• State TI Thinks Resolved
  • Locked Locked
  • Replies 10 replies
  • Answers 3 answers
  • Subscribers 30 subscribers
  • Views 480 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

TAS5825M: Heat Dissipation Issues With Custom Board

Alex Batts1
Prodigy 50 points
Part Number: TAS5825M

Hello,

I am currently working on a senior design product using the TAS5825M using a custom built board. The board will play music, and the most recent amplifier we tested lasted about a week playing music. However, the amplifier runs very hot. Running at 24 volts, the amplifier with the same address on the TAS525MEVM eval board was at a temperature where we could hold our finger on it when playing music and it was only slightly warm and didn't burn us. However, when running on our board, the amplifier was very hot. It burned our fingers almost immediately when we touched it with no heatsink, and then we added a couple Raspberry Pi heatsinks and it seemed to cool down some, but even then if we held our finger on there for too long it would start to burn. One difference is that our board is running in mono whereas the eval board runs in stereo. I don't know if the configuration would make any difference in heat dissipation, but I would think it shouldn't make a difference.

I can include a schematic if necessary. I don't know if there is any sort of current limiting resistor on the eval board that we are missing, but we followed the PBTL sample schematic in the datasheet exactly. We also did include a ground plane in our layout. 

I would tend to think that there wouldn't be a short because of the fact the amp was playing for almost a week with no issues besides being hotter than on the eval board. The setup we had going was that we had our computer connected to the purepath console motherboard, which then hooked up to the eval board. We then have individual I2C and I2S lines running from the eval board into our board, and our amp has the same address as one of the amps on the eval board. So the amp on our board should be programmed the exact same way as the amp on the eval board. When the board with a broken amp is hooked up like this to the purepath console motherboard, the system checks in purepath console fail. However, when our board is disconnected, the system checks work. 

We periodically checked the fault registers and never noticed any warnings/faults, including for overtemperature.

If there is anything that might be missing in the sample schematic for the datasheet that the eval board has, that would be good. Otherwise, if anyone has experienced this issue or knows of what the fix might be, it would much appreciated! As I've said, I can also include a sample schematic.

Thank you,

Alex

  • 0
    TI__Genius 14730 points

    Hello Alex,

    Can you provide the schematic and layout for your system. Also can you provide what your I2C initialization sequence is.

    Best Regards,

    Luis

  • 0 in reply to Luis Fernandes de Pina
    Prodigy 50 points

    Hello,

    Thank you for the response. I have attached a picture of the schematic. I can attach a screenshot of the layout if you need it. However, I am not sure how it would help in the same way the schematic would.

    The SDA, SCL and PDN pins all have pull up resistors attached although they are not shown (the TAS is on a board with other chips using I2C). 

    As for the I2C initialization sequence, it currently is the sequence coming from the purepath console motherboard.

    Thank you,

    Alex

  • 0 in reply to Alex Batts1
    TI__Genius 14730 points

    Hello Alex,

    I don't see clear issues with your schematic, could you provide the voltage rating of the decoupling caps, bootstrap caps, and the cap on the output just to be sure there isn't issues there.

    Can you provide the layout. Thermal performance definitely significantly related to the layout.

    Best Regards,

    Luis

  • 0 in reply to Luis Fernandes de Pina
    Prodigy 50 points

    Hello,

    All of the capacitors have a 50 V rating and all of them should have +/- 10% rating (except the large decoupling caps).

    Okay, I can provide some screenshots. It is a four layer board with a ground plane on layer two. Would you like 4 different screenshots with each layer emphasized? Or would you prefer something else?

    Thank you,

    Alex

  • 0 in reply to Alex Batts1
    TI__Genius 10190 points

    Alex,

    I think Gerber is best preferred(if possible) for Luis to review. if not, then please capture 4 screen shots with each layer.

    Dylan

  • 0 in reply to Dylan Yao
    Prodigy 50 points

    Here is a zip with the gerber files.

    Thank you,

    AlexPanda Stack.zip

  • 0 in reply to Alex Batts1
    TI__Genius 14730 points

    Hello Alex,

    I will review the gerbers and provide comments.

    Best Regards,

    Luis

  • 0 in reply to Luis Fernandes de Pina
    TI__Genius 14730 points

    Hello Alex,

    Looking at your layout i see a GND plane on 1 of your inner layer but i don't see any on the top and bottom. A big common GND plane on both top and bottom layer is recommended for this device and that could be affecting your thermal performance. We also recommend lots of vias to connect top and bottom layer so the heat can travel from top layer to bottom layer quickly.

    Additionally I had concerns on your output trace. What is your expected max output power, because your output trace is very thin/small and could be causing issue depending on your output power expected  I recommend looking at trace width calculator to see if your output traces are suitable for the peak current for your expected. https://www.4pcb.com/trace-width-calculator.html this link should be helpful in that regard.

    Best Regards,

    Luis

  • 0 in reply to Luis Fernandes de Pina
    Prodigy 50 points

    Hello,

    Thank you for the very helpful message! I was unaware that a top and bottom ground plane were recommended for the design. I will be sure to implement this in my next design! Since it is a four layer board and I already have a ground plane on layer 2, should I just put a ground plane on all 4 layers, or would it only be wise to use two?

    As for the output power, I believe we wanted it to be able to handle the maximum output power the amplifier. If this means that it is 70W output power, would the peak current be relative to the 24 V input, ie ~3 amps?

    Thank you again for all the help,

    Alex

  • 0 in reply to Alex Batts1
    TI__Genius 14730 points

    Hello Alex,

    I would probably put a GND copper pour on all your layers. Also if you are trying to output 70W I highly doubt your output traces are wide enough and surprised you only saw overheating compared to actually damaging the part, so I would recommend modifying your output traces.

    For calculate the total current i would back calculate from your peak output power, the current you get from that would be RMS current and you would need to calculate peak current to see if your new output traces can handle that current. You can also look at our layout on the TAS5825M User's guide for reference.

    Best regards,

    Luis