I am a new bee to PCB designing. While reading articles I have found people talking about "covering even number of layers with blind via". I have talked to a local PCB manufacturer and they said the same thing and they said they can't do via like 1-2 and 2-3, but they can do 1-3 and 4-6 (Assuming 6 layers board). For it seems that if I connect an internal plane to an external layer (Say 1-2), then I can't connect the internal plane (2) to any other layer. Is it the case? I am really confused with this. Can someone explain in detail with possibly a picture?
Normal vias go through the whole stack. Once the board stack has been fabricated, a hole is drilled through all layers, and plated up. This is the usual and cheapest option. Making buried vias increases the number of manufacturing stages, so increases the cost and manufacturing time.
Which combination of layers can be served by buried or blind vias depends on exactly how the board is built.
In a 6-layer board made from 3 cores, any core can be drilled and plated after etching and before assembly. This means you can have 1-2, 3-4 and 5-6 vias. You can also drill after partial assembly, so a 1-4 buried via is possible. However, if you have one of those, it's not possible to have a 3-6, as that would result in an impossible build sequence.
If your 6 layer board is built from 2 cores, with 2 outer foils on pre-preg, then you can have 2-3 and 4-5 buried vias.
With the latter construction, you can have micro-vias, which are laser drilled 1-2 or 5-6 through the pre-preg. These, as the name suggests, are much smaller than conventionally drilled vias, and are often used for routing away from dense BGA footprints.
Buried vias would only tend to be used on advanced boards, which are pushed for space or isolation. If you're new to PCB design, then it would be good to start on a few less demanding boards first.