Anyone ever tried blind vias in kicad,
If so how does one use them in kicad.
Thanks,
Wylie
They are mildly awkward to use, but here is how:
First make sure blind/buried vias are enabled in the design rules and that you are using a GAL renderer (either OpenGL or Cairo).
Then set your active layer selections/layer pair for the layers you want the via to go between (the button to do this is directly to the right of the layers dropdown in the top toolbar).
Lastly while routing you can either use the hotkey shift+alt+v or right click and select the “place blind/buried via”. Voila! The via will be partially colored with the color of the two layers it goes between.
When you plot your gerbers you will get a file for every blind via layer combination (so if you had vias going from F.Cu to In1.Cu and B.Cu to In1.Cu you will get separate files for each of those).
3 Likes
I just want to chime in and say that I was somewhat surprised that they worked so smoothly in KiCad. I honestly expected a more fringe feature like that to be pretty buggy, but I’ve used blind vias for my last couple of prototype PCBs (due to BGAs) without any major issues.
The only thing that has been an issue is using micro-vias in pads, but I worked around that limitation by just not doing it. 
One thing to be careful of is that flipping internal layers (and associated micro-vias) is broken in <= 4.0.1. A patch was submitted a week or two back, so hopefully that’ll get included in a release soon. So make sure that you’re either using a current nightly build, or that you get the top/bottom side placement of your components right the first time!