This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

TPA3125D2 instability / oscillation

Other Parts Discussed in Thread: TPA3125D2

Hi,

 

I am working with the TPA 3125D2 class D amplifier IC.  I am having a difficult time getting the circuit to operate well.   I have worked with a lot of audio amps over the years, but this is the first class D.  The circuit is based on the Evaluation PCB, and mono / BTL configuration.

 

There is a [ approximately ] 40KHz oscillation that I have yet to be able to find the cause of.  It shows up as distortion of course.  After building a prototype, everything looked ok, so we built 100.  Some just have a low constant 40KHz, some are high enough to cause the output components to become warm. 

 

I have tried re wiring the grounding a few different ways so far, nothing seems to have much effect.  Even with the inputs disconnected and terminated.

 

Thank you,

Dave

  • Hi Dave,

    Is it possible that the oscillation is coming from the previous stage feeding into TPA3125D2? Do you have the speaker load connected? What is your speaker load impedance? I can take a look at your schematic if you post it.

     

    Best Regards,

    Paul Chen

    Audio Applications

    Dallas, TX USA 

  • Hi Paul,

     

    I have the 2 inputs connected only to a capacitor, then a 4K resistor to GND at this time, to isolate any possibility of the previous stage causing the problem.  An 8 ohm test resistor is connected.  I also have the Audio Precision connected, with 500 ohms  resistors on each lead [balanced] to isolate the cable from the amplifier.

    As I mentioned, all of the other circuitry on the input side is disconnected right now.

    Schematic:

    0728.J-324 Rev 00.pdf

     

     

    Thank you,

    Dave

     

  • I forgot to add - The schematic has one error, that is fixed.  The AVCC pins are connected to the +24V supply.

    I have also found that if I disconnect the 10ohm / 1.5nF snubbers, the amp will come up stable, but when I even momentarily touch one of them back to connected, the oscillation starts, and won't stop.

  • Hi David,

    Usually it is required to have 1nF high freq decoupling caps. on the AVCC, PVCCL and PVCCR supplies (need to be placed really close to the device).  Without those high freq decoupling caps you might run into issues. Also you might want to use 50V 1uF for C8 and C27.

     

    Best Reg,

    Paul Chen

    Audio Apps

    Dallas, TX USA.

  • Hi Dave,

    Frank had asked me to look at this, too.  First question is where is the AVCC, PVCC coming from?  Is it a switching supply?  As Paul mentioned, power supply decoupling is important.   Have you looked at the noise on the power supply? 

    Also, is this on a pcb, or hand-wired?  You mentioned something about re-wiring the grounding, so that leads me to believe this is hand wired, and as such, this will not work.  Page 18 of the datasheet describes grounding, and connecting the GNDs to the thermal pad, which then is soldered to the IC at assembly.  

    If this is a pcb, would you send the layout please?   And 'scope captures of what you are seeing, as well as the power supply, AC component.

    -Leonard

  • Dave,

    I second what Leonard says, if you're using one of those white protoboard things, you're never going to get this to work. The high switching speed coupled with high current will kill you every time... That's a big difference between class-AB and -D!

    It might be useful if you could attach a screen shot of the 40 kHz oscillation as well.

    -d2

  • Ok, I'll get some scope pictures & post the layout. 

     

    It is built on a 4 layer PCB.   We have 100 of them :(   . 

    No switch mode power supply, just DC from a linear benchtop supply.  I wouldn't even try to use a plug in proto board for a switch mode / class D anything.

     

    The oscillation is has a couple of "states".  One is fairly low p-p voltage, looks like a sawtooth.  The other is much bigger, sine wave

    there are 1uF ceramic SMT caps near all the power pins.  Do they still need 100nF or 1nF also?

     

    For clarity,  the suggestion for C8 & C27 is to go from 25 to 50V?  [they are 1uFalready]

     

    Some of the "rewiring" I've tried is things like getting the caps closer and shortening the ground routing, tying them into different points.  I have seen cases where current in the ground routing shows up as a signal to the input.

     

    Thank you,

    Dave

     

     

     

     

  • The input is terminated, blocking caps & 4K to GND.

     

    The bottom trace is a scope probe directly on the + power rail and scope is 2.0V/div. [it's a non Textronix probe, so the display thinks it's 1:1]

    The middle trace is the output.  About 50mV BTL across the 8ohm test load.  The same waveform is on each output [ L & R ] referenced to GND, it is 8V P-P.

    The top trace is the distortion analyzer output.  Ignore it. 

    The "fuzz" on the sine wave, and the bottom trace is the class D switcher fundamental / ripple.

     

    Thank you,

    Dave

     

     

  • LeonardEllis said:

     

    Page 18 of the datasheet describes grounding, and connecting the GNDs to the thermal pad, which then is soldered to the IC at assembly. 

     

    I noticed that in the data sheet.  But there is no pad on the IC itself.  It is a 20pin DIP.

    ???

     

     

  • Hi Dave,

    Yes, the high freq caps (1nF) are needed as shown in the EVM. They must be placed within 1mm of IC. Your decoupling caps C22, C8 and C27 (1uF) has very long ground trace which decreases the their effectiveness due to the trace parasitic inductance. Yes, it is better to use 50V ratings (instead of 25V) for the cerm decoupling caps since the supply is 24V. This will prevent reliability issues and also at rated voltage, the capacitiance can decrease by as much as 80%.  

    Best Reg,

    Paul Chen.

    PCBlyt-hmnt-audio+EMC+T-100423.ppt
  • I added 1nF caps to the existing PCB, soldered directly to the pins, but it made no noticeable difference.

    Today is a short day, I'll be back at this Monday.Thank you,

    Dave

     

  • I also built this "dead bug" style to eliminate PCB routing issues.  I get the same 40KHz oscillation.  This one uses Tantalum caps.  I will add the 1nF ceramics, and check again.

     

    Thank you,

    Dave

     

  • Hi Dave,

      I'm not surprised this does not work.  Let's go back to the pcb version.  You stated that AVCC was connected to +24V.  Is it connected directly to your +24V power supply, or to the filtered PVCCR node? 

    If you look at the EVM design, the PVCCR is derived through a ferrite bead (you also have one) with a 1uF and 0.1uF caps at pin 10.  It then goes to pins 16 and 17 with a 10uF cap and another 0.1uF cap.  On your layout, I see only a 1uF on pins 16 and 17, and a 1uF at pin 10.  (see http://www.ti.com/litv/pdf/slou250 ).  

    Do you have an EVM?  If you make the same setup and measurements, I'm wondering if you will see the same 40kHz?  There could well be something in the power supply, measurement environment, etc that could be inducing this oscillation.  On your pcb, please look at the AVCC pin with the scope, looking for this frequency, then add the caps, match the EVM configuration, take the measurements again.

    -Leonard

     

  • Hi Leonard,

     

    The "dead bug" version, I used the simple schematic from the data sheet.  Routed the wiring to keep powers & grounds from interfering with each other, based on my experience with audio and switch mode power supplies.   I needed to try something.  It's not surprising it doesn't work, but it is that it's the same [very similar anyway]  as the PCB.

     

    I found the information on the 1uF capacitors we have, and they are only about 20% lower capacitance at full working voltage compared to half working voltage.  We will be changing the spec on those for this and other designs.

     

    This is about our PCB:

    It is based on the EVA board schematic.

    The AVCC comes from C7 on our schematic.  The PVCCR & L each have their ferrite beads, and caps.

    The schematic for the EVAL board shows 1nF = 1000pF caps across the 1uF caps on those pins, not 100nf  = .1uF caps.  I am uncertain on the correct value now

    We had an EVM, but it has gone missing, and I ordered another this morning.

    I have moved from testing on the production test area to my engineering area, so everything is different equipment - wise.

     

  • I added the 1nF caps to the dead bug circuit.  It will power up stable.  If I touch the signal generator outputs to the inputs of the amp, it begins the 40KHz oscillation.

    Is there a suggested driver impedance for the input of this amp?

     

     

     

  • Thanks for the additional info and description, very helpful.

    I would suggest you change the AVCC connection from C7, as this is unfiltered, to the PVCCR pin, as is on the EVM; alternatively, add the same filter network (FB + 2 caps) to the AVCC connection.  

    As for the cap value, conversion error on my part . . yes, 1nF as shown. 

    Did you see this on the EVM when you had it?  Or perhaps had not looked at it at the time.  EVM are in stock, so should be there to you soon.

    -Leonard

     

  • I added a ferrite bead to the AVCC feed.  The caps are already there.  The oscillation is about 2VPP now.  

     

    I have found that if I hold a 1uF stacked film cap [with 1" leads even] across pin1 - pin 20, the oscillation stops.  If I do the same with one of the 1uF ceramic caps, with maybe .4" of leads, it only lowers the amplitude a little. 

    Doing the same with pin 10 - 11 has little effect.

     

  • Another update:

     

    I have added leaded capacitor, soldered directly to the power pins.   A 1uF stacked metal film, and a 1nF mono, on each of the pins PVCCL - PGNDL and PVCCR - PGNDR.  I also had to run a connection from pin 11 to 20 using .075" wide solder wick - 26 AWG wire wasn't enough. 

    This makes me wonder - could the thermal breaks on the inner layers be contributing to the instability?

    The AVCC pins also gets a 1nF mono to the middle of that added GND bus. And it has an 80 ohm bead between the AVCC & caps. and the +24V rail.

    I tried grounding that 1nF cap to the AGND pins, and also a 1uF to either GND, but none of that seemed to help.

    I have 2 boards with all these modifications.

    I have reconnected the input stage, so I can run signal through.  I'm using a 1KHz amplitude sweep, to see what happens from idle to full output [limited to about .5 to 1 Watt by the diodes]

    One seems to be ok.

    The other still breaks into the 40KHz oscillation but only when the audio signal at the output gets above 0.8 VRMS. 

     

  • Another attempt to get this thing stable.  Added 1nF and 1uF ceramics on the solder side.  And a piece of copper to tie all the caps and GND pins together.  I also removed the 220nF through hole BS caps [and the traces] and used 220nF ceramics right on the pins.  This lowered the THD a bit on one of the other boards I have been experimenting on.  This board is still oscillating, with these modifications.

    If I add on the 2 film caps, as described in the previous post, it behaves like the other 2 boards.   They all begin oscillating at about 40KHz when the 1KHz test signal rises to the point that the output is a little over 1.5VRMS.

    One little update... If I tack a 47uF tantalum across pin 1-20 the instability is gone.  Hopefully there are some clues in all this.  I should have the eval board thursday, when I can work on this again.

  • David,

    One thing I noticed on your layout, and assuming you have all the connection for power through the 2 pins at the edge of the board, you have a large GND plane, but the connections to these pins is with two very thin traces.  This is going to act more like an inductor, and really needs to be a much larger path to create an effective GND.  It's like having a 6-inch fire hose with a 1/4-inch valve at the end of it.  I suggest you scrape away the solder mask, add copper braid and solder to these two GND pin connections.

    -Leonard

     

  • Update:

    I used .075" braid for the GND pins.   This is a 4 layer PCB.  the system GND is one of the inner layers.  All 4 GND pins of the IC are connected to it, but have thermal reliefs.  The copper & braid all tie them together now.  Caps on the 2 main VCC pins on the bottom: 1nF cerm, 1uF cerm, 4.7uF Tant.

    Added caps on the top:  4.7uF Mono.  This still goes unstable when the output voltage is around 2.0 / 2.1 VRMS. 

     

     

  • Hi Dave,

      The addition of the GND and braid at the IC, I don't think will change anything.  The GND plane in this area, and on the board in general, looks good.  What my comment/concern was about is at the connector, where there is one wire (maybe two - I can't see from the pic) trying to extract all this ground return noise back to the power supply/earth ground.  There is such a small etch connecting the massive (relative) GND plane to that one wire, so there is a restriction created. 

    If instead, you took the braid and routed it from the connector pins to one or more GND vias, or even this GND plane you created, thereby bypassing this small etch connection from the plane to the pin.  I don't know if this will do the trick, but it's worth a try, and it is a weakness in the layout I see.  

    We are also looking at the possibility of the output filter having a resonance at 40kHz, and being coupled back to the input; again, another idea of why this might be happening . . . . 

    Have you received the new EVM yet?  And from what you recall, this 40kHz did not occur on the first EVM you had, correct? 

    -Leonard  

     

  • Hi Leonard,

     

    In the blurry picture, the edge of the PCB looks like a trace - it is bizarre it looks so much like a trace - but it is not a trace.  The ground to the power supply comes into the inner layer plane though a pin on the modular phone jack near the center of the PCB.  The cable that powers this unit is about 10' long, and AWG26 conductors.  I may need more filter caps on the incoming power?

     

    I just tested the EVM, and it has way lower THD, and no trace of the oscillation.  Of course.  I will certainly be redoing the PCB, using the EVM as a guide.  [I didn't do the artwork for the PCB I'm fighting with.]  There are definitely things on it that I wouldn't have done.  I've been hoping to find a way to make the existing boards usable, and also, knowing what to do for the new revision, so I know it will work.

     

  • Dave, For the GND connection I was referring to, it is the one at the top edge of the pcb, labeled Gnd, next to the +12 and +24 pins. I'm assuming this is to the power supply, and this would be the primary path for all the GND returns.  Since the etch to this pin is so small, I'm thinking it is not helping this problem at all.  I had not even considered the RJ45 connection.

    How long is the cable to the power supply?  Is the GND on the power supply floating, or tied to building/earth GND?

    -L

     

  • David,

    Try changing your 0.68uF filter caps to 0.33uF.  Leave the 22uH inductors as they are.  Driving a BTL load with 2 single-ended channels is a little more senitive to your output filter parameters.  In my experience, moving the LC filter pole frequency out a little can help a lot.

    Best Regards,

    Ryan

  • LeonardEllis said:

    Dave, For the GND connection I was referring to, it is the one at the top edge of the pcb, labeled Gnd, next to the +12 and +24 pins. I'm assuming this is to the power supply, and this would be the primary path for all the GND returns.  Since the etch to this pin is so small, I'm thinking it is not helping this problem at all.  I had not even considered the RJ45 connection.

    How long is the cable to the power supply?  Is the GND on the power supply floating, or tied to building/earth GND?

    -L

     

    I am confused....  Along the top edge, there are 2 pads labeled "GND" that are connected to the inner plane layer.  The +24 pad has a long thin trace, but these pads are only used for measuring the voltage on the supply rails during production - if troubleshooting is required. 

    These units are powered from one of 2 sources depending on customer / site details.   One is a local wall wart power supply, which is not usually a grounded device.   The wire between the power source and the PCB would be a ten foot AWG#26 telephone style cable.  The type that goes from a phone to the wall jack, except ours have 4 or 6 conductors.

    The other power option, is backroom power, which can be more than 100 feet of #26 CAT5 cable plus the 10' station cord.  Usually, the power source is grounded in this case.

    I should also add, the audio passband of this project is closer to telephone grade than high fidelity.  Since the speaker can't really make any sound below 100Hz, I use the DC blocking caps to roll off the low frequency response.   The power supply does not have to support large bass transients.  We are not trying to get the full output power this IC is capable of.  The most we would ever want with this design is 1 or 2 watts.

    Thank you,

    Dave

     

    P.S.  I am going to try the different filter caps now.

  • Ryan Lind said:

    David,

    Try changing your 0.68uF filter caps to 0.33uF.  Leave the 22uH inductors as they are.  Driving a BTL load with 2 single-ended channels is a little more senitive to your output filter parameters.  In my experience, moving the LC filter pole frequency out a little can help a lot.

    Best Regards,

    Ryan

    This has made a huge difference.  I still need to add 4.7uF 50V ceramic caps to the power pins to make it work, but we can live with that for this build.  We happen to have a bunch of them left over from another project. 

     

    I will be working on a new PCB layout now, so a lot of the layout related trouble will be fixed.

    Thank you,

    Dave

     

  • I just noticed on the Eval board schematic, it shows C4 as a 1uF 16V.  Which is biased by the PVCC rail, which can be as high as 26V.

  • We have new PC boards.  With the ceramic caps on the solder side, under the IC.  And better  [shorter] routs for all the wiring.

    I still had to resort to using 10uF ceramic caps for the 2 main filter / supply / bypass caps, rather than the 1uF used in the evaluation board. 

    With the 1uF caps, I get about a 1VRMS 50KHz sine wave on the outputs.  Add a second 1uF cap, and I only have the switching fundamental. 

    Figuring 1+1=2, I also tried using 2.2uF caps, but the 50KHz was still there.  

    Going to 10uF gets rid of it.