understanding source+return current flow on PCBs

Status
Not open for further replies.
Jump to Latest
#42
CharlieLaub said:
Here's another question I have about the ground plane concept: since I am using a 2-sided board, the signal and ground sides are separated by the PCB epoxy board itself. Is that OK? Does a ground plane need to be the layer "right next to" the signal layer it is serving? For instance, would a board with a "back" layer, then the epoxy board, then ground plane and then signal plane be better?
Click to expand...

If you look at some of the 2-sided examples in audio datasheets, you will see that designs using one or both sides as a ground plane are not uncommon. See TPA6120 evaluation module TPA6120A2 Evaluation Module (EVM) - TPA6120A2EVM - TI Tool Folder. Currents flow line-of-sight, so judicious component placement can mean that flood-filled areas are quite acceptable, but in that case the path should be laid out physically to a notional point before filling to verify that currents do not cross.

Some people may object to this approach (on ideological grounds?), but Ti are trying to sell their parts, so I would expect this device to meet its datasheet specs on their board. This is an interesting board because it also satisfies the chip's heatsinking requirement using the copper on the board.

4-layer boards are more required for their connectivity, their ability to route high-speed digital signals on controlled-impedance microstrip, stripline or co-planar waveguide, greater EMC performance, or where miniaturised enclosures must be implemented on a PCB to keep emissions from e.g. a local oscillator from impacting other sensitive areas of a radio receiver. You should be able to do anything you need for some time with 2-sided.
 
#44
CharlieLaub said:
Here's another question I have about the ground plane concept: since I am using a 2-sided board, the signal and ground sides are separated by the PCB epoxy board itself. Is that OK? Does a ground plane need to be the layer "right next to" the signal layer it is serving? For instance, would a board with a "back" layer, then the epoxy board, then ground plane and then signal plane be better?
Click to expand...

The ground plane on the back of a double sided board is nest to the signals, have a look at some of the documentation I posted earlier.
The traces on this sort of layout (double sided with a groundplane) are microstrip. Better still is having the signals run between two groundplanes (stripline) where you get much better TEM signal transmission. The effect of this is minimal for audio signals and for most high speed up to the low GHz range with standard FR4.
 
#45
marce said:
Some part numbers then...
Click to expand...

Ah, don't be ridiculous, there's not an opamp in a regular 8- or 14-pin package with a ground pin. Or perhaps you'd like a list of variable Vregs.

Stop quibbling about a trivial side issue. You're just miffed because I shot your fox.

BTW, as I recall Doug's opamp/poweramp was a massively parallel unity gain buffer, nothing differential there at all.
 
Last edited:
#47
abraxalito said:
I'll humour you on this one....



Off the top of my head:

AD797
AD811
AD744
AD712
NE5517
NE5532
NE5534
TDA2030
TDA2040
TDA2050
LM1875
LM6172
TL084
TL074

enough to get your teeth into for starters? Never had to lay out a PCB with any of those?
Click to expand...

Yes I realised later on this morning that I've been having a brain f***...woops even sat looking at a design with OP249, I was getting the decoupling down to GND and not exactly working on all cylinders. To make it worse for me its the example I posted above and on my screen the GNDs are bright green. Boy do I feel very foolish this morning, cheers for humouring me Abraxalito.
It stems from what seems to be a big argument and point scoring exercise regarding single ended signals decoupling supplies to GND against decoupling across the decoupling supplies, that seems to be following me across threads and becoming a bit personal.
 
Last edited:
#49
Well certainly valid points here. The ICs listed don't have an explicit ground pin. BUT, the IC I am using and that receives the board inputs DOES HAVE an explicit ground pin AND is run from dual supplies. All the inputs are at ground potential (like the inverting amplifier configuration for an op-amp) so I need to keep the ground pin at a very stable reference voltage.

On another point, from what I seem to be gathering up from the many posts I have read is that:
The idea of bypassing a supply to ground stems from (early) single supply implementations. In a single sided application Vcc to ground is between the highest potential and lowest potential on the board. For dual supply applications, the highest and lowest potentials are the two supplies, so bypassing caps should be placed between these as close to the IC pins as possible.
For dual supply applications, caps between each supply and ground perform the function of "storage". Large caps store charge for low frequency demand and can be some distance from the IC. Because of track inductance, small caps between each supply and ground can be located close or closer to the IC supply pins to supply charge for high frequency and transient signals.

Is the above correct? Anything to add here about supply and bypass caps?

@ counterculture:
Thanks for posting the illustration of the current flow in your post here. It's a very good illustration. It might be slightly clearer if the load resistance was labeled as such. This is helpful (for me) and is a good visual about what tracks to keep together to reduce loop area.
 
#50
It's certainly true that when I wrote that 'decoupling caps are placed across the power pins' I intended to cover the case of single-sided operation, such as +5V TTL logic. I had hoped to avoid too long-winded a discussion of decoupling, but this proved impossible. I noted in passing Doug's recommendation regarding the decoupling of opamps and I thought it gave me room to state a broad generality without exciting too much opposition. I tend to think of bulk electrolytics as PSU smoothing, and caps local to the chip as decoupling, pretty much as you have restated it there.
 
#51
The really nasty gotcha is that in an class AB opamp output stage the current demand switches from one rail to the other depending on which quadrant the load is being driven in, and the annoying fact that the Vas stage is a integrator referenced to one of the power pins means that you NEED solid decoupling between this pin and 'ground' if the thing is to be stable...

Some of the modern 'audio' opamps have GBP in the 50MHz region and slew at tens of V per microsecond, making this more of an RF excersise then a DC - 20K one.

The loop that matters is usually opamp output -> load -> decoupling caps (both of them) -> opamp power pins.

One other thing to watch is the plane inductance when combined with a couple of modern low ESR caps of the large value elco sort can actually have a moderate Q resonance in the audio band, not fun on a square foot of board, sometimes adding esr on purpose is the right thing to do.

Regards, Dan.
 
#52
On pages 119~120 of Small Signal Audio Design:

'The essential requirement is that the positive and negative rails should be decoupled with a 100nF capacitor between them, at a distance of not more than a few millimetres from the opamp; normally one such capacitor is fitted per package as close to it as possible. It is not necessary, and often not desirable, to have two capacitors going to ground; every capacitor between a supply rail and ground carries the risk of injecting rail noise into the ground.'

This is evidently the principle being employed in the opamp/poweramp, which is incontrovertibly single-ended (not differential), but has 100nF across the rails at each package.
 
Last edited:
#53
 
Last edited:
#54
Power Supply component connections to IC's etc are important, but so are the ALL the audio components connected to Common, often called Ground/Earth. I say Common because sometimes there is NO connection to Ground/Earth. In fact circuits do NOT require one to work correctly ! Think of All the audio devices etc such as portable radios/stereos etc that have NO such connection, but still work. & even home equipment that is mains powered, but only has a 2 core lead that is only Live & Neutral. Sure there are lots of gear that does have a 3 core lead that is earthed to the case, & often the circuit in some way too, but that is usually for safety.

If due consideration isn't taken to how ALL the audio connections to the Common are connected, then don't expect to get the lowest possible hum reduction you could have ! That's why i posted the previous screenie showing how i Have acheived this in my PreAmp, that i designed & built some time ago. Unwanted modulating AC current can be injected into other and/or near and/or adjacent components, via the Common PCB tracks, if they are not returned individually to the Common point. The same goes for the PS connections configuration.

I would be a Lot more concerned about the above, than any "potential" parasitic issues !
 
#57
Zero D said:
If the Common lead/s from PS decoupling capacitors are connected DIRECTLY to Audio Common, then all sorts of grunge can be injected
into it, & therefore Audio components = Not good !
Click to expand...

If a local loop is correctly made, this does not happen. A single star ground for all return leads (even if this were physically possible) is not good practice.
 
#58
CharlieLaub said:
OK, I will just post the layout that I created so that it can be critiqued here in terms of grounding and signal routing. Please refer to the attached pic when reading the following.
Click to expand...

Input and output connectors are better placed at the same side of the board.

A common mode current flowing in your cable shields will then go from one connector to the other and not though the whole board.
 
#59
Zero D said:
If the Common lead/s from PS decoupling capacitors are connected DIRECTLY to Audio Common, then all sorts of grunge can be injected into it, & therefore Audio components = Not good !
Click to expand...

Are you referring to bypass caps at the ICs or PS reservoir caps in the above statement???

I have heard this stressed before, by AndrewT for instance, but I am really confused. I have seen diagrams that explicitly show a connection of some finite length between the common connection of the PS cap grounds and the main audio ground. So if you have an onboard power supply, how are you supposed to achieve this??? Run a long track from the PS across the board and then connect grounds to it??? Won't that just increase loop area? Currents are returning from the circuit to the power supply via ground. Either these current flow through the main audio ground and pollute them, or have to be connected to the PS cap common point, and so get polluted there. I don't see how a track on a PCB could possible achieve all that much "isolation" of the ground. See why I am confused here?

Also regarding statements "star ground is bad": why then do so many promote using a star-ground? How many power amps use a ground plane? Use plane for line level circuits and star for power amp? This is yet more confusion... 😕

Anyway, I will hopefully learn from ongoing discussion here, so let's keep the discussion going!
 
Status
Not open for further replies.
Top Bottom