Hi!
I’ve a problem with my PCB layout. DRC is complaining about board outlines but I can’t figure out the reason.
Zooming, deleting all the circuit borders and tracing it again, retracing all the junction points DRC suggest me was not helpful.
I can share the whole project if you want, because it’s making me crazy 
Assuming the yellow lines on your screenshot are the edge-cut layer, it looks like there are 3 lines meeting at that point (one thick line going up, one thick line going to the right behind the gray line, and the selected thin one going to the bottom right). That’s obviously not a valid polygon as usually only 2 lines should meet at a point.
1 Like
Thank you Jonathan_Haas for the reply.
You’re right, not enaught information about the PCB. Try to post more pictures…
The whole PCB
1 Like
I think the problem is that the connector (Jamma) has already an outline, because if I delete the whole Edge.Cuts outline, the yellow outline of the Jamma connector stay there.
I noticed also that the outline of the Jamma is thicker than the default Edge.Cuts line.
Yes, if the edge connector includes an edge cut, you must not duplicate it. Just connect your lines to the edge cut lines of the connector.
If you don’t like the edge cuts of that connector, you should probably either remove the edge cuts from the footprint, or change them inside the footprint.
The different thickness probably doesn’t matter, but again you could change the thickness of your lines, or change the thickness or the lines in the footprint.
Yes, that was what I’ve think also, just said:“Try not to trace the outline on the connector outline”.
Run the DRC, same problem but in a different place of the connector like in the picture
If you post your .kicad_pcb file I will have a look.
Of course, thanks!
I solve the issue only by deleting the edge.cuts layer of the JAMMA connector, refreshing the footprint with the new one and then drowing the outline of the whole PCB again.
So, there’s a problem with the JAMMA connector footprint I think. It will be interesting to understand what was the problem.
Here’s the file:
I had a quick look at your PCB.
Both JAMMA1 and JAMMA2 connectors have graphics on the Edge.Cuts layer, and on top of that you have also drawn a third outline around the PCB.
Here I moved the connectors, all the yellow lines are on Edge.Cuts.
The lines on Edge.Cuts must form a single closed outline, that means that the endpoint of a line segment must fit perfectly with the startpoint of the next line segment, and in each corner only 2 line segments meet. You can not draw lines over each other.
If I just delete the two JAMMA connectors, the board renders fine in the 3D viewer:
And this means that the outline as you have drawn for the PCB is OK. There is no need to redraw those.
Then there is a small difference between the endpoints of the lines of the JAMMA connectors and the rest of the PCB outline. There is a difference of 30um between the endpoints:
It is possible to use the “Edge.Cuts” layer in a connector (but a bit finicky to get there). If you do this, then it still stands that the PCB must be a single closed outline. This means you can not put two of such connectors on top of each other. It is also unusual to use two footprints for a single connector. The normal way is to draw pads on both the top and the bottom in a single connector footprint. If you have graphics on Edge.Cuts in a footprint, then you must connect the rest of the Edge.Cuts lines to the open endpoints of the Edge.Cuts graphics of the connector, and not draw another outline over it.
2 Likes
Can’t be more accurate! Thank you so much for the input!
Yes, it’s strange to use two footprints for a single connector, I don’t know why the guy who have draw it made it like that.
I modified the footprint of the two JAMMA in the footprint editor, removing the outline and redrawing it manually.
This looks like a typical hobby level project, and such projects are often made by people who do not have much experience with KiCad (or PCB design in general) and this leads to mistakes like this.
2 Likes
Of course it is, this is my first project in Kicad. 
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.