4 layer PCB, 2 gnd layers? - Page 1
Forum section: electronics / projects

author: trevwhite
author_rank: Frequent Contributor
timestamp: October 27, 2016, 12:21:30 pm
content: I am creating a 4 layer board. I have the topside as 0V. The inner top layer for signals. I was thinking of also having the inner bottom layer as 0V. The bottom layer is for signals and components.My concern is that if I have two ground layers will this create noise and issues with ground loops? Some of the ground paths have 1,2 and 3 amps on them.ThanksTrev

author: TiN
author_rank: Super Contributor
timestamp: October 27, 2016, 12:32:47 pm
content: Questions like these are pretty much meaningless without a board image/layout drawing. Is it high-speed? High-power? Analog? Digital? Different rules apply.Usual layout for mixed signal stuff is top and bottom for signal, inner for power planes (GND/VCC) for 4-layer. Very common GND is second layer, under top, to provide solid reference plane for signaling on the top side.If you have high-frequency/RF stuff, often opposite, top and third are ground, and sensitive signal on the second layer, while power and aux signals on bottom.

author: trevwhite
author_rank: Frequent Contributor
timestamp: October 27, 2016, 01:17:02 pm
content: The way the board ended up all the components are on the bottom side. Maybe this is the 'normal' topside. So really my bottom inner wants to be my primary 0v so as to be a nice solid ground under the component side and the signals. Then there are some other signals on the next inner layer.I think my main question though is the difficulties in having two 0v layers? There isnt any high frequency stuff. 1Mhz near a switch mode. Maybe I shall just stick with 1 0v layer. There are a couple of 0V return paths that might see up to 3A.I do need to heatsink a bit through the 0V. That was the other reason for wanting an external layer as 0v as well.

author: tszaboo
author_rank: Super Contributor
timestamp: October 27, 2016, 01:31:05 pm
content: I dont know what is the size of the board and such, but you can put two GND layer on a PCB. Just connect them together with a bunch of vias. If you are interested in RF and such, look it up how, if you are not, just place a via every ~5mm on the board edge and next to traces. It is never going to be worse than a two layer board, unless you do something very bad intentionally.3A is really nothing.

author: dmills
author_rank: Super Contributor
timestamp: October 27, 2016, 01:33:14 pm
content: Just make sure everything is stitched firmly together, most CAD tools can automatically add via stitching between planes.Your internal signal layer will probably be mostly reference to the closer of the ground planes, so ensuring there is stitching near where the signals from this layer change layer is important (If you have edge rates fast enough to matter).I would however point out that buried signal layers are a pain in the arse when it comes to prototypes because they are hard to access. Unless you have a pressing reason, the more conventional stackup of Signal-Ground-Power-Signal is easier to modify, and the power plane is usually just as good a reference as the ground plane is providing the two are adequately coupled by 'decoupling' caps.

author: trevwhite
author_rank: Frequent Contributor
timestamp: October 27, 2016, 01:45:05 pm
content: Thanks all.That is a good point about the signal tracks being buried. I may well move the inner signals to the other outer layer.

author: eb4fbz
author_rank: Regular Contributor
timestamp: October 27, 2016, 03:19:50 pm
content: Just use lots of stitching vias to increase the frequency of possible ground loops. Above 1GHz the ground loops between two planes gets impossible due to the parasitic capacitance between them.

author: trevwhite
author_rank: Frequent Contributor
timestamp: October 27, 2016, 04:53:05 pm
content: Thanks this is really useful information and much appreciated.

author: CraigHB
author_rank: Regular Contributor
timestamp: October 27, 2016, 05:56:40 pm
content: Traditionally you use the inner layers for power and ground, but sometimes there's just not that much power routing. Don't need a whole plane for power when the board carries various supply voltages. Then it's like which voltage do I put on a plane. The choice I make is no power plane.A couple times I've used three layers. The option is always two or four layers so I just tie the two inner layers together in those cases. Hasn't given me any trouble, but as stated it depends on what the board does. The ones I've done were for power applications so RF stuff didn't come under consideration. Usually there's enough ground vias for components to tie the planes together.