Hello,
I have a problem with only one of my pin on my project.
As you can see on the picture below, B2 pin isn’t connected to my copper zone while all of the other are connected.
On the above picture, you can see my schematic, they all have the same net name.
I don’t understand why onyl my B2 pin doesn’t connect. I have 4 connectors PCIe like that and for each, B2 pin isn’t connected to the copper zone.
If you have any information on how to correct this problem, I would be more than happy to hear them 
Best regards
Thomas
have a look at the pin properties of b2 compared to b1. Is there a difference?
Also what is the horizontal line through b2/b4 or A2/A4?
(Do you have the same color for silkscreen/copper?)
1 Like
In that screenshot, I see a vertical line running through the right-hand edges of pads B2 and B4. Is that a trace? If so, I suspect PCBNew is interpreting it as a connection between the B4 (“GND”) and B2 pads. That, in turn, makes the B2 pad part of the GND net . . . and PCBNew will not make a connection between a GND pad and the “3_+12V” net.
I see a similar situation on the left side of your screenshot, between the A2 and A4 pads.
Another, less likely, possibility is that the local clearances assigned to the B2 pad have become corrupted.
Dale
1 Like
Hello,
There is no difference between B1 and B2 pin properties.
The vertical line that you can see is the top silkscreen of my connector. I am not sure it’s silkscreen fault otherwise I would have the same problem for A2 pin no ?
Thomas
(Your keyboard fingers are faster than mine. Each of us saw the same thing, but one of us is still laying sideways in bed, so the vertical/horizontal reference is rotated.)
Dale
Did you run drc lately? Sometimes zones only refill properly if drc is run. (DRC does more than just check if everything is ok)
Also try to close kicad and reopen it.
Not laying sideways in bed. I just confuse horizontal and vertical sometimes.
The KiCAD DRC does not check for silkscreen violations at this time. In the short run, it’s nice that the DRC report isn’t cluttered by a bunch of silkscreen squawks, but in the long run I’d like to have the assurance that I haven’t parked a reference designator on top of a SMT pad.
Dale
I haven’t been to a party like that since university days.
Dale
1 Like
I used DRC, but there is no mistake here, only unconnected pin. I tried to close and reopen Kicad but same mistake.
I have no idea ho to correct this problem. I could make a trace between B2 and a connected pin but it would be a lil bit “dirty” no ? ^^
Thomas
What kicad version are you using under what operating system?
Can you share your pcb_new file maybe we can find something that is wrong with it.
I use Windows and I tried it with Kicad 4.0.2 and Kicad 4.0.5
Here is my pcb file
backpanel3.kicad_pcb (2.7 MB)
The puzzling thing is the little nubs from the copper pour near pad B2. They imply that the copper filling algorithm is trying to make a connection to B2, but some clearance rule is preventing it from doing so. Typically this is because the zone properties (spoke width, thermal relief gap, etc) are incompatible with pad sizes and spacings in the footprint. Since the other pads in your footprint have connections to the fill zone, it’s not something in the basic geometry of the footprint - which is why I suggested looking at the properties of pad B2.
At the moment you have me stumped.
Dale
Give that a try. Use a thin trace, and connect it to pad B2 at a 45-degree angle. The fill zone will overlay the trace and you won’t even see the trace.
(If there is no explicit connection to a pad, the fill zone algorithm may not incorporate it into the zone even though it has the correct net name assigned.)
Dale
There is a circle on edge cuts over this pad. Removing this circle solves the problem.
This circle is part of the footprint. Where did you get this footprint from?
There is also a big circle on edge cuts that is missaligned to the pad in the same connector. Is that on purpose?
1 Like
Exact this circle was the problem. My colleague did the footprint of the board with fixing hole using a dxf and when i converted it to edge cut, all of my fixing holes and pin indicators had those circle around them…
Anyway, problem is solved now ^^
Thanks a lot for your help !
Thomas
Explanation: If the pad is partially or completely outside the board perimeter, the zone filling algorithm will create a clearance around the edge cut line.
Normally, the KiCAD footprint editor will not allow you to put anything on the edge cut layer when editing a footprint. Anything on the edge cut layer of a footprint was put there by manual intervention using a text editor. That raises questions about the integrity and accuracy of the footprint (and perhaps others from the same source).
Dale
1 Like
Yes, I just noticed I had same problem with fixing holes. I deleted them and no problem anymore
Thomas
