected to the battery -ve.
I’ve only found ways to highight the whole of the Gnd fill and I wouldn’t be surprised if there is an island somewhere else, but I can’t see anything obvious or find a way to highlight islands.
You can set the zone fill to not create islands, then you will see a void where the copper cannot be reached.
@retiredfeline I’ve got Remove Islands set to Always, but that only seems to remove them when there’s not enough clearance between pads and traces to connect them. If there are GND pads that can be connected together, but not to a real GND, the zones still seem to get filled (at least with my workflow).
If you have set the net of the fill, and remove islands to true, then if there is a fill there it should be connected to the specified net. You can examine the net of a copper location by looking at the bottom status area.
Without your layout and schematic files and just one limited screenshot it’s hard for us to deduce anything especially as you say there is a real GND, and I suppose some pretender GNDs, whatever that means.
From the files extensions, I think these are the respective files:
Syncheck v2 kicad project.kicad_pcb (328.7 KB)
Syncheck v2 kicad project.kicad_sch (134.8 KB)
(By “real ground”, I just mean a fill zone that is actually connected to 0v of the battery, as opposed to one that’s supposed to be.)
@idris You have an island.
Note the Ratline showing a connection somewhere between the Gnds. is still required.
One other comment about your PCB.
It is considered good design practice to ground all unused inputs of these comparators, so connect pads 1& 2 of U1A to Gnd.
You will have to place U1A on the schematic and connect Gnds to those pins before Kicad will allow the PCB pad connections.
@jmk The area you’ve highlighted is connected to one of the two GND pins on an Arduino Nano, whilst the other is connected to the battery’s GND. (See my green scribbles.)
I had assumed that there would be an internal connection between the pins that would be sufficient.
Thanks for the tip on the 393.
Maybe the internal connection is sufficient. I do not know the internal workings of Arduino. I’d check, if I was you. Sometimes the tracks on those modules are very fine.
Kicad did not know that there is an internal connection between pins 4 & 29. I did not realize there was a connection. Nor did a few others 
If you place a wire between pins 4 & 29, Kicad will know they are connected and you will no longer have a problem.
There probably is, but it’s not a thing I would rely on. It could just as well be that you are supposed to make those GND connections external to the module and not assume an internal connection. In the same vein if an IC datasheet showed two pins to be connected to GND I would do just that.
And you are surprised that KiCad didn’t read it from your brain.
We didn’t reach that stage of integration yet 
I’m using microcontrollers that have 4 GND pins (one at each TQFP side) that are internally connected.
It would be very bad idea to connect GND supply pin to one of them and the (Open Drain) MOSFET Source pin to the other one, specially if this Open Drain output is intended to output several Amps.
Genuine Arduinos will not have a problem with the ground connection - they’re pretty good with having a solid ground plane in their PCB stack up. If you’re using something from a third party that matches their footprint then you should research it as much as possible.
Regardless, I wouldn’t consider it good practice to rely on an internal connection between two pins of a plug in module in any case - especially not for ground. My recommendation would be to have one of the Arduino’s pins connected to ground and the other left floating.
I presume that this is an Arduino Nano with the footprint:
There hasn’t been enough information provided here to really provide a good understanding of the project but I would think that it’s a two sided board and there should be the ability to provide a ground path/extended ground plane on the other side of the board.
Agree.
Disagree. If the Data sheet shows two grounds, then two grounds it shall be.
I should qualify my comment from above.
If there is a nice wide visible copper track connecting pins 4 & 29 on the PCB module (which would basically replace a 0 ohm resistor, it could be used as a jumper. Personally, I wouldn’t, but this is not my project. If pins 4 & 29 go to different areas on the module, then no way should those ground pins be used as a jumper.
The same comments would apply to two or more same value V+ pins on a module.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.
