• State Resolved
  • Locked Locked
  • Replies 7 replies
  • Subscribers 63 subscribers
  • Views 514 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.

LM5118: LM5118

Soumyajeet Dutta
Prodigy 40 points
Part Number: LM5118


Tool/software:

Dear Experts,

Our Requirement is having multi output DC-DC Converter, 

Vin: 24V 

Vout1 : 12V, 5A

Vout2 : 12V, 5A 

Vout3 : 19V, 6A

i have used TI Power Design tool to generate the circuit and simulate it.

Further designed the PCB Layout which is a 4 Layout, needed a review, feedback and help 

 

LM5118Complete BoardLM5118 Schematics

  • 0
    TI__Guru 60001 points

    Hi,

    thank you for using the E2E forum.

    I just reviewed the Schematic and this this items should be fixed first before starting layout review as this will have a impact on the layout.

    • Connection of sense resistor to CS and CSG is not correct
    • C43 would impact the compensation and loop stability - so do not recommend this here.
    • VCCX should only be connected to VOUT after the system powered up - if this should be used then an addition circuit would be required.
      But as VOUT is very close to VIN this does not give a big benefit for efficiency. So might not be used and VCCX can be connected to GND
    • HB is directly connected to VCC which is not correct
    • For that power level it would be good to have footprint for snubbers on the switch nodes, in case need the snubber could then be placed

    Best regards,

     Stefan

  • 0 in reply to Stefan Schauer
    Prodigy 40 points

    Hi,

    Stefan Thanks for your valuable feedback and suggestion, 
    I have done the correction as suggested, 

    I realized the copper pours are not proper and thermal relief is very small,
    Further was wondering if the Inductor sizing is correct or not, i have used TI Workbench to generate the BOM and do the component selection.

     Thanks 

    Tido 

    Updated Schematics as per suggestion,

  • 0 in reply to Soumyajeet Dutta
    TI__Genius 17715 points

    Hi Soumyajeet,

    We do not recommend to use thermal reliefs in the layout. This will introduce parasitics to the design and the heat cannot be distributed equally over the copper plane.

    The inductor size of 10uH seems to be ok for your application. What is the current rating of this inducto? Can yoshare he datashee please?

    Best regards

    Moritz

  • 0 in reply to Moritz
    Prodigy 40 points

    Hi,

    Moritz points taken, once again thanks, curre rating on the inductor Irms=15.5A

    www.farnell.com/.../3356787.pdf

  • 0 in reply to Soumyajeet Dutta
    TI__Genius 17715 points

    Hi Hi Soumyajeet,

    Thanks for providing the datasheet.

    The inductor seems to be a good fit for this application.

    Best regards

    Moritz

  • 0 in reply to Moritz
    Prodigy 40 points

    Hi,

    Moritz, Thanks for all the help, i am really grateful,

    This will be my last question based on the above suggested changes, i have placed and done a layout and made the switching nodes closer and done a thick solid copper pour,

    If you could just do a quick review of the layout that will be a big help, once again thanks for all the time, to provide the feedback.

    1. Regarding the current sense resistor placement CS and CSG 

    2. Vccx Resistor Placement

    3. HO, HB, HS, LO components 

    Marked the Input and Output side

    1. Current Sense Resistor Placement, 2. Vccx resistor placement which must be placed after power on1st pin and components11-20 Pins and components

  • +1 in reply to Soumyajeet Dutta
    TI__Genius 17715 points

    Hi Soumyajeet,

    1. The current sense resistor is part of the power stage. It is a main current path. It has to be connected accordingly:

    I should have a short and strong connection to the diode as well as to GND.

    2. According to your schematic, VCCX is connected to GND directly. Why is there a resistor?

    3. Gate resistors should be close to the IC, not close to the FET. The bootstrap cap can also be closer to the IC.

    Best regards

    Moritz