[oops] - I deleted my previous post because I can see now exactly why those inner pads are large. The blind via spans layers 3-6, so all those layers will have the annular size of the blind via.
Anyway, we’ve known for a few years now that KiCad desperately needs a padstack and editor but so far no one’s had the resources to put into it.
as I posted a footprint module with different size pads is required…
(it is possible also avoiding blind vias)
I wouldn’t put *.Mask on this annular vias
and moreover you’ll get a DRC violation…
so it is a dirty trick 
we will wait for a legacy padstack and editor…
OK, kick out the inter-layer pads and have just a simple footprint for a through hole like this:
(module z_via (layer F.Cu) (tedit 561F5CF9)
(fp_text reference V101 (at 0 0.9) (layer Cmts.User) hide
(effects (font (size 0.2 0.2) (thickness 0.02)))
)
(fp_text value Via (at 0 -0.9) (layer F.SilkS) hide
(effects (font (size 0.3 0.3) (thickness 0.03)))
)
*(pad 1 thru_hole circle (at 0 0) (size 0.7 0.7) (drill 0.4) (layers .Cu))
)
You can now put tracks to this without DRC violations and when you make a buried via with bigger sized annular rings it will work…
So all that would be left to do for some programmer is to put in an option to tell the buried via method to not to create annular rings between the layers the buried via is supposed to connect.
Then you’d be done, as you’ll have at least 2 tracks going to the via at different levels, otherwise you don’t need any bigger sized annular rings anyway, right?
Or do I miss a case here?
Thank you very much for your hints! We will try it out.
I have talked now to the PCB manufacturer and got some news. They told me that we might simplify the things a bit, because they will remove annular rings from vias in inner layers anyway - if there is no track connected to it. They call them “Non Functional Pads”. Thy will do it with their CAM tools on gerber basis.
But even if thy do so, one problem remains: In our gerber files, the surrounding copper area will not be filled near enough to the via in inner layers (because the filling algorithm will see the annular ring there).
Maybe this problem can be solved without a padstack editor. In our case, it would be nice to have an option, removing all annular rings from inner layers, when they are not connected to a track.
I will keep you informed and post our results here.
if you don’t want annular rings on non connected to layer inner pads, you can do like that:
a module with pads only on tracked/connected-to-layer pads
(module ann_via (layer Front) (tedit 561F5CF9) (tstamp 561F9B2E)
(at 126.45898 136.2202)
(fp_text reference AV100 (at 0 0.9) (layer Cmts.User) hide
(effects (font (size 0.2 0.2) (thickness 0.02)))
)
(fp_text value Via (at 0 -0.9) (layer F.SilkS) hide
(effects (font (size 0.3 0.3) (thickness 0.03)))
)
(pad 1 thru_hole circle (at 0 0) (size 0.7 0.7) (drill 0.4) (layers Front)
(net 4 N-000002))
(pad 1 thru_hole circle (at 0 0) (size 0.7 0.7) (drill 0.4) (layers Back)
(net 4 N-000002))
(pad 1 thru_hole circle (at 0 0) (size 0.7 0.7) (drill 0.4) (layers In4.Cu)
(net 4 N-000002))
)
that will produce only annular on tracked pads, but with DRC violations
that will reduce also the filling problem
from the picture you can see that internal fill zone (layer without annular) is closer to drill than the top fill zone where there is the annular
interesting for me that on layers where there are no pads it keeps zones from filling up to the hole. Fascinating.
Well, if it filled the zone all the way, there would be a pad again, a large one. Can’t have that if the hole is plated. Even for unplated holes it would be pushing one’s luck. Can’t guarantee that the inside surface of the hole is 100% free of copper, especially if the drill is a bit dull and starts smearing the stuff all over the place.
The case shown in the image above seems a bit excessive though. I guess it would be sufficient to keep the zone away from the hole by oh say 0.5x drill diameter, maybe less if the drill registration is optimal.
I’m happy about your support in this forum - thanks to you all!
Yesterday we’ve checked the proposal from maui, using pads instead of vias. This would solve our problem. We will see if we can define those pads within the BGA footprint, allowing us to reuse those settings for other projects.
Of course, all of this is a workaround, and a padstack editor would give us a much more elegant solution.
But in our case - we would also be happy with an option for the gerber export dialog like “Remove Non Functional Pads from Inner Layers”. This is something the PCB manufacturer will do anyway. It would be necessary that the released area of the annular ring will be used by the surrounding copper zone (respecting the clearance area around the drill hole). This option would also be useful if the padstack editor is completed one day.
For me it seems that an option like this is no witchcraft. I could ask one of our C++ experts if he is brave enough to try it.If this works we could contribute the code.
But what is you opinion? Would this option be useful for you, too? Would it be a an easy job to implement it? Or do you see any pifalls?
I think that would be a good idea…
please have a look at
https://kicad.org/contribute/developers/
a padstack editor would be a useful thing
you can ask at the developers mailing list if someone has already started something (but I don’t think so) and if there are some constrains to follow…
also the chat is available…
looking for your feedback 
M
I like it. I don’t do 4 or more layer boards yet, but it would be definitely helpful if I ever came across BGAs where every little space one can get for routing underneath is worth it’s space in gold
Any more thoughts about this? I was referred to this topic, having had a related problem wanting special pads on the solder side only of through hole components, especially circular connectors and would find a padstack editor very useful for even two layer boards.
Padstack editor is nice, but it does not solve this problem.
Removing unconnected internal layers annular ring is an optional processing step before tapeout to fab.
Needs to be an option to remove.
But you can normally also ask your pcb manufacturer to remove them in theirs cam station.
The good ones will do that, and even remind you when you forget.
Capacitance is what’s to be reduced.
Not resistance as mentioned earlier.
And thermal load affecting soldering
Hello guys,
just wanted to check is this problem solved. I have been doing 6 layer board and I need my ground plane underneath MCU and RAM not so drill riddled.
you need to select the option to render as technical mode (not realistic mode)
Thanks man! Now its so obvious. 
I did some research and even with 0.4 mm via pad and 0.2 mm via drill i still have the same problem, there is just to much clearance between via annular ring and nearest copper ( I calculated that default setting in KiCad is 0.2 mm clearance ). And there is no way i can route properly without losing my ground plane. 
For my design ( BGA packaging with 0.8 pall pitch ) I need at least 0.1 mm clearance.
You can change the clearance settings in within the design rules.
Ground plane clearance is set within the plane settings itself. (Don’t forget the copper min width.)
