• State TI Thinks Resolved
  • Locked Locked
  • Replies 9 replies
  • Answers 3 answers
  • Subscribers 40 subscribers
  • Views 2574 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.

WEBENCH® Tools/LMR16020: LMR16020, forgot by WEBENCH, problems with simulation.

Andrey Porokhnyuk
Prodigy 100 points
Part Number: LMR16020
Other Parts Discussed in Thread: TINA-TI

Tool/software: WEBENCH® Design Tools

I am trying to simulate LMR16020 for +36V output with free and generally PSPICE compatible LTSPICE.

But using unencrypted model simulation fails with no POWER-GOOD signal and no good voltage at SW. I checked and double-checked all the pin numbers... and still.

Tried to see what WEBENCH thinks about it, and it knows nothing about LMR16020. Why?

Is it some king of orphaned and abandoned IC? In whitepaper it looks very pretty, simple to solder package, high power, integrated 2MHz clock and nMOSFET, relaxed inductor requirements(!)...

And still, I can not check the design in software.

Does the circuit look good?

  • 0
    Prodigy 100 points

    BTW, there's a weird declaration in the .SUBCKT:

    .SUBCKT LMR16020P_TRANS BOOT EN FB GND PWRGD RT/SYNC SW VIN PAD PARAMS: SS=0

    What is SS?

    TI Tina can not simulate this PSPICE model.

  • 0 in reply to Andrey Porokhnyuk
    TI__Genius 11085 points
    I will move your question to the Webench forum to get better support with Webench and simulation issues.

    -Yang
  • 0
    TI__Intellectual 1440 points

    Hi Andrey,

    Due to legal issues (LTSpice EULA), we can not support models in LTSpice.

    Also to use LIB file in TINA, please try removing the '/' form the net/pin names such as 'RT/SYNC' and replace it with '_' on all instances.

    'SUBCKT LMR16020P_TRANS BOOT EN FB GND PWRGD RT/SYNC SW VIN PAD PARAMS: SS=0'

    And let us know if you still face any issues with TINA-TI.

  • 0 in reply to Andrey Porokhnyuk
    TI__Intellectual 1440 points
    Hi Andrey,

    Parameter SS=0 is used to observe normal startup behavior and SS=1 to see steady state faster.
  • 0 in reply to Imran Dharwad
    Prodigy 100 points

    - Due to legal issues (LTSpice EULA), we can not support models in LTSpice.

    oh. Even giving a hint is illegal?. wow.  OK.
    But can you confirm, it is not kind of wrong beta model, uploaded by mistake?
    Or maybe anyone outside of TI staff on the forum?

    - Also to use LIB file in TINA, please try removing the '/' form the net/pin names such as 'RT/SYNC' and replace it with '_' on all instances.

    Thank you. So it is not just a problem of generating the symbol, but the engine takes it the same.

     

    - Parameter SS=0 is used to observe normal startup behavior and SS=1 to see steady state faster.

    Oh! maybe the core of the problem is here. Thank you again! I will check it.

  • 0 in reply to Andrey Porokhnyuk
    Prodigy 100 points

    Welll... with changes above the model gets accepted by Tina, but "Operating point not found: Component: U1.D_U100_D74", when input voltage is applied.
    If there's no input voltage(I had put there a voltmeter instead of source by mistake), the model tries to make Vout out of nothing, so I get kind of 36V noise at the output.

    test_36V_.TSC

  • 0 in reply to Andrey Porokhnyuk
    TI__Intellectual 1440 points

    Hi Andrey,

    The model works fine with the following changes in the test setup.

    1. The reverse breakdown(BV) voltage of Diode used is lesser(20V). Recommended operating condition is to keeping higher than VIN and then it works fine.

    Currently I have made it to 50V.

    2. Also while keeping SS=1, please make sure to add proper initial conditions on Cout capacitors and Inductor.

    Also I have updated analysis parameters to support simulation. PFA the updated working schematic with above mentioned changes.

    test_36V_updated.TSC

    Please let me know if you have any other questions.

  • 0 in reply to Imran Dharwad
    Prodigy 100 points

    Thats weird

    I had RBR1MM60A in LTspice, and in Tina I took the first thing in sight, just in order to see anything at the output. And I do not see anything even when putting BAS70 there.

    SS=0 at my side.

    But your file simulates well.

    What did you do else, to make it run?

  • 0 in reply to Andrey Porokhnyuk
    Prodigy 100 points

    Ah, I see, you circuit could not be simulated either, until you know initial conditions for sure.

    Is it possible to fix the model for it to be capable simulating device start-up transition with unknown (dynamic) load? (I have a bunch of soft-starting amplifiers and want to know, where can I cut sources safely by paralleling power) Or publish newer unencrypted model? At the moment encrypted model is 10 times size of current unencrypted, which I expect is related to updates taking that space.