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.

LM5146: LM5146RGYR

Part Number: LM5146
Other Parts Discussed in Thread: LM5145, , CSD19531Q5A, LM25148


I need help in getting schematic review for the board design.
Can someone help me with it?
I need it ASAP


  • Hi Bob,

    Apologies for the delay.

    Here are some comments:

    1. You may want to use different high-side and low-side FETs (depending on Vin, Vout and where optimization should occur in the Vin range). Use the quickstart calculator in tandem with the NexFET selector tool: No harm checking WEBENCH as well.
    2. NC pins of the controller can be tied to GND (for better heat spreading).
    3. C10 6.8pF should go from ILIM to PGND (not from SW as shown).
    4. Check compensation values with the quickstart. Ensure that the correct derated value for ceramic Cout is entered. 5 x 22uF/25V may derate 40-60% in the 8.4V-16.8V range. Higher Vout is worst case, as it results in a lower effective Cout and thus higher crossover (for a given compensation circuit).



  • PS: If Vin-max = 60V, then you can use the LM5145 75V input version.

  • Can you share with me exact part number for it plz?

    Regarding you 1st message, I used webench and EVM design files to create this schematic. I will look another link as well..

    Can you elaborate 4th point further please?

    I also need layout review after it. 


  • LM5145RGYR, see 

    You can use Murata's tool to check the effective capacitance of the ceramic at a given voltage:

    Here is the plot for a 22uF/25V/1210/X7R at room temp:

  • Hi
    I guess, LM5146 is fine considering future use because i don't see any reason to choose LM5145 over 46.

    Second, I need to know why i have to choose different MOSFETs for High and LOW side. Can you help me to understand it?
    I noticed in the Webench that they are different.
    I want to use low cost MOSFET but if I use HIGH side CSD19531Q5A then Webench suggest SUM90N10-8M2P-E3. This MOSFET is not only expensive but different package as well.

    I tried to use NexFET selector tool but I couldn't understand it much. It has different GUI than the video available for it.

    The output capacitors that I used is C3216X5R1V226M160AC from TDK.
    I got your point about its effective capacitance.
    Can you suggest some solution for it please?
    I checked at Webench. It change the capacitance values
    8.4V = 22uF
    12.6V = 2x 22uF
    16.8V = 3x10uF


  • Hi Bob,

    The LM5145 is lower cost, hence that suggestion. They are pin-to-pin compatible, so you could change in future as well if needed.

    In terms of the MOSFETs, the high-side FET has all the switching loss, so higher Rdson (lower capacitance) is possible. And the low-side FET is conduction loss dominant, especially for large step-down ratios, so it can be lower Rdson. I would stick with 5 x 6mm MOSFETs - take a look at the LM5146 EVM, which is a 12V/8A/400kHz design (close to your spec).

    The LM5146 quickstart calculator will be really helpful for your design - please complete and send that for review.



  • In terms of output caps, I recommend using 22uF/25V/X7R/1210. The total effective capacitance will be lowest at the highest Vout setting, so design the compensation for that and then do a quick check at the lower output voltages with those values.



  • Hi
    I added the values according to the requirements and some values that i already used in the circuit. For example, compensation circuit. 
    I have no idea about pole and zero that you might adjust it.
    I have different battery power sources so i selected minimum voltages consider low battery cell count and Nominal/Max considering higher cell count.
    I setup current limit to 12A that was previously i guess set at 25A.

    Now here is the tricky part because, the output will change i.e. 8.4V/12.6V/16.8V

    1. The Cal suggest 3x22uF 25V Cout and 2x 4.7uF Cin100V for all outputs

      I used 35V 22uF and 100V 4.7uF Capacitors.

    I attached all the sheets for various output. Plz, have a look and let me know if i missed anthing.
    I will use then final sheet BOM that you will suggest.

    Last, If this is your email then I have another request also pending on your end at TI customer support. Plz, confirm me if it is yours.

  • Hi
    Is there any feedback about above message?
    Plz, let me know,
    I have to finalize this board asap to get layout review.

  • Hi Bob,

    Let me check email for the layout.

    Are these 3 separate designs or just one with adjutable Vout? If it's the latter, then we design the compensation with highest Vout (lowest effective Cout) and then check the lower voltages with the compensation values fixed.



  • These are same design but i adjusted Vout differently in all three.
    I also noticed in other buck design that most of the time(Even reference design and Webench Design) used same MOSFET for High and Low side.

    This is my email for layout review of LM25148 that i sent you few weeks ago.

  • Three different output voltage but one implementation - so it has an adjustable Vout, correct? Just wondering if we need to have one compensation network for all three, or if we can optimize it for each Vout setting.

  • Yes correct.
    I need 3 different outputs select able through a switch.
    I need one network for all because i don't want to add more components for each setting.
    There should be one optimal solution that can do all three.
    It's like adjustable buck converter and I found many in the market

  • Just looking at the quickstarts, I see you are not adjusting Cout for the different output voltages. Go ahead and insert the correct "effective Cout" for each output voltage setpoint, and keep the compensation network constant based on the stability for the highest Vout.

  • Just looking at the quickstarts, I see you are not adjusting Cout for the different output voltages. Go ahead and insert the correct "effective Cout" for each output voltage setpoint, and keep the compensation network constant based on the stability for the highest Vout.

    Also, you may use 80V FETs here for better efficiency. No need for 100V device if the layout is good and Vin-max is only 65V.

  • Is that you mean?
    I changed output capacitance based on Webench recommended for different outputs.

  • I found the layout. Here are some comments:

    1. The switch for the output setting looks huge - can it be reduced? The FB trace needs to be as short as possible, as this is a high impedance node very sensitive to noise (note high feedback divider values).
    2. It would be nice to have an input cap on the top side as well.
    3. No need for SW vias - these just put the high dv/dt on the bottom side of the PCB (facing the EMI table). SW copper should be minimized, as it is a radiating plane. See the LM5145 EVM layout, which resembles this design. More important, the SW vias disrupt the GND plane under the power stage.
    4. The shunt looks quite large, 2512. Consider using a wide aspect ratio shunt for lower parasitic inductance (see EVM).

  • Thanks
    I will update these suggestions and will send you again for another review plz.

  • Okay, thanks Bob.

  • PS: looking at the three captures from the quickstart calculator in the post above, Cout should be highest at low Vout and then progressively reduce for the higher Vout setpoints.

  • Hi

    So what's the final value should be because I don't have an option to change capacitor while changing output.

  • No, what I mean is select the capacitance, then insert the correct derated value for each output setpoint. the screenshot above has 22uF for 8.4V and 44uF for 12.5V, which has to be incorrect.

  • But the CAL and WEBENCH increase capacitance as Vout increases

  • Hi Bob,

    This still shows 22uF for 8.4Vout, but it should give the highest capacitance based on the derating with voltage of ceramics.

    My assumption is you're selecting a set of capacitors that will work with this adjustable output design, so just enter the applicable capacitance for the three Vout levels. Actually, we usually just check min and max Vout -- design the loop for max Vout and fix the compensation values when checking the min Vout with the higher effective Cout value.



  • Hi
    I sent you an email for layout review of this design.
    Plz, check that and Let me know if you need anything futher.
    I need some guides related to buck converter that i can follow up in the future design.
    I actually design many buck/boost converter and I feel like missing many aspects from design perspective.
    Last but not least,
    Where i can learn about the following.
    1: Compensation Circuit,
    2: Pole and  Zero placement
    3: Crossover Frequency
    4: Input/Output capacitor selection

    I checked datasheet. It has some equations.
    Are there some thumb rules that i can follow to design TI based buck converters.

    Thanks for all your help.
    I really appreciate it.

  • Hi Bob,

    The LM5145 / LM5146 datasheet actually has some good info on compensation for voltage-mode control. I have a couple of articles on on current-mode control as well that are worth looking at.

    I'll check my inbox now to see if I got your latest layout. The LM5145 and LM5146 EVMs are actually good templates to copy from a layout standpoint. Also, the datasheet guidelines for layout are pretty comprehensive.



  • Hi 

    Plz confirm me if you are able to find layot files in email.

    It would be great if you can give me some feedback before next week.


  • Yes, I see the email and should be able to get to it this evening or tomorrow.

  • Thanks
    Looking forward to hear back your feedback.

  • Hi
    It would be great if you can give me feedback today.
    I am a bit getting late on production cycle.

  • I will take a look here shortly and get back to you this evening.

  • Thanks 

    I will wait for your feedback 

  • Hi Bob,

    Here are some comments upon reviewing "Voltage limiter V1":

    1. Being the most important caps in the design, the 4.7uF input ceramics are way too far from the FETs. Bring the FETs closer together and move the 0402s cap right by the high-side FET drain. This allows closer placement of the 1210 caps. Add more GND vias at the cap return terminals. See app note SNVA803 for power stage component placement.
    2. Tie NC pins of the controller to GND (better heat spreading).
    3. Minimize the area of the SW copper polygon connecting the FETs to the inductor.
    4. The gate and source pads of the FETs look like they could be bigger.
    5. Move the SW via near the FETs such that the HO and SW traces route close to each other, effectively as a diff pair.
    6. Layer 2 should be a solid GND plane under the power stage -> move the HO trace to layer 3 and route in parallel with SW on the same layer. This takes the high dv/dt SW trace off the bottom layer as well (note: the bottom layer faces the EMI table and can easily couple noise to that GND).
    7. Consider adding two more vias in the DAP for the controller.
    8. Keep the VCC and BOOT caps close to the respective pins of the controller (e.g. move vias closer to the controller pins if needed).


  • Also, take a look at the LM5145 EVM layout for reference. The LM5145 is effectively the same controller as the LM5146, just a lower Vin-max rating.

  • Hi
    Thanks for your feedback.
    I will update the design of LM5146 based on all these valuable suggestions.
    It cleared a lot of my concept.
    I need one final request if you can help me with it plz.
    It is about LM25148.
    You mentioned that i should use sense resistor different size.
    Can you help me to fill out this CAL for the following parameters.
    1: Priority small size inductor and board size
    2: Vin 10 to 36V
    3: Vout 7.4V 15A

    The height of the components should be minimize as well. The major component that drive height and all parameter is inductor.
    I tried to follow up WEBENCH and other recommendation but due to board size it is not feasible for me
    LM5148-LM25148 Quickstart Calculator_rev2.xlsm

  • Hi Bob,

    What you have looks pretty good for the LM25148. Just drop the shunt to 3mΩ, so you have some margin from full load to current limit. We typically recommend 125-150%, so you could even drop it to 2mΩ. Also, you can go with a 2.2uH inductor, which is a standard value - take a look at Coilcraft XGL series of inductors. The output cap ESR should be a few mΩ if you use ceramics.

    I recommend submitting a separate E2E for the LM25148 if you need further support - then the responsible engineer will reply.