I made a footprint which has vias in an SMD pad. In this specific application, the pad gets connected to ground on top and bottom planes.
On the top plane the vias are not connected to the ground plane as they are on the bottom plane.
Yes, I have seen that the SMD pad is connected, but all the connections to the vias are missing.
I misformulated my question, what I was curious to know is why there are no connections to both
Changing the plane options removes the SMD-pad connections and the PTH connections are not complete / very small.
not sure…
I’d rather guess its a problem calculating the intersections of the adjacent thermal relief spokes. The outer ones that don’t have a neighbour are fine.
Vias in thermal pad function is to transfer heat from pad to GND zone working as radiator.
Using thermal relief connection ruins this functionality.
Thermal relief are good for hand soldered THT elements as soldering them you heat only one place - this pad and the heat escapes to the cold rest of the PCB. But I think (I’m not a technologist) they have little influence on reflow soldering when the whole PCB is heated at once and heat have no way to escape. I don’t know how with thermal pad that is under the IC case but I have never used thermal relief connection for vias in thermal pad and it was never questioned by contract manufacturers.
OK, I understand your use case now . . . it is a little specific to your particular need though so I think you are going to have to try and fit it to your specific use case. I think @mf_ibfeew has the right answer, try adjusting the clearances and spoke widths till you find what you like the look of.
I’d rather guess its a problem calculating the intersections of the adjacent thermal relief spokes.
The outer ones that don’t have a neighbour are fine.
The drawn outer spokes was the reason for my guess. Do you have really checked if a change in the mentioned values shows some influence? How much do you have reduced the values? Reduce all 4 values as much as possible.
Different solution you could try: select only the via/THT-pads, enable properties panel in pcb editor, change “Thermal relief spoke angle” to 90°
sidenote: you should inform the readers of your post about the used kicad version. Some/many answers depend on the version of the used software. My answers were given with kicad v8 in mind.
For hand soldering a QFN, one method is to make a quite big hole in the center under the QFN, and then poke your soldering iron though it from the bottom to heat the QFN directly. I have not used this myself (yet) but from what I’ve seen on youtube it looks quite reasonable / usable. Of course you need to apply paste to the pads first, and an iron with a big tip to get enough heat transfer. Also, paste placement is not very critical, as you can wiggle the QFN a bit during soldering. You’re already looking at the thing (maybe though a microscope). But I guess it does need some practice and experience to do this efficiently.
Changing/reducing these values does change a lot and reveals what the actual problem (imo) is.
The vias are too close together, so the relief spokes touch each other and the underlying logic thinks:
Nice! Found some copper of the same net, can stop.