I have designed a lot of 2 layer PCBs so far and am trying to slowly move to 4 layer versions.

One of the major challenges I'm currently facing in that aspect is the acceptable stack up of the layers of the PCB.

I'm currently using the following stack up as I am dealing with a high voltage application.

Could anyone tell me if the stack up I'm going with is accurate? I have attached a screenshot of my current settings in Eagle.

My concern is with the blind vias connecting layers 1-15 and 2-16. Would a pcb manufacturer be able to achieve these interconnects?

enter image description here

  • 1
    \$\begingroup\$ Why would you need blind vias on a 4 layer board? The two inner layers are probably just going to be planes and not signal layers. How high voltage is high voltage and how complex are the high voltage traces that they would need to be routed over/under low voltage traces? I just section an entire part of the board for high voltage. \$\endgroup\$ – DKNguyen Jun 2 at 5:01
  • 2
    \$\begingroup\$ DKNguyen, the voltages are in the order of 7.4 KV and around 3.3 KV at places, and the minimum clearance is somewhere around 10 mm or above. According to IPC 2221, having a buried trace in FR4 can help in increasing the insulation strength between traces and is much better than surface traces. The board form factor is very small and is the main reason why I am running into these issues. \$\endgroup\$ – Kartikeya Veeramraju Jun 2 at 5:17
  • \$\begingroup\$ Hmmm, kV is out of my expertise. \$\endgroup\$ – DKNguyen Jun 2 at 5:20
  • 2
    \$\begingroup\$ I'm not aware of any limitations on connecting layers with buried vias but those are manufacturing details that some fabs might be able to do and others not, so you should talk to your PCB fab. \$\endgroup\$ – DKNguyen Jun 2 at 5:26
  • 2
    \$\begingroup\$ You might have warping trouble with the asymmetry. Talk to your fab. If cost is not a big issue, maybe just make it thicker. \$\endgroup\$ – Spehro Pefhany Jun 2 at 17:49

The problem is indeed with the crossing 1-15 and 2-16 vias. The manufacturer has to be physically able to make the board. There may be a way to attempt that construction, depending on the equipment the manufacturer has.

There are two straightforward ways to get close to what you have drawn.

1) 1-2 core, drill, thru plate. 15-16 core, drill, thru plate. Assemble, drill, thru plate. That gives 1-2, 15-16, 1-16, but not 1-15 or 2-16

2) 1-2 core, drill, plate. Prepreg 15 foil, drill, plate, prepreg 16 foil, drill, plate. That gives you 1-2, 1-15, 1-16, but not 2-16 or 15-16

More expensive, but I have used the process, micro-vias. It's mainly used for their small footprint, to get tracks between BGA balls.

3) As for (2) but with a final micro-via step which is laser drilling 15-16, power set to ablate the prepreg, but stop at the 15 foil. These vias would be very small and fragile, pads connected to them do not generally survive rework.

4) Speculative. The micro-via process only works because of the small thickness 15-16. It may be possible to micro-via from 16 through to 2, via an aperture etched in 15. Ask the manufacturer. They may have the capability. If you wave money at them, they may be able to develop the capability for you.

5) Speculative. You could replace the 2-16 via with 2-15 and 15-16 micro-vias, if the board vendor was happy to insert another micro-via step in the (3) buildup above.

It would be far better to think harder about your layout, and try to use the standard routes.

Do note that your board construction is unbalanced through the Z direction, this is strongly discouraged by most board vendors. It will probably warp after exposure to soldering heat, cracking your ceramic caps.


Without agreeing that you should do this, it's possible to make all the connections you want using mechanically drilled blind vias. You might find you need to make the diameter of the deeper drills (like layer 1 to layer 15) fairly large to ensure good plating in the via. One vendor I just checked requires an aspect ratio less than 1.0, so you'd have a minimum diameter of about 1.7 mm for those vias (But check with your vendor for their requirements).

You will certainly pay extra for all the additional drilling set-ups required.

Another option that will probably reduce cost and improve the aspect ratio requirement, is controlled-depth back-drilling. In this process, you make a through via, plate it, then drill back to remove the plating from the part of the via you don't want connected.

enter image description here

(image source: multi-cb)

You could then fill the hole with non-conductive epoxy to increase the isolation and prevent contamination getting into the path you're trying to isolate. Caveat: I do not work with high voltages, so if this is meant to provide safety isolation, check with your safety expert whether this process will be accepted as providing the isolation you need.

Alos, asymmetric stack-ups are generally not preferred. Probably your vendor will want you to waive any requirements on board bend and twist.

  • 4
    \$\begingroup\$ Strongly second the comment on asymmetric stackup that bugger is going to warp. For this sort of thing you really need to be talking to your board house before you go too far, even if possible you can wind up adding a LOT of cost. You are well into the specialist assembly space where shopping the job to another manufacturer then the one whos advice you took will be 'difficult'. \$\endgroup\$ – Dan Mills Jun 2 at 15:09

As others have mentioned, symmetry is very important with PCB stackup, so you should really aim for that. FR4 can withstand 20 kV/mm (according to Wikipedia, you probably want to verify this from the fab). You require 7.4 kV, so it should be more than enough if you make the thickness of 1-2 and 15-16 both 0.8 mm, which would result as a symmetric stackup.

For vias I'd recommend buried via for 2-15 and blind for 1-2 and 15-16. You can then combine one blind and one buried via in the layout to make 1-15 and 2-16. Though buried via for 0.8 mm dielectric can be tricky.

  • \$\begingroup\$ This is exactly what I was looking for! Also, could you suggest the settings I will have to change to, in order to enable the configuration you suggested? I am very new to the shorthand notation of Eagle. \$\endgroup\$ – Kartikeya Veeramraju Jun 2 at 20:57
  • \$\begingroup\$ I haven't used Eagle for a decade, so I can't help you with that. \$\endgroup\$ – TemeV Jun 3 at 4:11

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.