Connecting internal ground planes on 4layer PCB - Page 1
Forum section: electronics / beginners

author: John Celo
author_rank: Regular Contributor
timestamp: December 08, 2024, 05:12:54 am
content: I'm using a power+signal,gnd,gnd,power+signal layout. This seems like a very simple beginner stackup.Am I supposed to connect two internal ground layers with through vias (the vias that go through all 4 layers)? Have to be very careful with contents on both top and bottom signal layer not interfering in this case!Or am I supposed to use buried vias (connects only inner two gnd layers?)Does jlcpbc (for the budget 4layer designs) even support blind (connects either 1:2 or 3:4 layers) or burried vias (connects layers 2:3)?Does this add extra cost?Am I understanding this correctly?

author: Nominal Animal
author_rank: Super Contributor
timestamp: December 08, 2024, 06:23:11 am
content: Quote from: John Celo on December 08, 2024, 05:12:54 amNo, listed in the Drilling section.With JLCPCB, through vias are the only option, but they don't need to be large: minimum for 4-layer design is 0.15mm diameter hole, 0.25mm diameter ring. Recommeded is 0.20mm or larger diameter hole with at least 0.15mm larger diameter ring (so 0.20mm diameter hole, 0.35mm diameter ring). EasyEda DRC defaults are way too large, so you'll need to edit your Design Rules to match.I'm also a hobbyist, but power+signal/gnd/power+signal/gnd stackup may be even more useful, because the second power+signal plane is then sandwiched between ground planes, so you can do low coupled noise ("shielded"?) traces too.

author: Siwastaja
author_rank: Super Contributor
timestamp: December 08, 2024, 08:55:28 am
content: Blind and buried vias are expensive, usually used only in designs where you truly need that increased density (being able to do routing/components on outer layers with vias hidden underneath).Use normal vias through the whole stack. Also remember to stitch the layers together throughout the design. If you end up filling unused space on top/bottom with ground fill, that will increase need of stitching.

author: Siwastaja
author_rank: Super Contributor
timestamp: December 08, 2024, 08:58:10 am
content: Quote from: Nominal Animal on December 08, 2024, 06:23:11 amYeah, and you pretty much "automatically" transition into this kind of stackup when you realize you are out of routing options and "it would be handy to have a third routing layer".One contiguous ground-only-plane is really fine for everything else except when you have impedance controlled high speed traces on both sides. Having two mid-layers only dedicated to GND seems a bit wasteful, but well if the design is really simple then it doesn't matter.

author: PGPG
author_rank: Frequent Contributor
timestamp: December 08, 2024, 10:07:25 am
content: Quote from: Siwastaja on December 08, 2024, 08:58:10 amI don't understand. I don't see 3 routing layers in this stackup.Quote from: Siwastaja on December 08, 2024, 08:58:10 amHave you noticed that typically distances between top and first internal and second internal and bottom are much smaller then between internal layers. This is not a coincidence.2 years ago I could say that all my PCBs are 2 layers, but if (recently) I have to use 4 layer I assume it is better to have GND return path to any signal as close to signal track as possible (for EMC emission/sensitivity area of closed current circuit counts). To adjacent internal layer you have about 0.2mm but to next it can be 1.3mm (in 1.5mm PCB).

author: Nominal Animal
author_rank: Super Contributor
timestamp: December 08, 2024, 10:44:37 am
content: Quote from: PGPG on December 08, 2024, 10:07:25 amYes. The point is that that distance stays the same, even if you swap the bottom layer with the internal layer closest to it, so you get signal:GND:signal:GND instead of signal:GND:GND:signal (or GND:signal:signal:GND).With signal1:GND2:signal3:GND4 stackup, the signal3 layer is shielded from above and below. If you absolutely run out of signal layers in a tight spot, you can use parts of GND4. The normal ground plane continuity stuff still applies, but having that GND2 relatively nearby makes it a viable option.

author: PGPG
author_rank: Frequent Contributor
timestamp: December 08, 2024, 12:28:41 pm
content: Quote from: Nominal Animal on December 08, 2024, 10:44:37 amMy question was related to suggested by Siwastaja (I hope I understood well) to have 3 signal routing layers and that using two layers on GND seems being wasteful.

author: tooki
author_rank: Super Contributor
timestamp: December 08, 2024, 01:14:56 pm
content: Quote from: PGPG on December 08, 2024, 12:28:41 pmI suspect he meant that once you have completely filled the two signal layers, you can start using one of the ground layers to route what doesn’t fit. (You then leave one ground layer totally intact.) I don’t think he meant dedicating an entire third layer to signals.Another common stackup is two signal layers, one ground layer, and one power layer. There, too, you want to keep the ground layer totally intact.

author: Siwastaja
author_rank: Super Contributor
timestamp: December 09, 2024, 03:15:00 pm
content: Quote from: tooki on December 08, 2024, 01:14:56 pmYes. At that point, for many designs, it doesn't make much difference if you remove the filling from this third routing layer, because you still have one full contiguous ground plane. But when you have high speed traces with significant edge rates (or, impedance-controlled stuff), then having a planevery closeto the signal traces is important, so if you route such high-speed trace on top layer you need uninterrupted fill on top-mid.

author: PGPG
author_rank: Frequent Contributor
timestamp: December 09, 2024, 05:10:24 pm
content: Quote from: tooki on December 08, 2024, 01:14:56 pmBefore even considering to use 4 layers I thought that this is the only one practically used stackup.Later (also before I used 4 layers) someone at KiCad forum said he uses stackup with two internal GND layers. I thought - why I never got that idea - it will be the best for me (as all my PCBs were 2 layer with whole bottom GND (few 0Rs happened to use) I don't see problems having only 2 power/signal layers.Now I have few 4 layer PCBs behind me and all of them with unusual stackup - signal-GND-totally empty layer-power. At power I have 2 or 3 tracks only.