I'm working on a PCB with 0.4mm WLCSP's and 0201 discretes. It will have components on both sides. The routing is very tight; I can't use a simple plated through hole ("PTH") design.

I'd like to avoid the costs of sequential laminations. It looks like I can get away with six layers with a single-lamination design. This only gives me one set of blind vias and no buried vias. I've figured out fanouts that should allow for a mechanical drill (6-mil drill; 12-mil ring; filled via-in-pad).

Now I have to decide how to use my stackup. The board has RF at 2.4GHz and 3.5GHz. The transceivers will be very close to their respective antennas.

If I place ground and power planes on L2 and L5, I can use the blind vias for power, as shown:


In this case, one of the power connections will be a blind via and the other will be a PTH. All of my signal routing will have to be carried by PTH's. There are decoupling benefits when using blind vias for power connections. This layout gives me a close reference plane to the RF on layer #1. It also shields the signal layers L3 and L4.

Or, if I put ground/power on L3 and L4, I can use the blind vias for signal routing:


In this case, the routing will be much easier. However, I lose any low-inductance decoupling benefits of the blind vias. Also, my RF on layer #1 is now farther from a reference plane (I'd remove copper on L2 to make L3 the reference...)

The first case strikes me as better, but the second case will significantly simplify my routing.

Is there an obvious better choice here? What are the primary considerations?

  • 2
    \$\begingroup\$ How big are your fine-pitch parts? Usually blind vias come up when you are trying to escape a big BGA, and you end up having to use them for signal rather than power/ground. Can you do a controlled depth drill that reaches through 3 layers instead of just 2 (There will be limits on aspect ratio for this)? \$\endgroup\$
    – The Photon
    Commented Sep 19, 2018 at 0:50
  • 1
    \$\begingroup\$ Thanks, @ThePhoton. The largest of the 0.4mm wlcsp's is a 7x9 grid, but not all the pads are being used. I can break it out with 3 layers (including the top), even if I just use PTH's. I want to use blind vias to assist with routing - the board is very dense and has wlcsp's on both sides. Option 2 will help immensely. But Option 1 would probably help "enough", if Option 2 is ill-considered. \$\endgroup\$
    – bitsmack
    Commented Sep 19, 2018 at 4:58
  • \$\begingroup\$ BTW, @ThePhoton, thanks for the "controlled depth" idea. I hadn't realized that this was a thing :) I'll talk to my board house. \$\endgroup\$
    – bitsmack
    Commented Sep 19, 2018 at 4:59
  • 1
    \$\begingroup\$ I mostly see them used for back-drilling, but I found a Sanmina document that shows them used for blind vias. I worry you might need to use a pretty big diameter to be sure the via plates correctly. \$\endgroup\$
    – The Photon
    Commented Sep 19, 2018 at 5:01
  • \$\begingroup\$ In case one you have better control on cross talk reduction and in case 2 the GND/Power sandwich could make very good buried capacitor for you if the prepreg is not very thick but you have to be cautious about cross talk. \$\endgroup\$
    – BD_CE
    Commented Oct 28, 2018 at 4:38

1 Answer 1


Well, PCB is a circuit itself and needs lots of reviews. One of the main goals in a good PCB is providing lowest possible loop area and controlled return paths for the signals. To do that, we normally use power planes as return paths. Power planes are also good for making high frequency response buried capacitor inside the PCB. the less distance between power plane and a signal layer is equal with less cross talk on the signal layer and the less distance between sandwiched power/GND planes is equal with higher capacitance of the buried capacitor. the best bypass 0201 capacitors are not so good for 1GHz frequency or higher but the buried capacitor has very good capacitor up to 4~5 GHz.

In case "1" the GND layer (L2) could be a good return path for layers L1 and L3. Layers L3 and L4 are separated with relatively long distance (prepreg). L5 is power plane and also usable as return paths for layers L4 and L6. In this case you have good control on cross talk reduction and Emission/susceptibility reduction due to providing controlled return paths.

In case "2" Providing return paths for Layers L1 and L6 is hard and also controlling cross talk in layer pairs L1/L2 and L5/L6 are hard too. The good point is the power planes sandwich that is made a buried capacitor but its capacitance is highly related to reduction of the prepreg's thickness that is normally not in the hands of the designer and depends on the budget and the manufacturer capabilities.

PCBs must be symmetric too. in both cases "1" and "2" copper balancing of the layers depends on the PCB drawing and making copper density balanced PCB is possible.

Due to the RF parts of the circuit, normally we have to follow chip manufacturer's reference design and line impedance characteristics. therefore these limitations are effecting on the layer thickness, trace widths and distance between layers.

  • \$\begingroup\$ it is very kind of you. \$\endgroup\$
    – BD_CE
    Commented Oct 30, 2018 at 4:47

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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