Help for LM1875 PCB layout

[ozlow.own]

Hi all! 

I'm trying to design a PCB for a LM1875 amplifier (the circuit won't drive a speaker, but a reverb tank: hence the non-standard choice of values some components).
SCHEMATICS:


I've read the LM1875 datasheet and I'm worried about the layout. Seems that it needs a carefully designed layout. It's like the 4th PCB I'm designing in my life and I've never had my PCB public or someone helping me, so I never received any feedback about it.

TOP:


BOT:


I'd like to know if the circuit can be prone to oscillation, capacitive coupling and problems like that with this layout. I tried to run separate traces for power ground, compensation, output and signal ground (actually the ground for low level signals is completely separated on this PCB, I will join the two grounds in star ground point in the PSU PCB). The curved traces are just to try something new

If you need more clear pics of the PCB (3D view or some other way to see better the PCB) just ask.

[JS]

It shouldn't oscillate if that's your concern. Maybe taking the inverting input components closer to the pin could help with that, they are a bit further away...

There are some other considerations. Star ground is for electricians, not for PCB routers. It's been used as a way to cheat and get away with poor designs but not the right way to do it. For signal integrity you want a single ground (maybe two for noisy stuff like digital, lights and relay switching etc.) but one analog ground, which should follow the signal thinking it as a differential signal. I should have a drawing around there to explain this more clear, I'll try to find it.

Think it this way. Most of the current goes to the load by the output pin of the output stage, that current comes from rails, that rails needs to close the current path to ground from the power supply (decoupling caps for fast response) that ground needs to close the current path to the load.

That last stage acts as a load for the previous stage, and do on till youtube.com get to the input of your circuit, at which point you should treat your input signal as differential even if it comes unbalanced and referenced to ground. In that case you use the ground of the source as reference for the signal.

Let's say your input circuit is an inverting stage, the non inverting input should go to the ground of the input and from there some resistorand to your local ground to ensure dc bias to your input stage even if the source is ac coupled or not connected.

If the input circuit is non inverting you need to watch the path for the current in the feedback network

JS

[ozlow.own]

Thank you for answer.
As i said, i never got feedbacks about my works so, being a newbie, i need every kind of advice...all considerations are welcome!

I don't think i got all you said 
I've always read that for minimizing noise in sensitive audio circuits (i.e. mic preamplifiers with a lot of gain) i should go for a star ground topology. Here's what i mean:



I've planned to wire all the grounds separately to a common large pad on the PSU board (the dotted line you see from the PSU board to the main board is the "GND_S", separate from "power" ground).
The reasons I've always read associated with this practice are:
1) ground loops - as far as we have one ground connection for every board it's impossible to have a ground loop, as long as you connect the boards with just the signal wire;
2) high current return: PCB traces got a resistance value. If we've got high current flowing into the ground trace, for Ohm's law we "raise" the potential from our ground reference point.
We could get rid of this second motivation just running two separate grounds: one for power and high current devices (and digital/impulsive/noisy stuff) and one for all the other components.
I probably understand the reason behind treating a signal as a differential signal with his ground - it's about common mode interference, right? So I should take the ground coming from the input jack and routing it together with the input signal (and then join it with my ground PSU of course)?

[JS]

Ground loops is a no no, of course, hence the resistor I told between the input ground and the circuit ground.

Now, vumeter should be treated as noisy stuff, as switching and digital. Power output no, it's not noisy, it's signally! Ground there should be trated as precious signal, the previous stage referenced to it, it doesn't matter if the ground there isn't the same ground than at the power supply, that's just a concept, you need your consecutive stages to agree in the gound, so each stage should take the ground reference from the same place the previous stage output, then that stage from the previous one and so on. Probably the most adequate point to connect all the grounds to the power supply is close to the last stage bypass caps.

  It's very very important to understand and consider opamps as 5 terminal devices, not 3 terminal devices that need power, as current at the output will always come from one of the power rails, then come back from the load to ground and through the bypass cap to the rail again, this loop should be keept small and closed, taking the ground to the PS and back is bad, same for inter stage grounds.

JS

[ozlow.own]

OK! A 10 to 100 ohm between audio input and output ground and PSU ground seems to be the way to go. This will solve the ground loop problems that will occure whenever I'll connect the unit with a earth-connected device, preventing the ground loop (actually limiting the current in the ground loop, from what i understood).

Yep, the actual star ground will be at (-) of the last bypass capacitors.
I wired the LM1875 "output" ground separately because of the stability chapter in the amp datasheet (for high currents). I actually planned my ground layout from this: http://www.circuitbasics.com/design-hi-fi-audio-amplifier-lm3886#Designing-the-Ground-Layout

[JS]

Again, no.

Star grounds is a safety concept used by electricians, in electronics isn't any good, just brute force to make it work without giving s***t about it, not an optimal solution.

First you are not making a 40W amp, still good grounding should be done. Then, what that article says is that high current ground path shouldn't cross low current ground path. That means a high current path shouldn't share conductors with low current path, but the high signal current is closed at the output stage bypass caps, not at the power supply.

  If ground goes to the power supply with a wire and come back with a separate wire for high current and low current you are actually sharing more path than connecting them together at the pcb, as all the coming back from power supply to pcb at the high current side has high current for whatever your bypass didn't cover and that polutes more than a short trace putting together both at the pcb.

You will have to wait the drawing, I've been away from the pc since this topic started, if I can't find it I can make it again so to explain, and save it better this time as it's a discussion that always pops up.

JS

[ozlow.own]

I'll wait for the pic then, I'm definitely not on it. Thank you for patience!

[Relayer]

Hello ozlow.own,
You really need to read the data sheet of the LM1875.
Here's a portion I picked out for you:

When designing a different layout, it is important to
return the load ground, the output compensation ground, and the low level (feedback and input) grounds to the
circuit board ground point through separate paths. Otherwise, large currents flowing along a ground conductor
will generate voltages on the conductor which can effectively act as signals at the input, resulting in high
frequency oscillation or excessive distortion. It is advisable to keep the output compensation components and the
0.1 μF supply decoupling capacitors as close as possible to the LM1875 to reduce the effects of PCB trace
resistance and inductance. For the same reason, the ground return paths for these components should be as
short as possible.


You have to remember one thing, this IC has been around for quite some time, therefore
people who have produced this amplifier using this IC, have had excellent results without
the need for modern ways of producing it (i.e. Old school ways).
I hope the above helps.
Regards,
Relayer

[JS]

Well, here it is!


I use the image on this post https://groupdiy.com/index.php?topic=59590.msg756894#msg756894
You could check the explanation there and ask again, I mention 8 bypass caps, because the discussed design used two output opamps as a differential drive, so paralleling 2 caps for each position, 2 opamps, 2 rails add up to 8 caps, call it two in a simpler design as the pict. Seen it from now, 6 should be fine as the bigger ones could be shared and further away from the opamp, but still between output and load as I'll explain.

  There it is an inverting stage, but look how it looks like a differential amplifier, if rG1 and rG2 were actual resistors and not parasitics of the PCB. If this is the last stage the PS ground should be connected to the bypass caps and rG1 to the a previous stage's bypass caps. Bypass caps might bring noisy ideas to your mind but they are the ones that carry the signal current from rails to ground, so think them as signal decoupling caps, as ac coupled current signals, going from opamp "vcc/vee output" to the load or receiver reference ground.
  If it were a non inverting amplifier, swap the input with the rG1-rG2 node, leaving the non inverting input to the input as it should and the resistor from the inverting input to the rG1-rG2 node.

With this you should see how the ground follows the signal, if your ground is messy you might get crossed resistances along those 3 and even some between this circuit and adjacent ones. Then, how to integrate this to a ground plane is kind of tricky, but think in component placement so it behaves like this, leaving the non inverting input closer to the input and the bypass caps between the opamp and the output, close to the opamp, and close to the output signal trace. As I explained in the original post this is how you squeeze the best THD+N figures of the given opamp/circuit.

JS

PS: along this topic I messed with decoupling caps and bypass caps, calling decoupling to what it should been bypass, so did the guy who wrote the datasheet. Decoupling os for AC coupled signals, bypass is from rails to ground, close to the opamp as a dedicated current path.

[ozlow.own]

Hi Relayer!

Thank you for your contribution. I've actually seen some existent layout for the LM1875 looking for a guideline: many of them use a ground plane or a "star ground" wiring. Seems that the latter one (and also the first one, as seen as can easily mess with high current return path) are not really ok, as pointed out by JS.

JS, thank you for your pic! I'll have to slowly read your topic on GroupDIY. Then I'll be back for some other questions for sure.