I’m new to kicad and to making PCBs in general. I’m trying to making a PCB for a project and ran into this error
“Copper belongs to a net with no pads. This is strange. Zone outline (56F5D98E) [GND] on B.Cu.”
My project involves 3 components DC jack, ESP8266 breakout board and a sensor. There wasn’t a component available for the Esp8266 and the sensor so I created them. I was trying to fill both the F.CU and B.CU with the GND net with thermal relief.
PCBnew… right hand toolbar (Visibles).
Uncheck F.Cu and check B.Cu in the ‘Layer’ tab…
For SMDs (you got TH components there) one also switches off the respective Pads/Footprints under the ‘Render’ tab (not needed for your case atm).
Hm, would there be a ‘GND’ net that the copper can connect to?
Also the F.Cu zone did fill and connect to the correct pads of the ESP adapter…
So there must be a netlist.
@guevaral
How did you create the B.Cu filled zone?
Via right click menu on the F.Cu zone and then ‘Duplicate Zone’?
Can you get us a screenshot of the properties of the zone as well please?
Originally I tried manually drawing both the F.Cu and B.Cu when I posted my question. I tried using the “duplicate zone onto layer” option and I am still getting the same error.
Interesting… I can’t remember having the ‘GND’ entry at the bottom of that list… ever.
It’s usually the first after < no net >… can you check the top of that list please and see what you got there?
Now would also be a good time to have a look at your schematic.
You somehow managed to create a GND net without anything connected to it…
Do you have a link for that ESP breakout board?
Is pin8 GND or something else?
Also, your barrel jack connector… do you want the sleeve to carry positive voltage and the pin the ground? (that’s unsafe to do)
See this picture for reference:
Ah… there we go… your GND symbol is not connected to the wire… see the little circle at the end of the ‘pin’?
Move it a bit down, draw a wire to connect it (circle needs to vanish), recreate the netlist, then import the netlist into PCBnew again and you should be good to go.
To ‘test’ for stuff like this (if you’re unsure if a symbol has connection or not) grab it with [G] and move it with the mouse… any wires which are connected will move with it like rubberbands… hit [ESC] to cancel the action and proceed with drawing
Yes, you’re right. I’m still working off a hangover from a different brand of layout tool, where it WAS possible to assign (and re-assign) copper features to a net of your choosing. (In practice it was perilous to do so, except for filled zones. But simply having the capability allowed you to create boards “on the fly” and without schematics or explicit netlists, by pointing to pads, traces, or filled zones and assigning them to a net. When it came to things like DRC, the program treated these ad-hoc nets as if they had been read from the netlist.)
I have been bit by this behavior more than once. It also happens when symbols are drafted using a grid size that’s different from the grid size specified in EESchema.
In all honesty . . . . I’d expect the drafting engine of a world-class tool to detect that there wasn’t a connection, and either make the connection or ask me if I intended to have a connection. Barring that behavior at drafting time, I’d expect to see a squawk at error-check time. I shouldn’t expect a draftsman to go through a completed schematic and check everything that looks like a tee-connection to see if it’s truly connected or not.
