For a through-hole pad one can choose between All copper layers and F.Cu, B.Cu and connected, for the Copper layers option. Are there any disadvantages in choosing F.Cu, B.Cu and connected ?
Background:
In e.g. a 4-layer design where I have a 2.54 mm through-hole pin header, a copper fill does not pass through the pin header when the pin header pads use All copper layers because the pin header pad gets a copper pad on the inner layer which blocks the copper fill. However, choosing F.Cu, B.Cu and connected for the pin header pad, the copper fill now goes nicely through the pin header. To me the last option is the obvious best choice, but for some reason not the one used by the KiCad footprints.
This is exactly the sort of thing why this was added to KiCad.
It also improves signal integrity (for very high speed signals with steep flanks).
This feature was added relatively recently to KiCad (I think in V6), and probably nobody bothered to put it in the default footprints after that. But it’s easy to remove those annular rings in a post-processing step.
I am not aware of any disadvantage of removing these annular rings.
Are there any disadvantages in choosing F.Cu, B.Cu and connected ?
I only know one: My standard board house says the mechanical stability is a little less than normal.
But another point:
There were issues with this setting and the zone fill algorithm under some circumstances, at least in v6. As I don’t use that feature I don’t know if that all got fixed. So look careful at the first zone-fill results (and maybe report back if you find issues).
edit: found at least the corresponding issue #12964, which is marked as fixed for v7.
I have heard (information not checked) that some manufacturers having not very modern technology need these annular rings if the hole is to be plated.
Recently I asked my local manufacturer (but he is probably one of the best in my country - he offers 4/4 mils process) and got the answer that they need not those annular rings.
Thinking that I have to have these annular rings I just changed the vias in QFN exposed pad to have 0.6mm between them. Then I set copper fill clearance to 0.2mm and minimum width to 0.2mm.
Depends on the manufacturing process. When holes are plated, they use some chemical solution to grow a copper layer in these holes. That growth usually starts from existing copper, so having existing copper rings in the hole can improve the quality and thickness of the copper plating.
I would be cautious about removing copper layers from very small vias or from vias that have to transmit a lot of power, especially when using a very cheap manufacturer.
The holes may also be mechanically stronger with the annular rings, but that could only be a (perceived?) advantage in extreme cases such as pins for screw terminal blocks.
But it’s all speculation. Your reference for things like this should always be:
