Hi, I’m making a PCB using a .bmp file as canvas for my design included in the Eco1 User. With this method manual routing and No DRC are used.The PCB type is using very large zones of copper and to avoid to place many tracks one after the other I would like to use filled zones but I don’t know how to get copper for this areas ? Any are welcome. Thanks. Vincent.
You need a net that ‘contacts’ the zone for the copper fill to work… without a net, the copper pour won’t pour.
For the net anything like a piece of track or a pin of a device works. The nets must be the same for the pour and the pin/track.
Hello thanks for the answer, unfortunately I’m not working from Schematic / Netlist, this is more a “brutal” approach of the PCB design, anyway if I create a “Dummy” net that could be work, I’ll try that and let you know.
Thanks again.
Vincent.
That will work, been there, done that 
I can’t find a solution on my problem, I try to put a sample file (TRY.kicad_pcb and TRY.pro) but I can find a solution ? How to joint files to this topic ?
Thanks
If you mean attach/upload… in the little window, when you reply, there are buttons at the top of it… one is the upload button. If you did read enough and been around for some days it will allow you to upload something.
Otherwise use one of the file hosters, some are free until that works here…?
Hello Joan, you’re right I’m not able to upload at this time, too young on the forum or what ever, I use this link to upload it : http://www.filedropper.com/try_2 then you need to create an empty Try.pro to start my example, thanks for your help !
Vincent.
Btw, the outline was broken, I fixed it.
I already manipulated the kicad_mod file to have a GND net.
TRY.kicad_pcb (21.8 KB)
…
(net 0 “”)
(net 1 GND)
(net_class Default “Ceci est la Netclass par défaut”
(clearance 0.2)
(trace_width 0.25)
(via_dia 3)
(via_drill 1.5)
(uvia_dia 0.3)
(uvia_drill 0.1)
(add_net GND)
)
…
The (add_net GND) entry for the via section will vanish without footprints… that’s why there is one in there.
You need to 'convert//replace those vias with footprints of through hole pads.
Pcbnew seems to want to have some footprints on the pcb to ‘hang’ those nets onto for the ratsnest… without that there will be no filling.
You will need 1 footprint per zone, as otherwise you need to run tracks from zone to zone (for the ratsnest).
Best is to replace all vias and save the pcb.
Once you got that, save the pcb and open the kicad_mod file in a text editor and replace anything like (net 0) with (net 1)… that’s for the tracks to be on GND now (you find them in the file as (segment…).
And then you need to set the pads of all footprints from this:
(pad 1 thru_hole rect (at ? ?) (size ? ?) (drill ?) (layers *.Cu *.Mask))
to this:
(pad 1 thru_hole rect (at 0 0) (size 2 2) (drill 1) (layers *.Cu *.Mask)
(net 1 GND))
One zone works - have fun!
<img src="//kicad-info.s3-us-west-2.amazonaws.com/original/2X/a/adef19309ef587f107f95a80fa35029f3620e460.jpg" width=“690” height="499>
1 Like
Many thanks for your support, sorry for the mistake on Outline. Not sure to understand from a first read, I’ll try tomorrow and let you know. Thanks again !
Vincent.