• State TI Thinks Resolved
  • Locked Locked
  • Replies 3 replies
  • Answers 1 answer
  • Subscribers 63 subscribers
  • Views 1022 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.

TINA/Spice/LM5069: SNVA683 / LM5069: Convergence problem

ZackZack
Prodigy 20 points
Part Number: LM5069
Other Parts Discussed in Thread: TINA-TI, ,

Tool/software: TINA-TI or Spice Models

In snva683 application report Texas provides a solution for surge stopping and reverse voltage protection with the LM5069.

I tried to rebuild the circuit in Figure1 in TINA-TI but there are convergence problems for transient analysis with various parameters including the default parameters.

The only component I did not paste in the simulated circuit was the TVS Diode at the input, but that should be no problem for convergence. The problematic device seams to be D1. If D1 is bridged with a wire the transient analysis works without any problems.

Is there a problem with the model of LM5069 or are ther any Analysis parameters to get the simulation to work?

Thanks in advance

SNVA683.TSC

  • 0
    TI__Intellectual 1760 points

    8475.SNVA683.TSCHi Zack

    The reason the simulation was not converging was due to the PGND net actually not connected to a physical ground pin as suggested in the EVM users guide. Adding that pin fixes the problem right away, we will update the product folder model as well. Thank you for catching the error.

    Regards

    Ranjani

  • 0 in reply to ranjanir
    Prodigy 20 points

    Hi Ranjani,

    adding the PGND net to physical ground like you did in the attached simulation file is actually the same as bridging the diode D1. Doing this leads to a negative voltage between VIN and GND pins of LM5069, which violates the absolute maximum ratings of the device. That is not the same as suggested in snva683 or on LM5069EVM-627. In these circuits there are two different ground nets, one device ground for LM5069 and one global ground for the whole board. These two grounds are connected by the diode D1.

    But your reply led me to the idea to switch the to ground nets. In the simulation attached i used the TINA-TI ground symbol for the device ground and some jumper symbols to provide the global ground net SGND. Input and output voltages of the circuit are now realted to SGND. Now VCC is not negative anymore and does not violate the absolute maximum ratings and the simulation is converging.

    So it seems that the calculation needs the TINA-TI ground symbol at the GND pin of LM5069. I'm sure this workaround is possible if there is only one LM5069 in the simulated circuit. If there are two LM5069 (for example for bidirectional switching) one would need two undependent device grounds. Is there a chance that the device model is updated in order to make such simulations possible and when could it be distributed? Or is it a general problem of spice simulation which can not be changed by a simple model update?

    Best Regards

    /cfs-file/__key/communityserver-discussions-components-files/196/SNVA683new.TSC

  • 0 in reply to ZackZack
    TI__Intellectual 1760 points

    Hi Zack

    Sorry for the late reply but the model was released a decade ago is not configured to handle the global ground as the local GND is probably replaced by a 0V ground in the internal nets. We have been checking for these configurations more extensively for the past years.  

    Regards

    Ranjani