Hi guys
I have another question related to edge of a board and castellations. I have a board with a cutout and a castellations on the edge. The problem is that I have a internal copper GND layer that needs to reach the castellations but it does not because the copper pour on that layer is not offset from the edge as seen below. Is there a way I can make sure that the copper is pouring over to the edge of a board at this place?
It’s not clear what has made the pour pull-back just in that area - do you have some not-shown entity ?
If you want copper to the board edge, usually holes + routed edge is enough, so you could just extend more GND pins into those areas?
You could also make those oval fingers to give more copper/no acute copper angles.
Which one is the copper pour that doesn’t reach the castellations? The yellow or red one?
The red + purple areas block sight of the yellow one, so hard to say where it ends.
Can you switch off the layers that are not involved and take another shot?
Maybe also the settings for the yellow copper fill (might compare it yourself with the settings of the red one right away)?
Shouldn’t the nets be the same then (GND)?
Your via for pin #1 of U7 doesn’t connect to the yellow copper fill either…
Hi, thanks for fast reply
The yellow copper pour does not reach the castellations.
I removed the top components and their silkscreen from the screenshots. The first one shows only GND copper pour on inner layer and the second one shoes the top (red) layer also with the GND copper pour around/beneath the chip also.
Edge of a board is marked with the red arrow. The pull-back on GND layer is caused by the edge of a board which is fine for the rest of a board but I’d like to avoid it just here, I want it to extend to the edge of a board just on this part of edge.
P.S. I think via for U7 pin #1 is connected to GND layer
I was just playing around and realized that i can fill it with traces like below. Is there more “elegant” solution?
I can reduce the clearance in the copper pour setting to 0 and then the copper pour fills in to the board edge. Should I do that?
Instead of traces place another zone there and reduce it’s clearance to zero, then it doesn’t affect the rest of the board.
Thanks Gigawatts for input.
I’ve tried this before but the only thing I managed to get is to two copper pours to join with the settings of a larger one.
Then I fiddled for an hour or two again with the same idea and I managed to get it right but I am not sure that I could repeat the steps. I have deleted copper pours several times and redrawn it again and again and finally it seems to me that it worked. I’m not touching this layer again ever. 
Hi,
Do as Gigawatts says but give the zones different Priority level.
Regards,
Pedro.
Also discuss this with your board maker, normally copper does not go right to the edge of the board
I wouldn’t have made the new zone any wider than the castellations. Might be easier to simply run short lengths of wide traces from each castellation pad to the ground plane. That might also provide some thermal relief.
Thanks for advice it is greatly appreciated.
I plotted the gerbers and checked them in gerbv program so I as ran out of time I already send it off to fab. Reason for making the smaller copper fill so wide was that it would merge with the bigger pour if it was not pouring over one pad connected to GND layer or it seemed so to me at least. Gotta stop doing this on late afternoons. I’ll redo the layers most probably on the second run so I’ll try it then. I have this thread to go back to now when the time comes.
Already did, they are doing castellations without problem. The only thing they complained on this board is that the castellations have 0.5 mm holes instead of 0.6 as their req so I made them bigger and it passed the review. Hope it’s not coming back in a later point.
