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.
You can see that thermal spokes are generated, but only connected to the via, not to the plane.
Any idea why this is so?
Nope, the pad is also connected with a spoke . . .
change the plane to connect only to PTH with spokes and you should have a 100% connection between the plane and the pad.
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.
Initial question still remains unanswered, why is there only one type of connection? only SMD or only PTH, why not have both?
I would guess it’s caused by too big values (clearance + minimum width + thermal relief gap + thermal spoke width).
Your device and my device (see below) are both surface mount so in this case I don’t use thermal reliefs . . .
I set my thermal vis (TH pads) and thermal pad (SMD pad) to be solid connections from within the footprint properties . . .
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.
as a solid connections affect solderabilty, I am not to keen on using them…
apart from that, good idea
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.
You’re right, but I still do handsoldering a lot.
So for my personal use case it will be relevant.
How are you going to hand solder something with a thermal pad like that ?
Even if you use hot air or a hot plate I still think thermal reliefs are the wrong way to go
those are LEDs and the pad protrudes a few 1/10mm.
Easily done with a decent soldering iron
but aren’t we drifting away from the initial question?
I have read that amateurs solder thermal pads by making one big plated hole under it and soldering it from bottom side.
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.
Yeah, works like a charm 
Oh, sorry…
Your assumption is right, I am using v8.0.3
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.
Playing around with these values, I am able to find a configuration that works for my special case and is still easily manufacturable.
Thanks!
