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.

WEBENCH® Tools/LMR33630: LMR33630 would fail under 36V input

Part Number: LMR33630

Tool/software: WEBENCH® Design Tools

So I designed a 5V supply using LMR33630ADDR, switching frequency is 400kHz. We expect the input voltage would be as high as 36V, since that is what the chip is rated. In testing, the chip would fail at 36V input. In 24V it works totally fine.

The chip will fail in a conductive way, sending 36V down the line and killing every downstream devices. The failure is instantaneous, at the moment any load is applied on the chip (we use a small 5V, 170mA fan as load to begin with). Here is the schematic of the power supply part:

The design mostly follows the reference design in the datasheet, except:

Four small capacitors are merged into a large one, to save space. What is the benefit of using 4 small capacitor in parallel instead of one large one anyway?

Inductor is much larger than the reference, but that's what I got from the formula in datasheet : L = [(Vin-Vout)/(fsw*K*Ioutmax)]*Vout/Vin, where Vout is 5V, Vin is 36V, fsw is 400k, Ioutmax is 3A and K is 0.2. This would yield an L of 18uH(17.9398u), using 15uH due to space limitation, yeilding K between 0.2 and 0.3. It seems both WEBENCH and some form suggestion here never suggested any inductor larger than 10uH, I woulder why.

PCB layout also follows the datasheet suggestion. This is a reflowed PCB so there shouldn't be a problem on ground pad contact.

Any suggestions would be greatly appreciated.

  • Hello Hongyang,

    The absolute maximum input voltage of this device is 38V which must not be violated. I suspect that you may have some sort of voltage transient present upon power up that is violating the abs. max rating of the device.

    One suggestion to mitigate this would be to include an electrolytic capacitor with moderate ESR in order to dampen any transient overshoot that may be occurring.

    Try a 22uF 50V capacitor with ESR in the 100mOhm range.

    When you power this device, be sure to use the 4-wire sense method if available to ensure that your power supply is indeed supplying 36V to the input.

    Also you may want to add a small high frequency output capacitor near the Vout terminal of the inductor to shunt any high frequency noise at the output.

    In terms of your question about parallel capacitors, adding capacitors of various capacitance in parallel helps to eliminate different high frequency bands. Each of the parallel capacitors will look like a different impedance to various frequencies, smaller capacitors will shunt higher frequency signals in general. It is common practice to place multiple ceramic capacitors at the input to the buck converter because each will help to attenuate a different frequency band of interest.

    In regards to your comment on inductors, as long as the inductor meets the minimum value specified in equation 5 of the datasheet then it will work.

    Let me know if the changes above help resolve the issue, thanks.

    Regards,

    Harrison Overturf

  • Hi Harrison

    Thank you for your suggestions. I do not have a 4 lead configuration but I am using a fairly good lab power supply. After adding a 22uF capacitor to the 36V input the power supply would still fail the same way before. It surived one try, then it failed again.

    The power supply seems to work under 33V input, so it seems to be some kind of input voltage overshoot, but I don't think it come from the power supply? I have to use 24V supply for now to make sure the board will not fail. This is a system to drive motors in a robot, so using lower voltage resulting in lower torque avilable.

    All noise-sensitive devices have MLCC as close to their power input as possible.

    Also I do understand mixing capacitor supresses noise in different frequencys. I'm confusing about the fact a lot of power supply datasheet suggest using mutiple electroly capacitors of same value instead of one, for example 22uF x 4 instead of one 150uF capacitor. Using 4 capacitor is more expensive and take more space, not sure what is the benefit of that.

  • Hello Hongyang, 

    Could you share your board layout just for us to double-check?

    Also, could you please take some oscilloscope waveforms of the input voltage at the IC input and the SW node?

    Please use short ("pigtail") GND leads on your scope probe when you do the measurement so you don't pick up extra noise. 

    Cheers, 

    Denislav

  • Hi,

    I'll set up a test environment soon, but I don't think it is the problem of 36V any more, because it just died at 24V input the exact way before. Under 24V power supply, there is no way the input could spike beyond 38V.

    The power supply is killed when we try to reboot the operating system of an onboard ARM chip. In the 36V test before, turning on a 170mA fan will kill the chip. The chip is killed from down stream, and the failure is triggered by load transient. The regulator is also not running healthy, per say, it is outputing 5.04V during no load, 5.2V+ with load.

    PCB layout shown here (top layer only):

    U1 is a 3.3V linear regulator, TLV7333P and is unrelated here. P1 is connected to power ground, and every other ground conenction is digital ground. Digital ground and power ground is connected by a ferrite bead somewhere else.

  • Hello,

    The issues you describe could be caused by the way you routed your GND connection. When you do your testing, please make sure you connect the device thermal PAD to pin 1, just like the datasheet example layout. See the layout example in the datasheet and refer to the pin description table.

    Also, please provide oscilloscope shots of the SW node, VIN, and VOUT so we get an idea of the regulator operation.

    Cheers,
    Denislav

  • Hello,

    I got confused because in datasheet, pin1 (SOIC) is marked as "PGND" and thermal pad is marked as "AGND", so I think the ground can be fairly far apart to achieve better noise proformance. This system have a number of stepper motors running so MGND(PGND) can be very noisy. However during testing the motor drivers are not enabled.

    I cannot change board layout easily without major project delay, so what I am doing right now is to short DGND and MGND as close to the chip as possible, which I use solder to bridge the ground side of C34 and C28 (see layout). This is also where the ground of the scope is attached. Under 24V input, low load (~200mA), Vin looks like:

    Vout (5V side of C34) looks like:

    SW pin looks like:

    I don't want to test under 36V input again because I'm running out of board what hasn't been killed. Please tell me if the waveform look norminal so I can try 36V again.

  • The waveform looks OK for light load condition. 

    Another place where you could stich the two GNDs is between L1 and U3. That would be closer to the IC.

    Here is a snapshot.

    Please connect the two GNDs together and re-test to see if there is any change in behavior.

  • Thank you for your advices. Brigding the ground seems to do it. The system is stable under 36V input and it can handle load and load transient. We decide to not modify the solder mask because if opssible, we want to continue use this design in production to shorten lead time. Even we change the PnP location of the inductor, the solder might just pull it back during reflow. This works ok for now, thank you for the help.