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.

TPS54394: Design feedback

Part Number: TPS54394

Hi,

Please could you give me some feedback on the following design.

TPS54394

1V1 @ 3A

1V5 @ 3A

Most parts have their ratings on the schematic.

L1 & L2 = ABRACON ASPI-6045T-2R2N-T

Here's the layout:

There are internal layers that are not shown, but these are solid GND pours. Should I relieve GND pours under the inductors? I've seen conflicting recommendations.

I've split the 5V inputs so they don't share the input capacitors, each input has it's own capacitors. Is that a good idea or should I just pour it all?

I would have liked the high frequency filter input capacitors closer to the input pins, but then they won't be connected to the top GND pour. Do they look ok where they are?

I'm a bit nervous about the width of the pour from the switching node, under the input caps, to the inductor. But I think this gives the best compromise? Thoughts?

Many thanks,

G

  • Hi

    Amod will reply you tomorrow!

    Shuai

  • Hi Graham,

    The schematic looks fine to me. 

    On the layout-

    1. You can have the VIN pour like you have done or just pour it all. Do you have separate VIN sources by any chance? Per your schematic looks like just one 5V source. In any case, adding here that VIN1 is always required for output 1 and output 2 to work. 

    2. Will need to check what the EVMs have done for the ground pours under inductors. You can follow the same.

    3. The input cap placement looks fine to me and follows datasheet guidelines. 

    4. SW node connection looks ok to me. This falls under "special considerations" in this app note: https://www.ti.com/lit/an/slyt614/slyt614.pdf#page=3 

    Thanks,

    Amod

  • Hi ,

    No, there isn't separate sources, just one 5V in. I was just attempting to separate the input capacitors.

    The design files do not seem to be available, but the user guide shows a split of two pours under the inductor, GND and the output voltage. I'm not sure that's the greatest idea?

    What is Ti's general recommendation for GND pours under inductors? I know of at-least one manufacturer that recommends solid pours, but the usual recommendation is no pour.

    Would you suggest adding snubber components? Could these be on the bottom of the layout? Are 0402 components sufficient for these?

    Are the diodes a good idea on the switching nodes?

    Many thanks,

    G

  • Hi Graham,

    Yes unfortunately I am unable to locate the design files on the EVM as well. I discussed internally on the ground pour under the inductor and consistently see ground pour being used under the inductor. Since you plan to use a shielded inductor, the magnetic field generated by the switching current will be mostly contained within the inductor package. It is true that you could induce small currents in the GND plane, but these would be local eddy currents and not affect the GND plane. I found an interesting article in support of having ground pour under inductor: https://resources.altium.com/p/should-ground-be-placed-below-inductors-switching-regulators 

    Snubber circuits can be used to reduce the electromagnetic interference (EMI) by slowing down the rise/fall times of the SW node and are completely optional unless you need to meet certain EMI requirements. The downside of having the snubber is reduction in efficiency due to increased switching losses. You can place the snubber RC on the top layer if you choose to use it. I have not seen diodes on the switch node - do you have a specific problem you are looking to solve with these?

    Thanks,

    Amod

  • Hi ,

    Thanks, I'll read through that.

    I have all the PSU components on the top layer, but am thinking about adding snubber parts on the bottom layer, I know that's not ideal, but if I put them on the top layer and don't fit them then that compromises the layout. What are your thoughts?

    The diodes are fit options on the evaluation board for this part, could you take a look and tell me what they are for and why they would be fitted?

    Thanks,

    G

  • Hi

    Amod will reply you next Monday!

    Shuai

  • Hi & ,

    Do you have any further feedback for me yet?

    Kind regards,

    G

  • Hi Graham,

    Agreed. If these are potentially optional components, you can place the snubber on the bottom layer. EVM does the same too when I just looked at it. The diode is optional too as the internal LSFET body diode is already present. But adding the Schottky diode will have a lower Vf than the body diode of the LS FET so it will boost efficiency by lowering the loss during the dead-time. Also, the Schottky diode will have low reverse recovery current (Qrr) so it can reduce the overshoot on the SW node when the HS FET turns on and provides the QRR. The lower Qrr also improves efficiency a little bit more. Again the snubber RC and diode are completely optional but can be used to help meet any EMI requirements you may have.

    Thanks,

    Amod

  • Hi ,

    Thanks for the reply.

    Are 0402 parts typically beefy enough for the snubber network? I know that the values would need testing, but would 0402 100nF 16V and 0402 2R2 parts be suitable as at least placeholders?

    Can you advise the ratings required for the schottky diode as there are no clues in the evaluation board document.

    Thanks,

    G

  • Hi Graham,

    Apologies I missed the question on snubber sizing. 0402 components will be fine. For the resistor, you can calculate the estimated loss and pick a resistor with sufficient power rating. Typical range of the resistors will be in the 1-10ohm range and caps in the 100pF-1nF ranges. But to actually optimize this selection please refer to this document: 3660.RC Snubber.pdf

    Schottky diode voltage rating can be VinMax plus some buffer so you could pick a 10V or higher. Current rating should be at least the peak inductor current ("IC Ipk" in WEBENCH) plus some margin. In addition, you can improve efficiency and overshoot by picking a diode that has low enough forward voltage and low reverse recovery charge.

    Hope this helps.

    Thanks,

    Amod

  • Glad this is helpful. Please feel free to ping with any more questions.

    Thanks,

    Amod