Why am I not getting zone in the remaining area? Do I have the related concept lacking?
In Kicad zones are only filled if they are connected.
1 Like
I didn’t really get it. Should I leave it as it is? Is the remaining portion not supposed to be grounded?
I made another zone within the black area. Is that recommended?
The problem with your zone is that there is no way to connect the inner part to the outside on the same layer with your clearance and minimum width settings.
To connect it to the inside you will need to move some of your traces to the other layer. Or you could change your connector and have for example pin 7 as ground.
You could also read the topic i posted. There an alternative is proposed where there is non connected copper pour.
2 Likes
That seems hectic 
Couldn’t understand neither in that topic nor this line.
As you might have guessed already. I’m not an english native speaker. (And it seams i’m not yet fully awake.)
By the way got it. ‘Got the no net’ thing. Thank you.
but the no net thing made it insulated layer. What does that imply?
Ok now a bit slower: (After my second coffee.)
Starting with your design as is. At the moment there is no copper pour in this large space in the middle because there is no way to get an electrical connection to anything in this space.
(A zone is limited to one layer.)
If you want ground in this space, you need to create a path where the zone can create a connection.
There are a few options on how to achieve that:
- Option 1: move some of the traces that are currently in the way to the other layer.
- Option 2: play with the clearance and minimum with settings of the copper zone. (But remember: This settings depend on your manufacturing capabilities.)
- Option 3: Change the circuitry. Example: make pin 7 of your connector the ground pin. (This option is only available if you can define the connector as you wish and are not constraint from the outside.)
If you only want copper in there, because you want to save etching fluid. (or some other reason)
You can create a separate zone in this area with no net selected. This will fill this area with copper, but will not connect it to anything.
1 Like
okay. Thanks for such detailed solutions. Option 3 isn’t possible because the circuitry can’t be changed by me.
Luckily I don’t have GND here so its alright to just have copper here, all over and no net works here.
Well for next time…can something be kept in mind as precautionary guideline before making pcb layout so that such a case doesn’t arise i.e., such case where problems arise of zone filling.
OK, but please understand that a floating island of copper does not give shielding and may make EMC emissions worse
1 Like
So what could be done here then?
Connect GND to pin 14 of that connector and bring it over from where ever that is…
So then 'no net ’ option while zone filling won’t work, i guess?
You then have to connect pin 14 in the schematic to a GND symbol naturally.
Export/import the netlist and you can fill all that stuff with GND.
If emc is of any concern in this project, i fear the board needs to be redone completely.
Many resistors are placed in a less than ideal way.
This are only the worst examples. Some of the others are not placed in an ideal way either.
What would you mean by using it in an ideal way?
Smallest possible area between signal and signal return path.
No unnecessary loops.
1 Like
this is the result of using ‘no net’ .
Even if physically i connect GND to pin 14 …how to make it GND plane from here on, which will take care of EMC. if i do it using using pin 14 as net then I will again reach back to the position from where i started this thread. Do you suggest something else?
I connected pin 14 to GND and imported the updated netlist to pcb new .
Notable messages.
1. Changing component “P1:/589ACEB8” pin “14” net name from “Net-(P1-Pad14)” to “GND”.
2. Warning: Copper zone (net name ‘’): net has no pads connected.
Warning: Copper zone (net name ‘’): net has no pads connected.
What next to make it a GND plane to avoid emc emmisions etc