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.

TPS552882-Q1: Schematic Review - 12V Output buck boost

Part Number: TPS552882-Q1
Other Parts Discussed in Thread: TPS552882, TPS55288, , TPS55288-Q1

Hi, I have a schematic based on a webench solution which I have modified slightly  and I just want to check if everything looks ok. It is for 6-36V input with a 12v 6A output.

1 question I have is about the input and output capacitors. Are the large aluminium capacitors necessary? I saw on the datasheet that they don't put them in the example application but they are added on webench. I have this as this power feed which supplies the VIN input to this circuit:

It already has a large 220uF capacitor. Can I change the aluminum ones on my buck-boost?

Thanks all!

  • Hi Matthew,

    Thanks for reaching out. 

    1. May I know what is the product type and application here?

    2. Does the device need to operate at 36Vin? Because the max recommended operation voltage is 36V for this device.

    3. What is the part number of the output capacitors? The ESR and effective capacitance is needed to calculate the compensation. You can also use the calculation tool on product page for that.

    4. The input and output capacitors are decided by the voltage ripple and undershoot/overshoot voltage during transient. Is the VOUT of LTC4368 far away from TPS552882 input side? If so, recommend to populate the aluminum capacitors at the input side.

    BRs,

    Bryce

  • Hi Bryce

    1. This is for an automotive grade BMS to modify the 6-36V input to a solid 36V output.

    2. It does need to operate at 36V but I expect it never will be operated that high in reality. The VIN to this will be shut off at 36.5V

    3. C20: 12101C475K4T2A C21: EEE-FK1J221AV C72-C74: GCM32EC71E226KE36K C69-C71: EEHZA1E560V

    4. The next 2 pictures will show the layout so far and the voltage path. LTC is labelled as 1 and TPS is labelled as 2:


    Thank you!

  • Hi Matthew,

    Thanks for reaching out.

    1. It this a typo? Because this device can't support that high output voltage.

    solid 36V output.

    2. The max recommended input voltage is 36V, so if the operation Vin is higher than that, it is not recommended and guaranteed.

    3. I think the input capacitors C63 and C64 can be replaced with 10uF ceramic capacitors since the 220uF cap is close to the input side.

    4. Recommend to add RC snubbers at both SW1 and SW2 pins.

    5. Recommend to add 10nF at DITH pin to enable dithering function for better EMI.

    6. Recommend to change R63 to 22k to set the average current limit to 15A to leave some margin.

    7. To enable output current limit, you will need to add the sense resistor at the output side and connect to ISP, ISN pins. See User's Guide for more details.

    8. Strongly recommend follow the layout guideline. www.ti.com/lit/an/slvaer0b/slvaer0b.pdf

    9. Recommend to choose another MOS with smaller Ciss and smaller tr/toff.

    BRs,

    Bryce

  • Hello,

    1. Yep sorry, was meant to say 12v output!
    2. That's ok, 36 is the limit on my board, any more is a fault cause and therefore this will be protected upstream
    3. Ok so 4 x 10uF overall? Or go to more than 4?
    4. Where would you put this? between the Sw pin and pin 2 of the capacitor shown in the schematic?
    5. Ok, thank you
    6. Ok, will do
    7. I have current limit elsewhere, I was planning on skipping this?
    8. I have the following layout at the moment. I started with the layout guide and it is only the output that goes off in a different angle, does this look ok?
    9. What is a MOS? is that refering to a MOSFET? If so, which one should I change? These were the TI suggested ones on webench.

    Thank you for the help, much appreciated!

  • Hi Matthew,

    Please see my follow up comments below.

    1. Ok so 4 x 10uF overall? Or go to more than 4?

    -> I think 4pcs is ok.

    2. Where would you put this? between the Sw pin and pin 2 of the capacitor shown in the schematic?

    -> See below for example.

    3. I have current limit elsewhere, I was planning on skipping this?

    -> It's ok.

    4. I have the following layout at the moment. I started with the layout guide and it is only the output that goes off in a different angle, does this look ok?

    -> The output capacitor is very important for Boost mode, can you share the pictures for each layer?

    5. What is a MOS? is that refering to a MOSFET? If so, which one should I change? These were the TI suggested ones on webench.

    -> It refers to Buck side MOSFETs, it's ok but would be better if you have better choice with smaller tr/toff.

    BRs,

    Bryce

  • Hi Bryce,

    1. Ok, will change, thank you.
    2. Ok will add. I assume I still use the 16V rated caps like webench uses for the outout? On that note, shouldn't all the caps connected to VOUT be 25V rated caps to be double to voltage?
    3. Ok will ignore, thanks
    4. Here is the transparent view and an individual view of all 4 layers. Just the serperated AGND on L3 and MOSFET gate, VIN for pin 3 and output to LED on L4. GND on L2.




    5. Would this choice be better: changing both MOSFET to the same PN and going for IAUC41N06S5L100? Should they be different as I saw on yours that they are the same?

    Thank you!

  • Hi Matthew,

    2. Recommend to use 50V rating capacitors for RC snubbers because of the switching voltage spike.

    5. The IAUC41N06S5L100 looks better with smaller Tr/Tf and Qg.

    4. Here are my comments about the layout:

    (1) Put more GND copper plane and vias on L1, and put two more ceramic caps to decrease the buck switching loop.

    (2) Move the boot cap close to the pin out.

    (3) Put more GND copper plane on L1 layer and shorten the AGND trace to leave the space for Cout cap. Move the Cout cap as close to the Vout and GND pins as you can to decrease the boost switching loop.

            

    (4) Widen the VCC trace.

    (5) Recommend to put another Vout and GND plane at the bottom layer, and add one more 0402 0.1uF cap under the vias.

     

    (6) You can see more details in the layout guideline. www.ti.com/lit/an/slvaer0b/slvaer0b.pdf

    BRs,

    Bryce

  • Hi Bryce,

    Thank you for all the help. I think I have implemented everything you have saidf but there are still a couple of confusions on my part. I will attach the new layout and schematic below to help show you what I have done.

    1. The 2 extra ceramic caps on VIN, I have just made them 10uF like the other input caps should these be 0.1uF instead?
    2. The Infineon MOSFET can replace both MOSFET's? I have swapped both for now, please let me know if this is not ok!
    3. I am confused about the PGND and AGND loop tbh! The link you sent has them connected at the IC in 1 image and then seperated with a via on another so I am really not sure what this AGND loop should look like!
    4. Does having this close to my MCU present an issues? It is this far away:

    Here are my design files, I have all 4 layers, transparent view, 3D view and schematics. Thanks agains for the help! I think we are nearlly there!

     3D

     Tranp

     Top Layer

     L2 - GND

     L3 - Contains AGND

     Bottom layer

     Schematic

  • Hi Matthew,

    Please see my comments below,

    1. The 2 extra ceramic caps on VIN, I have just made them 10uF like the other input caps should these be 0.1uF instead?

    -> Recommend to add one more 0.1uF at the inner loop like below.

    2. The Infineon MOSFET can replace both MOSFET's? I have swapped both for now, please let me know if this is not ok!

    -> I think it's ok.

    3. I am confused about the PGND and AGND loop tbh! The link you sent has them connected at the IC in 1 image and then separated with a via on another so I am really not sure what this AGND loop should look like!

    -> The EVM use separate AGND for all signal pins and connect to PGND at VCC cap ground. The current connection is also ok for me, you can widen the AGND trace at the L3 layer.

    4. Does having this close to my MCU present an issues? It is this far away:

    -> It think it's ok if the ground is clear for the MCU.

    5. Recommend to use 20mil for SW1 trace and DR1L, DR1H trace.

    BRs,

    Bryce

  • Hi Bryce,

    Great, thanks!

    I have made the few changes you just suggested.

    Just to check, this means having 7 input caps overall (6x10uF and 1x 0.1uF) is that right? is there a downside to this many caps?

    Also, is there anyway you could show me layer 3 of that AGND image? So I can see what is on your AGND path and how it's layed out please?

    Lastly, how can I change my schematic to be able to control the output of this with a MCU digital signal?

    Many thanks for the help!

  • Hi Matthew,

    1. I think the downside is the cost increases with more caps. From my point of view, 4*10uF+1*0.1uF is ok here. Keep C67, C68, C65, C66 which is close to the FETs.

    2. I can send you the file via personal message, please send the friendship request to me.

    3. You can choose I2C version TPS55288 to control the output voltage. The package is same, just pin5 and pin6 are different.

    BRs,

    Bryce

  • Hi Bryce,

    Great, I have removed 2 of the 10uF capacitors and sent you a friend request.

    The TPS55288 does not appear to be automotive grade, unfortunately this is a requirement of mine. Is it not possible to have an enable on the TPS552882? Maybe an example of this:

    Thanks!

  • Hi Matthew,

    Please check the file which I sent to you.

    TPS55288 has automotive version which is TPS55288-Q1. Sorry I thought you mean program the output voltage to different values. If you mean turn on or shutdown the device, this TPS552882-Q1 also has EN pin which I saw you connect to Vin through the resistor divider.

    BRs,

    Bryce

  • Hi Bryce,

    Yes I mean enabling and shutting down the device from the uC. So would putting a MOSFET in the middle of my voltage divider shown above work? Output off when mosfet is open and 12v on when mosfet is closed? 

    Can I confirm that the device current will be in the uA range when shutdown? 

    Thank you 

  • Hi Matthew,

    Yes, the above method is ok for this. And a simpler way is to use GPIO of the MCU to output high/low level voltage directly to EN pin. 

    The shutdown current is smaller than 10uA as datasheet marked.

    BRs,

    Bryce