[SOLVED] Blind Via and Burried Via usage cost.

Hi,
My question is: Does the pcb manufacturer charge me when using blind /buried vias in a multilayer pcb or no compared to only using through hole vias.
Thank's

In general, yes. Any additional process step adds a cost, but based on my experience, the primary cost driver is the number of lamination steps. If you can keep your PCB to a single lamination step, that would be ideal cost wise. If you have to use buried vias, it would be best if those buried vias occur across a single core since those can be drilled and plated prior to any lamination step. A multicore buried-via will require an intermediate lamination step before the drill. Some blind vias can be accomplished using controlled depth drilling after the complete lamination assuming the layer spacing is adequate, so a controlled depth blind via may not add much cost.

If you can design your board to use only traditional vias, with no blind or buried vias, that would be the lowest cost route. Depending on the complexity of your board, you may not have a choice however.

Are we talking traditional drilled vias or HDI vias (laser drilled)....
As Toohec as stated lamination processes add cost (the intermediate plating processes add the main cost).
If you go to HDI though it can be as cheap or cheaper than a traditional mechanical drilled board depending on hole count, drill stack height etc. as well as achieving a better yield rate.
If I require blind or buried vias I will use HDI technology, I wont use mechanical drilled vias except for the inner cores (Ref: IPC-2226).
Using blind and buried vias takes some thought and is best done by an experienced designer, I have had to re-do boards in the past where blind and buried vias have been used with NO thought of subsequent PCB manufacture.
So think and plan out your design first there are many pitfalls (as well as advantages) of blind and buried vias.

We are talking about traditional drilled vias down to 0.3 mm, no HDI here.

I would try and avoid them if possible. If not plan your layer stack very carefully.

Thank's marce and toohec.

Could you post a screenshot of the board in question? If the board layout is done properly there is usually no reason to use blind or buried vias, unless you're going to extreme high density designs.

The layout is not done yet, it's just a brainstorming before the layout because it's my first multilayers pcb. I'm collecting informations here and comparing with the PCB reference designe of a componant that I'll use in this board and see what is the efficient way. The PCB ref designe said 4 layers and all vias are through-hole. The layout is not HDI and all the layers have GND plane. There is also only one TL controlled impedance at 50 Ohms. Now I think don't need the buried or blind vias.

Then in that case, do not consider them.

They increase cost & complexity.
As useful as they are for HDI boards, for a 4 layer board there is little use for them.

Buried and Blind vias should be avoided whenever there is a feasible alternative. If you're just having trouble routing traces, then adding another two layers to the stackup is always going to be cheaper than BBV. They should only be resorted to when dealing with very high density routing, like if you have a 0.5mm BGA with hundreds of pins.

@Mattylad and mtwieg. Now I have more clearer vision about BBV and have the answer I expected. Thank's to all.

"BBV's" are sometimes necessary in complex high layer count controlled Z signals and add a reliability risk that must be proved by design verification and supplier process verification. THis cost if done right is far more than the 10% or so extra Fab processing costs but saves much more from a smaller area material which is 90% of the PWB cost in high layer count copper , such that good designs in high volume can be estimated from Copper weight total alone.

Definitely I must forget using BBV's in low density design even with controlled Z signal and low layer count. Thank's SunnySkyguy.