• State Resolved
  • Locked Locked
  • Replies 7 replies
  • Answers 1 answer
  • Subscribers 62 subscribers
  • Views 395 views
  • Users 0 members are here
Support feedback
Options
Options
Related

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.

TPS55289: TPS55289 works for few seconds than shorts external 5V

Noah Kramer
Prodigy 40 points

Part Number: TPS55289

Tool/software:

Good afternoon,

We use a TPS25730D in combination with a TPS55289 to create an USB C Power supply.
The USB side works fine and can consume upto 100W. 
The TPS55289 on seems to work fine in the beginning, but fails after a few seconds, under low load(< 10 W). After which the IC shorts the 5V rail with GND.

We use an exteral LDO (LM7805) as 5V power supply.

We've tried optimizing the PCB for great thermal efficenty, and used the datasheet for reference.

Does this problem sound familiair? Could somebody check our PCB/layout?

Thanks!

  • 0
    TI__Mastermind 29350 points

    Hi Noah,

    The layout looks very poor, to make the device operate well, a proper layout is needed. Compare with the layout example in datasheet, I don't think it followed the layout guideline in datasheet.

    For example, the VCC pin is used for internal control circuit and gate driver supply, but the trace is too thin and there is no cap close to VCC pin.

    And for input and output capacitors, there are no nearby capacitors close to Vin and Vout pins.

    Also for SW1, SW2 trace, there two pin carries high inductor current while the traces on pcb are too thin.

    Please strictly follow the layout guideline in the datasheet. And also attach the EVM example for your reference.

    7674.TPS55289 Layout Guide line.pdf

    You can share the layout files with us for review when you finished.

    BRs,

    Bryce

  • 0 in reply to Bryce Xun
    Prodigy 40 points

    Hi Bruce, thanks for your time!

    Weve updated the layout

    Kind regards,

    Noah

  • 0 in reply to Noah Kramer
    TI__Guru 69175 points

    Hello Noah,

    The expert is in public holiday. Please expect a detailed review next week.

    Best regards,
    Brigitte

  • 0 in reply to Noah Kramer
    TI__Mastermind 29350 points

    Hi Noah,

    Thanks for feedback, could you share your replies about the below questions. I will proceed the sch and layout review.

    1. What is the input voltage range, output voltage and max output current?

    2. What is the part number of the inductor?

    3. What is the ESR value and part number of the output capacitors?

    4. For the layout, it is not easy to read the pad of each capacitors, could you change the transparency of the copper to 60%, or can you upload the .pcb file here?

    BRs,

    Bryce

  • 0 in reply to Bryce Xun
    Prodigy 40 points

    Hi, thank you for responding!

    1. What is the input voltage range, output voltage and max output current?
    input voltage: 9-20V
    output voltage: the full range
    output current: the full range

    2. What is the part number of the inductor?
    nl.mouser.com/.../652-SRP1038WA-4R7M

    3. What is the ESR value and part number of the output capacitors?
    To be honest, I don't know exactly, as this buck-boost regulator is used for a test project and these capacitors are taken from the local stock, but they are of decent quality.

    I have included the PCB file.
    Thanks again!

    The PCB file, designed in Altium

    Combined_PCB (1).PcbDoc

  • +1 in reply to Noah Kramer
    TI__Mastermind 29350 points

    Hi Noah,

    The inductor looks ok.

    Depending on the output voltage range and the output current, and also the ESR and effective capacitance, the COMP parameters need to be checked. Or you can follow the below app note to check the stability or use the Frequency Response Analyzer to do the loop stability test. 

    Simplifying Stability Checks https://www.ti.com/lit/pdf/slva381

    For the layout:

    1. Recommend to add 0.1uF/0402 caps at Vin and Vout side, so the caps can be placed as close to Vin/Vout pins as possible.

    2. What is J3 used? If internal feedback is selected, then FB/INT pin can be used as fault indication and connect with VCC through 100k pull-up resistor.

    3. Add 3-4vias close to C10 GND pad.

    4. Recommend to leave EXTVCC pin floating, so it will need external 5V supply for internal LDO supply.

    5. Recommend to remove the GND trace beneath inductor.

      

    6. At bottom layer, recommend to move the Cin/Cout caps below, so the AGND trace can be routed as red trace.

    7. And recommend to use 0402 package for external signal pins' resistors and caps so the components can be placed closer to device.

    BRs,

    Bryce

  • 0 in reply to Bryce Xun
    Prodigy 40 points

    Hi Bryce,

    Thx for all your help!

    It works fine now.

    Kind regards,

    Noah