Wild guess: Are there no other GND pads on the top copper layer? Asked as another question: How does the rest of the board look like?
6.0 does not have the zone connection resolution info. 7.0 looks like this:
But for your issue it’s the “Clearance Overrides and Settings” tab of the Pad Properties that we need to see…
@TucsonDon : the pad-connection looks ok, the pad inherits the zone-connection-style “From parent footprint”. You now have to look at the same “clearance override” page of the footprint-parameter-dialog, if there is something unnormal. Normally there should be a setting that says: inherit pad connection: “use zone settings.”
My assumption regarding your non-connected pad is different:
- THT-pads are normally connected with 45° thermal spokes.
- above and below your unconnected pad nr.8 are horicontal tracks
- so there is possibly no room for 45°-connection the pad, as that would create a clearance-conflict with the existing tracks
- to test my assumption: delete one of the horicontal tracks and refill again
one remark: if you add your project as attachement (complete project-archive, not only the board-file) it is easier for all to spot the problem - we could directly investigate the problem instead of guesswork. Kicad contains so much parameters which all can influence such a behaviour. And it’s hard to write down all possible reasons for the behaviour (first in remember them and than regarding the time to write them down).
The zone is trying to connect with a thermal relief, but there is no room for a thermal relief. If you pull the +5V track above it a bit upward, or the track from Net-(J10-Pad1) a bit downward then there is enough room and KiCad creates the thermal reliefs.
Well… That was easy.
@paulvdh, Thanks for taking a look at it and your help!
@mf_ibfeew, @JeffYoung, @osterchrisi Thanks for your input and assistance!
1 Like
It’s one of those many things you find quickly if you have the project itself and some experience. Without that you get guesswork and endles “try this, try that” conversations on the forum.
Also, You’ve stil got some work to do 
In general, the routing of the PCB is pretty important. It is much more then just making connections. One of the main things of routing (a digital logic PCB) is the GND plane. Do a bit of research about GND planes, why they are important and how to make them properly.
I will, thanks for the input
Read articles I have mentioned some time ago:
And…
Don’t you (all) think that KiCad should be clever enough to make in this situation horizontal thermal spoke?
1 Like
Don’t you (all) think that KiCad should be clever enough to make in this situation horizontal thermal spoke?
my opinion: No (only gut feeling). I fear inconsistency and an increased zone-filling-calculation time (zone filling is currently already a time-consuming step on my typical boards).
I admit that this could be a good feature, but that must be implemented as a “test/prototype” version and I fear (it’s fearing day): if something is implemented it will be not withdrawn if it doesn’t works as expected.
1 Like
Now add a ground plane on your bottom layer as well. Then add stitching vias to really tighten up the ground system. When you add a ground stitch via in those areas on top where there is no plane – boom, you have top plane…
Maybe fatten up those traces. They look pretty weeny going into those big thuhole pads and solder heating can sometimes cause a crack… Or give them a fattening transition with two trace sizes:
Don’t throw in too much at once. A single good groundplane is preferable to a stitched together quilt. And concering that crack prevention, KiCad V7 (Expected soon) is going to get built in support for teardrops.
Yeah teardrops will be nice.
1 Like
@teletypeguy the traces were @ the default width(2mm), do I need to change the default width?
In my design I am using a 120VAC power supply and the ground plane is tied to the earth ground, is this acceptable?
To all-thanks for the great information and input!
Gotta stop you right there if you are putting 115VAC on the pcb. Just don’t. That is dangerous. I have been designing and building electronics since the 70s, and I have fully rewired a house (with permits and helpful inspectors). I have a healthy respect for high voltage but have never, nor will I ever, put 115 on a board. The highest voltage I ever put on a board was a dc converter that put out 400VDC to power a geiger counter tube that I sent up in a few high-altitude balloons, and that needed oodles of insulation (for vacuum leakage as well as safety).
Use an external power supply (wall wart or brick) that puts out an isolated DC. You can get lots of power from 5, 12, even 48vdc blocks.
Size the traces to suit the application. 0.2mm is a great size for many digital or analog signals. Fatter for power traces where you want a lower drop. Fatter where they enter a connector pad so the abrupt heat of soldering the pin does not cause cracking (thermal expansion and all that).
1 Like
@teletypeguy I would agree with you that it is dangerous if not done right. In my case I have the circuit fused and the source is on a GFCI. I know of several applications that have line voltage on the board, but I appreciate your thoughts and input.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.