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.

DRV8350R: some problem about vgls 、glc、cpl pins

Part Number: DRV8350R
Other Parts Discussed in Thread: DRV8350

hello TI' Engnieer:

         I developed a motor control board with drv8350. The datasheet of mosfet is in the attchment .But after test ,almost drv8350 broke.

Vgls and glc get short or vgls and cpl get short. I added an 8Ω Rg. And the Idrive-LS and Idrive-hs is 1A and 2A.

        Could you please help me analyze which parameter caused the damage of DRV8350. Now I have reduced the Idrive  and test

for a while.

        Looking forward to your reply.

best wishes



  • Hello,

    You need to select the best IDRIVE setting to match your MOSFETs. Please review this E2E FAQ: LINK

    It would be good to review the schematic, and potentially the layout of the PCB.



  • DRV8350.rar

    hello Matt:

             you can see the schematic.I add a Rg. I think the resistance will affect the IDRIVE configuration.But According to damage mode that the cause of the damage is related to VGLS, so I presume it is the IDRIVE problem.  Thank you very much for reviewing the circuit diagram and helping me analyze the reason.It make me nervous that the new 10 pcbs are all damged for this reason

    Best wishes


  • shengzhong,

    By my rough calculation, 1-2A, 3nC for Qgd (from datasheet provided), 8 ohm gate resistance, assuming ~12V Vgs, this means the gate would need to slew in ~25ns.

    Customers usually aim for 100-200ns which is still very fast.

    Your IDRIVE is much too high and the gates are getting damaged because there is likely overshoot/undershoot on the gate nodes.

    Please change the IDRIVE to 100mA or similar and try your experiment again.

    As mentions, please review our IDRIVE FAQ and App not linked above.



  • Adam:

            yes I think 100ma or 200ma is right.But when I used  CSD88537 in my perious version ,the parameter seems ok and 50 circuit boards can work well。 Is some things wrong my pcb layout.The CSD88537 ,I also added a 5Ω Rg. 




  • Hi Shengzhong,

    Your VGLS regulator should be bypassed to GND, the same net as the DRV835x thermal pad. It looks like it is not on the layout. We have seen that if the VGLS capacitor has long traces to the VGLS pin or GND, it can cause damage to the regulator.

    The use of R128/R124 to "select" the GND may be causing issues. DRV835x needs a solid connection to a GND plane for current as well as power dissipation.

    I noticed that a capacitor is missing from phase C high-side MOSFET drain to low-side MOSFET source in the schematic.

    The 1/2-bridges are on a separate ground (SPGND), and so you have three separate ground planes going on. You should trace the following paths to make sure they are as short as possible:

    • VGLS paths:
      • DRV835x VGLS pin to VGLS capacitor
      • VGLS capacitor to DRV835x PGND pin
      • VGLS capacitor to bottom of the sense resistor
      • top of sense resistor to low-side MOSFET source
      • low-side MOSFET gate to DRV835x GLx pin
    • VCP paths:
      • DRV835x CPH pin to CPH-CPL capacitor
      • CPH-CPL capacitor to DRV835x CPL pin
      • DRV835x VCP pin to VCP capacitor
      • VCP capacitor to DRV835x VDRAIN pin
      • High-side MOSFET drain to DRV835x VDRAIN pin
      • High-side MOSFET gate to DRV835x GHx pin



  • Hi Matt

          Yes,I think the gnd may be causing issues.Because I use an 24-5 isolated power supply which leds to the problem that dgnd is higher than pgnd,about 0.5V. This make sampling current difficult. But next version will fix the problem.The idea about the path of vcp and vgls is very helpful to me and I'll try it



  • Hi Shengzong,

    OK, that sounds good. Please let us know if you want us to review your updated schematic and layout!

    Should I close this thread for now?



  • Hi Matt;

               Could you see the attachment (drv8350.rar) which I add it to my reply five days ago ?The schematic and the layout is  in it.I am looking forward to your professional advice.After reviewing my pcb,you can send message to me.

               For this problem ,I think I have get much detail for my problem.You can close this thread.And after getting your advice,I will start next version of motor drive card with drv8350.



  • Hello Shengzhong,

    I did do a review of the schematic in my previous post and gave some comments there.

    Some other comments:

    • It is normally a good practice to have snubber footprints on the board, just in case you run into EMI or ringing issues.
    • When you put the sense resistor on a different layer than the MOSFETs, it can add inductance in that path, It is best practice to have the MOSFETs and sense resistor on the same layer with thick planes connecting them
    • Bypass capacitors should have as short and thick trace as possible to the DRV835x pin as well as the PGND (DVDD, VGLS)
    • Route VDRAIN and VM as separate nets, this is better for the operation of the VDS monitors.

    If you have not already, please review this resource: LINK



  • Hi  Matt :

          Thank you for your advice.And when I finished next pcb,I will ask for your valuable comment!

    best wishes


  • Hi Shengzong,

    Sounds good!