Charged capasitive layer inside a pcb - is that really so fantastic? - Page 1
Forum section: electronics / beginners

author: FriedMule
author_rank: Frequent Contributor
timestamp: April 04, 2019, 11:59:53 am
content: I have read a forum post on a HI-FI site, where a person talks about shielding between the power tracks on one side and audio-signal on the other side.He says that the absolute best on earth is using a 4 layer board, where the two inner layer act as a capacitor with constant DC power on.In other word, making the two inner layer work as a charged capacitor that blocks any AC or other signals from going trough. The two layer is charged by two separate wires, going directly from the PSU.Is that real or just ehm, audio-talk?

author: apblog
author_rank: Regular Contributor
timestamp: April 04, 2019, 12:29:08 pm
content: there are good reasons to have a ground plane, but capacitance is not one of them.If you enter the plane area and separation into a capacitance calculator, you will see that the capacitance is very small.The highest quality audio recording equipment, stuff that nobody could question, frequently does not have a ground plane on the PCB.

author: AndyC_772
author_rank: Super Contributor
timestamp: April 04, 2019, 12:30:36 pm
content: He's right, but for completely the wrong reasons.A capacitor doesn't block AC, it passes it - but the amount of capacitance formed by the planes in a PCB is so tiny as to be virtually undetectable at audio frequencies. (It's really important in digital circuits operating at hundreds of MHz and above, but that's for different reasons and has no relevance in audio).Charging a good quality capacitor - and a 4 layer board with solid planes meets this definition - makes no difference to its impedance. Xc=1/jwC regardless of dc bias.A solid plane acts as a shield, and is undeniably beneficial. Two solid planes may be very slightly better, but not for reasons that have anything to do with the fact that they form a capacitor. If anything, the capacitor effect allows coupling between them, and moving them further apart (eg. by using a thicker PCB) would help improve the screening effect.Tip: this is often why running a ground trace between a noisy signal and a sensitive one helps. The benefit is nothing to do with the ground trace itself; it's simply that it forces the two other traces to be further apart, so the field strength at the sensitive trace is reduced.

author: filssavi
author_rank: Frequent Contributor
timestamp: April 04, 2019, 12:35:10 pm
content: As always with audiophools there is a nugget of truth behind a pile of 💩Interplane what they are referring to is interplane capacitance, and while of very low value (100s of pF at most for large boards, it is one of the best high frequency capacitors available due to the very low inductances and is crucial when the design is going to work in the 100s of MHz or higher regionWith tat said there are 2 big caveats:-at audio frequencies it is completely useless-you usually need a special “inverted” stackup with prepreg in the middle and core outside that is going to be more expensive

author: FriedMule
author_rank: Frequent Contributor
timestamp: April 04, 2019, 12:55:49 pm
content: Okay, so we are talking about the same as "the skin effect" of wires do exist but no ware near 20kHz?Do I understand correctly in that a single or double copper layer, connected to ground, is fare better then any 0.5pF of capacity?Should these two inner layer be connected via "vias" or separately connected to ground?

author: AndyC_772
author_rank: Super Contributor
timestamp: April 04, 2019, 01:19:40 pm
content: The problem needs to be clearly, specifically defined before it can be answered correctly.If the question is, "does a solid plane act to reduce interference between a noise source on one side of the board and an audio trace on the other?", then the answer is 'yes'.If it's "does connecting a capacitor between a noise source and an audio trace reduce interference?", then the answer is 'no', quite the opposite.

author: FriedMule
author_rank: Frequent Contributor
timestamp: April 04, 2019, 04:41:30 pm
content: Thanks, my question is also therefore, to avoid the capacitor "effect" I think that i need to make some connection between the two layers.Can I just do that by make a row of via's 1-2 mm around from the edge, Or do I have to make via's in the center of the PCB also??

author: AndyC_772
author_rank: Super Contributor
timestamp: April 04, 2019, 05:22:34 pm
content: No, I still think you're misunderstanding.If one plane were connected (only) to the noise source, and the other were connected (only) to the audio signal, then the capacitor formed by the planes would be a way for noise to couple from one to the other. The effect would be small because the capacitance is small, but it would be a real effect that you could measure. You might even hear it, possibly.However, that's not the circuit. It is NOT the case that just placing a capacitor between two signals, without actually connecting it to those signals, allows noise to couple between them.A solid ground plane placed between two layers of the board acts as a shield. A second plane might also act as a shield, but since you already have one, there's no extra benefit especially at audio frequencies. Whether or not you join them with vias at the edges, in the corners, at a single point, or at 2mm intervals over the entire surface of the board, makes no difference.

author: T3sl4co1l
author_rank: Super Contributor
timestamp: April 04, 2019, 06:49:28 pm
content: Quote from: AndyC_772 on April 04, 2019, 12:30:36 pmOr, even more precisely -- a parallel capacitor to ground acts to block AC transmission (shunting it to ground), while a series capacitor acts to permit AC transmission (exclusive of DC transmission).And, even more generally, the purpose of parallel planes within the PCB is to achieve a low impedance, nevermind the capacitance. In general -- that is, over hundreds of MHz of bandwidth (such as matters for digital and RF circuitry, the domain where this kind of thing matters), the impedance will be up and down, not simply one way or another. The plane helps in achieving a particularly low impedance across the band. Compared with single capacitors, that have an impedance that falls until the SRF, then rises again. (Mind, you still have to be careful when putting together planes and different capacitors: they can resonate against each other and make things worse. PDN (power distribution network) analysis isn't terribly hard, and is cheap insurance!)To echo the point others have noted: notice this is only relevant at high frequencies. At audio frequencies (up to and including the low ~MHz, where active devices are just rolling off*), planes aren't very important.*Rolling off, i.e., gain is near 1, and phase shift is large (>90 degrees?). This is a sensitive region, and it doesn't take much phase shift to turn it into an oscillator. That phase shift will arise in the form of lumped capacitance or inductance though, because again, the frequency is fairly low (say, a wavelength of ~100m).Tim

author: FriedMule
author_rank: Frequent Contributor
timestamp: April 05, 2019, 12:49:28 am
content: Thanks, so if we are talking about a 4 layer board, it would be fare better to use the two topmost layers for the audio (running same track on both of them), 3th layer as shield and the bottom layer to power, to lower the impedance?