jarvis

Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« on: January 01, 2019, 01:39:10 PM »
Hey Guys,
so I've bought a new pair of studio monitors and since I need a suitable amplifier for them I looked into the the different models of different manufacturers like Hypex, Anaview, B&O ICEPower, Sure etc. A lot of them have a few problems, in my eyes, that I want to address in one PCB:
1. Low input impedance,
2. Unbalanced input,
3. Lack of a power limiter.
What most of them have, though, is an auxilary power output between 14V and 17V, although with limitations concerning the capacitance connected to them (most of them have a limit of between 330-470uF), that I want to use in this project.

Now I designed a board in Eagle based on the design recommendations of the LM317/337 for the ps-section, the THAT design notes for the 1200 series balanced input receivers concerning rf-rejection etc. and the limiter based on Rod Elliotts project 53’s power amp limiter. So the circuit features adjustable on-board power regulation, THAT 1200 series balanced input receivers and an unbalanced opto based limiting section that is buffered by a dual opamp. The output of the buffer is unbalanced but can be impedance balanced out if the power amp has a balanced input (which some have).

Now I have a few questions:
1. Can you guys spot any major errors concerning the circuit or the layout of the pcb? (something like the power supply is to close to the the other components, input/outputs are too close together or the limiters detector circuit from the amps output is not isolated enough)?
2. I’m planning on pouring a ground plane on both sides of the pcb, does that make sense?
3. Rod Elliott talks about potential oscillation problems that may occur when using off-the-shelf optocouplers and states that „some precautions must be taken to ensure that the amplifier's output signal is not coupled back to the input“ (http://sound.whsites.net/project53.htm) but then doesn’t really continue discussing any precautions you can take, apart from straight up not using them. So my question is: are there any precautions I can take in the board layout that benefit the „input-to-output-isolation“ he is talking about.

I’m thankful for any input!

Cheers
Jannis
« Last Edit: January 01, 2019, 02:00:33 PM by jarvis »


jarvis

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #1 on: January 01, 2019, 01:39:58 PM »
And here is the board since I can only attach one picture per post.

jarvis

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #2 on: January 01, 2019, 01:42:42 PM »
Oh and since the schematic in post 1 gives me a 404, here it is again. Sorry for that, I don't know what happened.

Pusch3l

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #3 on: January 01, 2019, 04:02:23 PM »
Happy new year...

Please compare the trace C6/U1 and C12/U2. On the solder pad on U2 that comes from C12 is a trace too much?
In my opinion you could play a bit with the component placement to avoid traces between the solder pads.

Greets

jarvis

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #4 on: January 01, 2019, 07:11:09 PM »
Hey,
thanks for the input, I really appreciate it. Any trace that happens to be between solder pads (also between C17/19 and R24/R25) was actually preliminary and I straight up forgot to delete them, so thanks for the hint. All of these traces are GND connections that are completely unnecessary as soon as I flush the top layer with a GND-plane. I attached a picture of how that looks below.

Best
Jannis

squarewave

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #5 on: January 01, 2019, 08:42:13 PM »
I think you need to connect the LDRs to ground and not just to each other.

jarvis

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #6 on: January 01, 2019, 09:35:53 PM »
I think you need to connect the LDRs to ground and not just to each other.

Hey,
thanks for catching that, you are most definitely correct on that one! What a massive oversight, I will correct this asap.

Cheers
Jannis

abbey road d enfer

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #7 on: January 01, 2019, 11:45:59 PM »
IINM, X1 et X2 are the input XLR's; Pin 1 should not be connected to the audio ground.
Same for X3/4 if there's a possibility to have long cables.

Now, isn't there a connection missing from junction of D3/C15?

We could debate about the actual usefulness of a simple power limiter. That certainly may prevent burning your woofers but your tweeters will still be under the risk of being massively overpowered. It's a very complex subject that is still the subject of heated debates between designers.

Regarding the „input-to-output-isolation“ issue, I have noted the rather high value of R5/10, that makes the circuit rather sensitive to capacitive coupling.
The bridge rectifier results in high-voltage noise (half-wave rectified signal) in the LED's, that is susceptible of serious pollution.

IMO a better option is using a pair of THAT4301 in its usual feed-forward mode. You would not need to return the amp's output signal to the sensitive input board.
« Last Edit: January 02, 2019, 12:50:46 AM by abbey road d enfer »
Who's right or wrong is irrelevant. What matters is what's right or wrong.
Star ground is for electricians.

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #8 on: January 02, 2019, 03:59:56 AM »
D6 , reverse it please .

abbey road d enfer

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #9 on: January 02, 2019, 06:22:26 AM »
Do you actually need the trimmers on the voltage regs? The circuit is pretty impervious to rail balance.
Who's right or wrong is irrelevant. What matters is what's right or wrong.
Star ground is for electricians.


12afael

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #10 on: January 02, 2019, 07:24:22 AM »
I suggest designing a soft start circuit, at least I´m sure that ICE power does not have one. I think it would complete the pack nicely ;) .
heavy metal is the law!!!

moamps

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #11 on: January 02, 2019, 04:34:05 PM »
...so I've bought a new pair of studio monitors and since I need a suitable amplifier for them I looked into the the different models of different manufacturers like Hypex, Anaview, B&O ICEPower, Sure etc. ...

Which model of studio monitors?
Maybe you can do an effective bi or tri-amplification.
Btw, R18 should be 10k and link between D3 and D4 anodes is missing.

jarvis

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #12 on: January 02, 2019, 08:03:48 PM »
First of all I want to THANK YOU all VERY MUCH for the amazing feedback, the ideas and the hints, I'm really grateful for that!
This might be a longer post, since there were quite a few contributions over the night and the past day, but I'd like to answer everything in one post, to not make this thread more cluttered than it has to be.

IINM, X1 et X2 are the input XLR's; Pin 1 should not be connected to the audio ground.
Same for X3/4 if there's a possibility to have long cables.

So just connect everything to the ground of the power supply and leave it at that?

Now, isn't there a connection missing from junction of D3/C15?

Yes, correct. Another error in the schematic that I didn't catch. There should be another connection to D4, so the placement has to change, if I want to go forward with this.

We could debate about the actual usefulness of a simple power limiter. That certainly may prevent burning your woofers but your tweeters will still be under the risk of being massively overpowered. It's a very complex subject that is still the subject of heated debates between designers.

Regarding the „input-to-output-isolation“ issue, I have noted the rather high value of R5/10, that makes the circuit rather sensitive to capacitive coupling.
The bridge rectifier results in high-voltage noise (half-wave rectified signal) in the LED's, that is susceptible of serious pollution.

IMO a better option is using a pair of THAT4301 in its usual feed-forward mode. You would not need to return the amp's output signal to the sensitive input board.

Yeah, I've read through threads on multiple forums and sites concerning that debate and there seems to be no real consensus on how to implement a limiting element and the actual effectiveness of different methods. The ESD project 53 seemed to be a pretty cost effective solution and as I simulated it in LTSpice, it seemed to catch transients sufficiently fast when set coservatively (though simulation is certainly not the real world, so I don't know how it actually performs).

I also came across the THAT4301 while searching for implementations of limiting circuits and THAT even published an application note on the subject, that combines diode clipping circuit with another feed-back implementation (http://www.thatcorp.com/datashts/dn03.pdf). Would that be a better choice, or is this prone to the same isolation problems? Would you recon that a feed-forward implementation would do the job just as well, while being easier to implement?  Going that route would be way more expensive, though (more than 20€). But if it's the safest route, I'd sure take it.

Thanks for the education on input-output-isolation and uncovering the weak points in the circuit! I could certainly lower the values of R5/R10 if that makes a noticable difference. Would shielding the vactrols there help against pollution?

Do you actually need the trimmers on the voltage regs? The circuit is pretty impervious to rail balance.

You are right, the trimmers are not a necessity and calculating resistors and putting them in their place would certainly do the trick. I thought about that and decided I'd include the footprint there since I wasn't sure what impact a slight mismatch might have. Since you can just substitute them with a normal resistor, I thought there was at least nothing lost by including the footprint.

I suggest designing a soft start circuit, at least I´m sure that ICE power does not have one. I think it would complete the pack nicely ;) .

As far as I could tell, a soft start circuit is present on most of those boards including ICEPower and to be honest, I think it would unnecessarily clutter the PCB. And there is a vast amount of kits readily available for that, which only cost between 6-20€.

Which model of studio monitors?
Maybe you can do an effective bi or tri-amplification.
Btw, R18 should be 10k and link between D3 and D4 anodes is missing.

The speakers are ME Geithain ME25 and bi-amping would not be possible without modification of the speakers, since they don't have seperate terminals for tweeter and woofer.

You are most certainly right about the wrong value in the schematic, I forgot to change it after copying the resistor from somewhere else. And yes, as noted above, that connection is missing and has to be established.

Cheers
Jannis

jarvis

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #13 on: January 02, 2019, 08:18:32 PM »
D6 , reverse it please .

Oh sorry, I kind of overlooked your post. Will definitely do, thank you for catching that!

Best
Jannis

abbey road d enfer

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #14 on: January 03, 2019, 02:59:51 AM »
So just connect everything to the ground of the power supply and leave it at that?
Pin  of XLR's should be connected as directly as possible to the chassis ground.

Quote
Would that be a better choice, or is this prone to the same isolation problems?
There would be no isolation problem at all.

Quote
Would you recon that a feed-forward implementation would do the job just as well, while being easier to implement? 
Yes, and probably better. The original bridge rectifier is an excellent compromise between cost and performance, but it's relying on too many things to be perfect.

Quote
Would shielding the vactrols there help against pollution?
No; capacitive coupling is within the optocoupler.
Who's right or wrong is irrelevant. What matters is what's right or wrong.
Star ground is for electricians.

jarvis

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #15 on: January 03, 2019, 03:50:53 AM »
Pin  of XLR's should be connected as directly as possible to the chassis ground.
 There would be no isolation problem at all.
 Yes, and probably better. The original bridge rectifier is an excellent compromise between cost and performance, but it's relying on too many things to be perfect.
 No; capacitive coupling is within the optocoupler.

Very well then, I guess I'll have to look into implementing a feed-forward solution using the THAT 4301. Since that thing seems to be a jack of all trades, it's going to take some time for me to wrap my head around it. Nevertheless, I'm going to read through the application notes and report back with a new circuit and a new board as soon as possible.

So if there's any interest, stay tuned. I'll report my progress and finding here.
Jannis

abbey road d enfer

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #16 on: January 03, 2019, 05:50:04 AM »
Very well then, I guess I'll have to look into implementing a feed-forward solution using the THAT 4301. Since that thing seems to be a jack of all trades, it's going to take some time for me to wrap my head around it. Nevertheless, I'm going to read through the application notes and report back with a new circuit and a new board as soon as possible.
Basically, you'll end up with a fully functional comp/lim with balanced in/out. For a real stand-alone product, you would need some kind of GR indicator.
For your specific application you can use trimmers instead of panel pots; GR indication is not an absolute need but I would recommend a LED indicator taking its drive from the GR voltage.
Who's right or wrong is irrelevant. What matters is what's right or wrong.
Star ground is for electricians.

jarvis

Re: Designing a Buffer/Limiter-PCB for a Class-D Power Amp
« Reply #17 on: January 03, 2019, 06:51:36 AM »
Basically, you'll end up with a fully functional comp/lim with balanced in/out. For a real stand-alone product, you would need some kind of GR indicator.
For your specific application you can use trimmers instead of panel pots; GR indication is not an absolute need but I would recommend a LED indicator taking its drive from the GR voltage.

Right, I'm going through the notes as we speak and it looks very well suited to get a good and versatile AGR with a simple LED indicator out of it. And since I want this to work as a set and forget type of limiter, trimmers are sufficient, yes.

I mean, it's not like I'm aiming for any commercial product here, but I want to make it as well rounded as I can for anyone else, who might also have a use for this circuit/board. Nevertheless, when everything is set and done, I'll be ordering PCBs and I'd be happy to give away surplus boards for the price of postage to anyone interested here at GDIY. I will also happily share the gerber files/eagle files or whatever anyone needs if there is any interest.

Best
Jannis


 

Related Topics

  Subject / Started by Replies Last post
9 Replies
6300 Views
Last post September 15, 2004, 07:12:28 AM
by Svart
25 Replies
14999 Views
Last post February 05, 2007, 06:21:19 AM
by Kid Squid
6 Replies
2338 Views
Last post April 10, 2008, 01:56:14 AM
by bcarso
52 Replies
14296 Views
Last post July 27, 2012, 08:37:15 AM
by dirkwright