Confusion around blind/buried vias

I am trying to use the blind/buried vias hotkey. I am working on a 2 layer board. I have enabled blind/buried vias in the design rules, but when I use the hotkey I get the warning:

“Only through vias are allowed on 2 layer boards”. I thought a buried via was just a via with solder mask on top of it? What’s strange is I can manually right click a via and change it to blind/buried, but I can’t just place these vias.

No, it’s a via between inner layers. Vias have automatically mask on them unless it’s removed explicitely. On the other hand if you want extra mask coating for vias on top of the basic one you have to negotiate with the manufacturer.

1 Like

I ordered a board from oshpark and all of the default vias are exposed. Is this normal? I was hoping they would be covered by solder mask to prevent soldering mishaps.

Neither blind, nor buried via’s are even possible on a 2 layer PCB.

A blind via is a via that starts on one of the outer layers, and ends on one of the inner layers, so it is completely invisible on the other side of the PCB (Even before a solder mask is applied)

A buried via is “buried” inside the PCB. For example it is made between layer 2 and 3 on a 4 layer board, and is made before the Top and Bottom layers are even “glued” to the inner layers.

Both of these processes add a significant cost to the PCB.

What you describe is a “tented via”. In KiCad this is a setting found in:
Kicad / File / Plot / (Plot Format: Gerber) / General Options / [ ] Do Not Tent via’s

This option is (I think) Off by default (I hate negative check boxes) So I guess that when it is off, the via’s should be tented.

Applying solder mask over the holes is a very simple and cheap (as in free) process, but it is far from perfect. Usually there is not enough material from the solder mask available to fill the hole in the via.
In some cases this may even lead to problems during production. If gas is trapped in the hole of a via if it is tented on both sides, then this may “explode” during soldering.
For this reason, the via holes are sometimes filled with some material, but this is also an extra production step, and is usually not used for “normal” / “simple” PCB’s.

Browse a bit around to learn more about PCB production processes. Eurocircuits has made a bunch of good video’s on Youtube about PCB manufacturing, there are lots of websites which describe different parts of PCB manufacturing, etc.

It seems to be common that manufacturers modify the gerber files, and for some strange reason a lot of people even prefer manufacturers to (silently) correct the mistakes they made. I am more of an opinion that I want my boards manufactured according to the Gerbers I sent to the PCB factory. Everything taken together, Ordering PCB’s is a bit ambiguous.

If you still have questions about your board, then:

  1. Have a good look at the settings on the website of your PCB manufacturer.
  2. Tell us which PCB manufacturer you use.
  3. Post a (macro) picture of what your via’s actually look like.
  4. Check your own gerber files for holes in the solder mask at via locations.
1 Like

No, but I suppose they did it in accordance with gerber files they got.
It is good practice to inspect the gerber files before sending them.

Yes, it gives a headache sometimes :slight_smile:
But, as I use Plot to get Gerbers and to get SVGs and KiCad (5.1.7) don’t remembers my both settings I prefer that at least for Gerbers I can just remember that I can have all checkboxes off and need not to think how to set them. If my PCB is not symmetric I locate it in the first quadrant of the coordinate system and use auxiliary origin = absolute origin. If it is symmetric I have only that auxiliary origin check box checked.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.