2
\$\begingroup\$

For a new project I am looking to use 8 layers and I am currently figuring out the layer stack I want to use. As for usage, I will most likely go with:

  1. Top
  2. GND Plane 1
  3. Signal 1
  4. Power plane 1
  5. Power Plane 2
  6. Signal 2
  7. GND Plane 2
  8. Bottom

And for an overall thickness of ~1.6mm (because the PCB will be plugged into a connector directly) I was thinking about using four 200um cores and three ~180um prepregs.

However, I just checked the layer stackup proposal on multi-circuit-boards. Unlike me, they did not use 4 cores and 3 prepregs, but 3 cores and 4 prepregs, with electroplated copper on the outer layers.

What are the advantages/disadvantages when using 3 or 4 cores?

\$\endgroup\$
  • 1
    \$\begingroup\$ If you want to use blind or buried vias, that makes your choice (well, not really, as you can move around your assignment of layers). Otherwise, use the stackup that your fab prefers to work with. That way, you're less likely to get delays, errors, whatever, even if the contracts for each do look the same. Two power planes? That's a helluvan investment in useless copper. You might want to dedicate one core with blind vias to a Manhattan pair (that's E-W only tracks on one side, N-S only on the other) if you have problems tracking, it means you can route anywhere without blocking. \$\endgroup\$ – Neil_UK Aug 16 '19 at 16:00
  • \$\begingroup\$ Blind vias are pretty expensive, so I would prefer not to use any. I made good experience with two power planes, as many more complex SoC's require a lot of different power supplies (the SoC in my last project had 14 different power supply voltages/nets). In case of just using a single power supply plane: what would be your suggested stackup to make sure all 5 signal layers have a good ground reference? \$\endgroup\$ – L. Heinrichs Aug 19 '19 at 13:11
3
\$\begingroup\$

This is due to how PCBs are built. Inner layers are etched in pairs to copper that is pre-laminated to both sides of a core. Outer layers are bare copper sheets that are etched when the whole PCB is already laminated. Thus 8 layer boards almost always have 3 cores and 4 prepreg layers because there are three pairs of inner layers. You can find videos in youtube etc that explain how multilayer PCBs are manufactured.

\$\endgroup\$
  • \$\begingroup\$ Hm i was thinking it might be easier to use 4 cores, do double sided etching, and then "just" glue them together with 3 prepregs. I didnt know its easier to not have the outer layers be cores. I will stick to the recommendation of the manufacturer. \$\endgroup\$ – L. Heinrichs Aug 22 '19 at 9:52
1
\$\begingroup\$

There are two differences that I could think of that would be affected by thickness:

  • Heat flow and thermal on power planes, additional material will thermally isolate planes, which may or may not affect your performance of the power planes of being able to dissipate heat or conduct heat. If you have components with high or dense power dissipation.

  • Capacitance between planes and routing of transmission lines (Striplines and maybe differential pairs). If you're routing striplines or embedded transmission lines between layers, then the distance between planes needs to be considered.

\$\endgroup\$

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.