• State TI Thinks Resolved
  • Locked Locked
  • Replies 7 replies
  • Answers 1 answer
  • Subscribers 63 subscribers
  • Views 214 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.

LM5122: Difficulty getting Tina-TI to do transient simulation beyond ~28 microseconds

Erik Snyder
Prodigy 10 points
Part Number: LM5122
Other Parts Discussed in Thread: TINA-TI

Howdy. I've been trying to do a transient simulation in TINA-TI on a boost converter using the LM5122. I can get the simulation to run for about 28 microseconds and then it dies with a convergence error. Said errors ALWAYS involve one of the semiconductors (e.g. component T2.DBD).

I have attached the TINA-TI schematic file. The design is a verbatim copy of what Webench suggested for my design given the input and output voltage & current parameters I entered.

I'm guessing maybe the spice files for the semiconductors might be goofy, but they came straight from the manufacturers (in the case of the MOSFETs they are from TI). I've tried adding body diodes in parallel to the MOSFETs, that made no difference. I've also tried fiddling around with the piecewise linear voltage to ramp it at different rates, that made no difference either. So, I'm kind of out of ideas on what to do.

Any help would be greatly appreciated. Thanks.lm5122_boost_conv2.TSC

  • 0
    TI__Mastermind 30080 points

    Hi Erik,

    Thanks for using the e2e forum.
    To make sure the convergence issues comes from the MOSFET part, I would recommend to simulate with an ideal switch first to see if the simulation is running.
    From experience, there are cases where the simulation models do not work well with third party model FETs, even if they are TI components.

    Please let me know if further simulation support is required.

    Best regards,
    Niklas

  • 0 in reply to Niklas Schwarz
    Prodigy 10 points

    Howdy Niklas!

    TSM_files.zip

    I gave your suggestion a try. Strangely, Tina will only work if I replace just one of the MOSFETs with a voltage-controlled switch30ms_plot.zip. 

    So, now the simulation is now running (see attached plot), but I am getting unexpected behavior: it's giving a voltage output that is LOWER than the input voltage...and this is supposed to be a boost converter. The inductor certainly sees some MASSIVE peak currents, but the FETs are only switched every few 10's of milliseconds, rather than microseconds. 

    So...any further suggestions would be greatly appreciated. Thanks.

  • 0 in reply to Erik Snyder
    TI__Mastermind 22680 points

    Hi Erik,

    Please expect a reply by tomorrow due to public holiday.

    Best Regards,

    Feng

  • 0 in reply to Feng Ji
    TI__Mastermind 30080 points

    Hi Erik,

    Thanks for the update.
    It is indeed strange that you cannot replace both FETs in your design.
    I copied over the two FETs from the original TINA testbench and saw the same issue you described.

    I noticed the load resistor is 1.1 Ohm. Starting up with this much load might trigger the overcurrent protection.
    A test with light load (1kOhm load resistance) and smaller output capacitance (22uF) shows that the simulation can indeed achieve the target output voltage.

    You can increase the load and output capacitance again, but I would suggest a longer startup time for the device to come up without OCP.
    This will strongly increase simulation time.

    Best regards,
    Niklas 

  • 0 in reply to Niklas Schwarz
    Prodigy 10 points

    Niklas:

    First, I would like to say that I greatly appreciate your help, I have definitely progressed towards 'getting somewhere' as a result.

    However (uh oh), I guess I would say my difficulty at this point is that a boost converter than can only drive loads at the ~kilo-ohm level is perhaps academically interesting but commercially useless. What is particularly odd is that ALL of the design values I used  are straight out of Webench (see attached screenshot). That the circuit will not function with the design that Webench supposedly created and validated is rather frustrating. Maybe that's why it failed to export the Tina model? LOL.

    Is it possible to run this boost converter with the overcurrent protection shorted out? I have tried voltage-dividing the input down and it didn't seem to do much.

    Again, any suggestions are welcome. I need to be able to have this thing driving ~22 amp loads without too much "babying", because again in the real world, it has to drive a power-hungry DC brushless motor. I totally get that I might have to monkey around with things to get it to simulate in TINA-TI, but I also need some kind of path to a system that will work in the real world.

    Thanks again.

  • 0 in reply to Erik Snyder
    TI__Mastermind 30080 points

    Hi Erik,

    Thanks for the feedback.
    I fully understand that the final design needs to support higher loads. The simulation I ran with light load was meant for debugging purposes only.

    Unfortunately, it is not possible to bypass or disable the OCP function of the device, as the current sensing is required for normal operation as well.

    Right now, I would assume that the main issue is the startup. I suggested to increase the SS cap to reduce inrush current.
    For example, you could try a 200nF cap and run a simulation. If you look at the differential signal of CSP and CSN and see that the voltage goes above 75mV (OCP threshold), the inrush current is too high and you would increase the softstart even further, or reduce the sense resistance.

    Best regards,
    Niklas

  • 0 in reply to Niklas Schwarz
    Prodigy 10 points

    Niklas:

    I think for the sake of yourself and the people reading this we can mark the thread as closed. I'll just have to experiment to find he work-around, but at least I have some ideas on what to do. Thanks for the help.