Building a TPA3132 amp board - Page 2 - diyAudio
Go Back   Home > Forums > Amplifiers > Class D

Class D Switching Power Amplifiers and Power D/A conversion

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 26th February 2014, 10:50 PM   #11
rosvall is offline rosvall  Denmark
diyAudio Member
 
Join Date: Dec 2009
Damn, it doesn't look like anyone stocks the NJU7181 and i can't figure out what to search for to get an alternative.
  Reply With Quote
Old 27th February 2014, 08:23 AM   #12
diyAudio Member
 
Saturnus's Avatar
 
Join Date: Jun 2005
Location: Copenhagen, Denmark
That is unfortunate. Well, there's always the option to build it from the ground up. Basically, you'd just need an input amplifier and a comparator like here Signal Detecting Auto Power-On Unit. Just scrap all unneeded parts relating to the relay. And choose op-amps that run at very low idle current.

On the new PCB layout; what a mess. I'm pretty confident in saying that it will have huge issues.
  Reply With Quote
Old 27th February 2014, 08:37 AM   #13
rosvall is offline rosvall  Denmark
diyAudio Member
 
Join Date: Dec 2009
Quote:
Originally Posted by Saturnus View Post
That is unfortunate. Well, there's always the option to build it from the ground up. Basically, you'd just need an input amplifier and a comparator like here Signal Detecting Auto Power-On Unit. Just scrap all unneeded parts relating to the relay. And choose op-amps that run at very low idle current.
It just seems like it would take up a bunch of precious board space. What i really want to squeeze in is an active 4th order linkwitz-riley crossover
Quote:
Originally Posted by Saturnus View Post
On the new PCB layout; what a mess. I'm pretty confident in saying that it will have huge issues.
I'm sort of new to this, i'd really appreciate some more specific criticism.
  Reply With Quote
Old 27th February 2014, 08:59 AM   #14
diyAudio Member
 
Saturnus's Avatar
 
Join Date: Jun 2005
Location: Copenhagen, Denmark
Quote:
Originally Posted by rosvall View Post
It just seems like it would take up a bunch of precious board space. What i really want to squeeze in is an active 4th order linkwitz-riley crossover
For what purpose? In a general amplifier design it is inherently a bad idea to include active filters as most people would want these to be adjustable, not only in frequency but also in topology, slope, etc etc.

For while you might like a 4th order LR xo, other people would probably prefer hybrids of 2nd order BW HP and 2nd order LR LP to get a phase and amplitude coherent filter. Or a bandpass filter. Or something completely different. Or nothing at all which means it's all just wasted space.

The circuit above was just a reference. There's tons of ICs that integrate an input amplifier and a comparator directly on a single chip cutting away most of the external parts.

In regards to circuit lay-out, I'll get back with a more detailed analysis.
  Reply With Quote
Old 27th February 2014, 10:44 AM   #15
rosvall is offline rosvall  Denmark
diyAudio Member
 
Join Date: Dec 2009
Quote:
Originally Posted by Saturnus View Post
For what purpose? In a general amplifier design it is inherently a bad idea to include active filters as most people would want these to be adjustable, not only in frequency but also in topology, slope, etc etc.

For while you might like a 4th order LR xo, other people would probably prefer hybrids of 2nd order BW HP and 2nd order LR LP to get a phase and amplitude coherent filter. Or a bandpass filter. Or something completely different. Or nothing at all which means it's all just wasted space.
You do, as always, have a very good point. It would make it a lot less versatile. But this amp is specifically for active speakers now, without the output filter.
And I think a cheap, all-in-one active (two way) speaker amp with XO would be useful. But, yeah, configurability. I suppose the right way to it would be with a DSP, and the cheap way would be with a couple of fixed frequency versions and a trimmer for tweeter volume.

Quote:
Originally Posted by Saturnus View Post
The circuit above was just a reference. There's tons of ICs that integrate an input amplifier and a comparator directly on a single chip cutting away most of the external parts.
I was considering something stupid like amplifying the difference of the 3V-biased positive inputs, a diode detector and the mute input. But it just dawned on me, that any sort of auto-power off will put a lower limit on output volume. I imagine it would be quite fiddly to get right. How annoying is it, in your experience?

Quote:
Originally Posted by Saturnus View Post
In regards to circuit lay-out, I'll get back with a more detailed analysis.
I appreciate you taking the time to do this. I'll try to tweak the layout image to be a bit more clear.
  Reply With Quote
Old 28th February 2014, 09:07 AM   #16
diyAudio Member
 
Saturnus's Avatar
 
Join Date: Jun 2005
Location: Copenhagen, Denmark
1) Ground planes. There's such a thing as too much of a good thing can be bad, and in regards to ground planes this is the case. What's important is to realize there are two (three) separate ground planes that should not be mixed together. There's the PGND which essentially is all the connections to GND from the chip outputs, PVCC decoupling, and the GND connection from the power source. And then there the AGND which is all signal and logic ground connections as well as separate AVCC decoupling if used. The third ground plane is the bottom ground plane which is often seen and used as PGND. Ground planes must be starred to the chip pad and AGND and PGND should only be connected in one place. Usually through PIN 4 to chip pad. There's a fourth and fifth ground plane if the CRC are ground referenced. These should be connected by separate ground connections for each channel to the star ground.

1a) Connect GNDs of PIN 17, 20, 21, and 24 to chip pad. Not to anywhere else.
1b) Decouple AVCC separately to AGND with 2 ceramic capacitor identical to those after the bulk cap on PVCC
1c) AM1, AM2, AM3 and MUTE should be ground connected through PIN 4, not directly to chip pad.
1d) Negative inputs must be grounded close to input terminals unless you use differential (balanced) inputs. Otherwise you will have no sound.

2) Output section.

2a) The ferrite beads are inductors so they should be paired as close together as possible so that any stray RF noise radiated are negated by the opposite radiation of the opposite rail. There should be no ground plane or any other connection running directly below the ferrite beads on the same side of the board at least but preferably and if possible not on either side.
2b) Bootstrap capacitors must be as close to the chip as possible and should be rated to at least 4 times the supply voltage, and preferably 10 times or more. They must be ceramic and to achieve the lowest possible ESL use 1210 or 0805 sizes. Do not use 1206 types.
2c) The CRC section should be close to the output terminals. There are many advantages to be had if it is not ground referenced but instead referenced directly to the opposite rail, just remember that the voltage rating has to be doubled. If a ground reference is used, make a separate connection directly to the star ground on the ground plane side. Avoid using the PGND or ground plane if possible.

2d) Don't know why you have 2 RCs filters on either side of the ferrite beads. Drop the one closest to the chip.

3) Ferrite beads on power connection? Why?

Last edited by Saturnus; 28th February 2014 at 09:27 AM.
  Reply With Quote
Old 28th February 2014, 11:54 AM   #17
rosvall is offline rosvall  Denmark
diyAudio Member
 
Join Date: Dec 2009
Quote:
Originally Posted by Saturnus View Post
1) Ground planes. There's such a thing as too much of a good thing can be bad, and in regards to ground planes this is the case. What's important is to realize there are two (three) separate ground planes that should not be mixed together. There's the PGND which essentially is all the connections to GND from the chip outputs, PVCC decoupling, and the GND connection from the power source. And then there the AGND which is all signal and logic ground connections as well as separate AVCC decoupling if used. The third ground plane is the bottom ground plane which is often seen and used as PGND. Ground planes must be starred to the chip pad and AGND and PGND should only be connected in one place. Usually through PIN 4 to chip pad.

[...]

1b) Decouple AVCC separately to AGND with 2 ceramic capacitor identical to those after the bulk cap on PVCC
Ordinarily I'd agree with you, but the datasheet doesn't really talk about an analog ground. Their eval board doesn't use split ground (or power) either (as you can see i've taken quite a bit of inspiration from that board). At this point I'm not sure if pin 4 really is AGND or it's a error in the datasheet or what. I think i'm going to hit up TI and ask them what's going on.

I did initially split AVcc off and decouple that separately, before i found the eval board. Then i just thought **** it, if they can pull that off, so can i. Still, if it would improve the SNR or whatever in any significant way, sure, i'll change it.

Quote:
Originally Posted by Saturnus View Post
There's a fourth and fifth ground plane if the CRC are ground referenced. These should be connected by separate ground connections for each channel to the star ground.

[...]

2c) The CRC section should be close to the output terminals. There are many advantages to be had if it is not ground referenced but instead referenced directly to the opposite rail, just remember that the voltage rating has to be doubled. If a ground reference is used, make a separate connection directly to the star ground on the ground plane side. Avoid using the PGND or ground plane if possible.
That makes sense. But i guess the bigger issue is that i don't really know what it is i'm trying to fix with that (C)RC-snubber. Where is that energy, spectrum-wise, and how much is common-mode? I should probably read up on this stuff.


Quote:
Originally Posted by Saturnus View Post
1a) Connect GNDs of PIN 17, 20, 21, and 24 to chip pad. Not to anywhere else.
And route the return path of the output filtering through the bottom?

Quote:
Originally Posted by Saturnus View Post
1c) AM1, AM2, AM3 and MUTE should be ground connected through PIN 4, not directly to chip pad.
I get that that is the right way, but they're digital inputs and connected with very low impedance to (the supposed ) AGND pin.

Quote:
Originally Posted by Saturnus View Post
1d) Negative inputs must be grounded close to input terminals unless you use differential (balanced) inputs. Otherwise you will have no sound.
Whoops. I'm adding a 5th pin for GND.

Quote:
Originally Posted by Saturnus View Post
2a) The ferrite beads are inductors so they should be paired as close together as possible so that any stray RF noise radiated are negated by the opposite radiation of the opposite rail.
That makes sense. But I can't see a good way to do that without messing up the return path for the positive output filters.

Quote:
Originally Posted by Saturnus View Post
There should be no ground plane or any other connection running directly below the ferrite beads on the same side of the board at least but preferably and if possible not on either side.
That i can fix.

Quote:
Originally Posted by Saturnus View Post
2b) Bootstrap capacitors must be as close to the chip as possible and should be rated to at least 4 times the supply voltage, and preferably 10 times or more. They must be ceramic and to achieve the lowest possible ESL use 1210 or 0805 sizes. Do not use 1206 types.
All passives are 0805. It would be a lot neater with 0603, but those aren't compatible with my caffeine intake.

Quote:
Originally Posted by Saturnus View Post
2d) Don't know why you have 2 RCs filters on either side of the ferrite beads. Drop the one closest to the chip.
Copied it from the eval board. The eval board has the nice property of being FCC part 15 compliant. Yes, what i'm doing is entirely cargo cult - i don't know **** about EMC compliance, i don't even have a spectrum analyzer. I just figured, what the hell, if it can dissipate some ringing or whatnot, great.

Quote:
Originally Posted by Saturnus View Post
3) Ferrite beads on power connection? Why?
My reasoning is basically just more ferrite = less EMI. Might as well try to nip the problem of a radiating power supply cable in the butt.

I apologize for being a bit contrarian and ignorant, i know it's a frustrating combination. I do appreciate your help though.
  Reply With Quote
Old 28th February 2014, 12:37 PM   #18
diyAudio Member
 
Saturnus's Avatar
 
Join Date: Jun 2005
Location: Copenhagen, Denmark
Hey. You don't have to take my advise I'm just a perfectionist. Please note that evaluation boards are just that. Boards to demonstrate the function of the chip and a reference for designers. They are never meant as being the only and final implementation, and there's many things that can be done a lot better.

Quote:
Originally Posted by rosvall View Post
That makes sense. But i guess the bigger issue is that i don't really know what it is i'm trying to fix with that (C)RC-snubber. Where is that energy, spectrum-wise, and how much is common-mode? I should probably read up on this stuff.

And route the return path of the output filtering through the bottom?

That makes sense. But I can't see a good way to do that without messing up the return path for the positive output filters.
It's for EMI suppression in general, more specifically the first C works in combination with the ferrite bead to from a 2-pole filter in the FM frequency range. The RC part works at the switching frequency (and in the AM frequency range) by reducing overshots when the output transistors turn on and off. None of them should be common mode, if anything they are differential, which is why they can be referenced the the opposite rail instead of ground.

Referring to the opposite rail also eliminates 3 components, ie. you only need one CRC node instead of two. And eliminates the need for the return ground connection as well.

Quote:
Originally Posted by rosvall View Post
All passives are 0805. It would be a lot neater with 0603, but those aren't compatible with my caffeine intake.
It's the psychical shape, not size, that dominates how much ESL an SMD capacitor has so naturally 0603 types would be just as bad as 1206 types (well, almost). Don't think you can get bootstrap caps in less than 1210 size if the advise of 10 times supply voltage rating is followed.

Quote:
Originally Posted by rosvall View Post
My reasoning is basically just more ferrite = less EMI. Might as well try to nip the problem of a radiating power supply cable in the butt.
Adding resistance, even very little, to the power supply line is definitely not a good idea. Trust that your power supply can supply clean power, or fix that. Don't mess with the power inputs.

Quote:
Originally Posted by rosvall View Post
I get that that is the right way, but they're digital inputs and connected with very low impedance to (the supposed ) AGND pin.
Still not a good reason to cut corners. But sure the AMs can be connected directly to the chip pad. The MUTE pin should not though.

Last edited by Saturnus; 28th February 2014 at 12:46 PM.
  Reply With Quote
Old 28th February 2014, 02:47 PM   #19
rosvall is offline rosvall  Denmark
diyAudio Member
 
Join Date: Dec 2009
Quote:
Originally Posted by Saturnus View Post
Hey. You don't have to take my advise I'm just a perfectionist. Please note that evaluation boards are just that. Boards to demonstrate the function of the chip and a reference for designers. They are never meant as being the only and final implementation, and there's many things that can be done a lot better.
I do want to get the most out of this chip. And i do want to do things the right way. It's just that most design choices are compromises. Slicing up the top ground pour will invariably result in worse thermal performance. But if it results in noticeably better performance in some other way i'm good with that.

Quote:
Originally Posted by Saturnus View Post
It's for EMI suppression in general, more specifically the first C works in combination with the ferrite bead to from a 2-pole filter in the FM frequency range. The RC part works at the switching frequency (and in the AM frequency range) by reducing overshots when the output transistors turn on and off. None of them should be common mode, if anything they are differential, which is why they can be referenced the the opposite rail instead of ground.

Referring to the opposite rail also eliminates 3 components, ie. you only need one CRC node instead of two. And eliminates the need for the return ground connection as well.
The BD-modulation scheme, with both outputs switching in the same direction at the same time ought to generate some amount of common-mode noise.

Quote:
Originally Posted by Saturnus View Post
It's the psychical shape, not size, that dominates how much ESL an SMD capacitor has so naturally 0603 types would be just as bad as 1206 types (well, almost). Don't think you can get bootstrap caps in less than 1210 size if the advise of 10 times supply voltage rating is followed.
Ok, i get it, but why the big deviation from the datasheet? Faster rise time? Illuminate me.

Quote:
Originally Posted by Saturnus View Post
Adding resistance, even very little, to the power supply line is definitely not a good idea. Trust that your power supply can supply clean power, or fix that. Don't mess with the power inputs.
It's coupling switching noise (from the amp) back into the power supply cable i'm worried about. Also, these ferrite beads have <4mOhm of DC resistance.

Quote:
Originally Posted by Saturnus View Post
Still not a good reason to cut corners. But sure the AMs can be connected directly to the chip pad. The MUTE pin should not though.
They're digital inputs with hysteresis. I don't get it. What sort of problem is going to arise?
  Reply With Quote
Old 28th February 2014, 03:10 PM   #20
diyAudio Member
 
Saturnus's Avatar
 
Join Date: Jun 2005
Location: Copenhagen, Denmark
Quote:
Originally Posted by rosvall View Post
The BD-modulation scheme, with both outputs switching in the same direction at the same time ought to generate some amount of common-mode noise.
Enough to necessitate using 3 extra components and a difficult to optimally route ground connection. Not in my opinion but yours may vary.

Quote:
Originally Posted by rosvall View Post
Ok, i get it, but why the big deviation from the datasheet? Faster rise time? Illuminate me.
Ceramic capacitor are not very linear nor noise free when voltages near their rated voltage. You should always use ceramic capacitor with 10 times (4 times minimum) the voltage rating required in every case where the capacitor is in the direct signal path (bootstrap capacitors are in the direct output signal path).

Quote:
Originally Posted by rosvall View Post
It's coupling switching noise (from the amp) back into the power supply cable i'm worried about. Also, these ferrite beads have <4mOhm of DC resistance.
If it's a problem for you use external ferrite beads. Not on-board.

Quote:
Originally Posted by rosvall View Post
They're digital inputs with hysteresis. I don't get it. What sort of problem is going to arise?
Probably none but it is still good practice to keep something that is referenced to a specific rail also to be ground referenced to the same.

I also recommend using the FAULTZ pull-up connection of MUTE as described in the data sheet. Although the data sheet is completely wrong in how it's actually done. If done like the data sheet suggests it will work, and will likely damage the chip. Do it as it's done in the eval board instead.
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
How to connect PSU board to amp board? emerth Power Supplies 6 17th June 2012 01:35 PM
HIFI 700W Subwoofer Mono Amplifier Board By 10 Pairs 1943/5200 Amp Board For Subwoofe nelnar Solid State 1 4th June 2012 01:20 AM
Building the TSE board upside down Alan Hope Tubelab 8 22nd September 2011 02:34 AM
FS- Twisted Pear Buffalo 32S Board &amp; System New &amp; Unused secretriches Swap Meet 1 10th August 2009 02:17 PM
SMPS &amp; tube pre-amp development board. ianl Tubes / Valves 2 10th April 2006 06:05 PM


New To Site? Need Help?

All times are GMT. The time now is 11:30 AM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2