• State TI Thinks Resolved
  • Locked Locked
  • Replies 9 replies
  • Answers 1 answer
  • Subscribers 39 subscribers
  • Views 1440 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.

Is there any way to reduce transient simulation time?

Kazuya Nakai59
Guru 21595 points
Other Parts Discussed in Thread: LM5085

Hello guys,

One of my customers is simulating LM5085 transient analysis with other company FET model using PSpice for TI.
They use 3 probes only at the simulation. But the simulation time was over 30 minutes 100ms analysis.

They want to reduce the transient simulation time. Is there any way for it?

Your reply would be much appreciated.

Best regards,

Kazuya.    

  • 0
    TI__Expert 5880 points

    Hi Kazuya,

    Can you please archive and share the project?

    Thank you,

    Jackie

  • 0 in reply to Jackie Horn
    Guru 21595 points

    Hi Jackie,

    Thank you very much for your reply.

    The customer gave me their simulation archive file and I attached it.
    Could you please take a look the file and please give me your idea to reduce the simulation time?

    Thank you again and best regards,

    Kazuya. 

    test1-2022-02-09T23-16.zip

  • 0 in reply to Kazuya Nakai59
    TI__Expert 5880 points

    Hi Kazuya,

    Thank you for sharing the file. I will look at it and let you know what I find.

    Thank you,

    Jackie

  • 0 in reply to Jackie Horn
    TI__Expert 5880 points

    Hi Kayuza,

    Can you please also share the external files rb162l-40.lib and SSM3J356R.lib?

    Thank you,

    Jackie

  • 0 in reply to Jackie Horn
    Guru 21595 points

    Hi Jackie,

    Thank you very much for your reply.
    I got and attached those .lib files.

    Thank you again and best regards,

    Kazuya

    SSM3J356R.lib

    rb162l-40.lib 

  • 0 in reply to Kazuya Nakai59
    TI__Expert 5880 points

    Hi Kazuya,

    Thank you for sharing. I will let you know what I find out.

    Thanks,

    Jackie

  • 0 in reply to Jackie Horn
    TI__Expert 5880 points

    Hi Kazuya,

    I have taken some time to look through this design. I agree that the simulation run time is quite long. Ultimately the problem is that this design has significant oscillation, likely due to the large inductor. A 500ms simulation with this much oscillation will be slow with any simulator. The simulator is running correctly and I believe this data is valid. I would recommend changing your design to reduce the ringing. If you really want to use the design as is, it will be slow due to the oscillation. Here are a few options to tweak the simulation settings, but they will likely reduce accuracy:

    • Reduce the simulation stop time (20ms may be sufficient to reach steady state)
    • In the sim profile, in the section Options -> General, you can increase the values of RELTOL, VNTOL, ABSTOL, or decrease the value of GMIN (This will cause the most significant decrease in accuracy)
    • In the sim profile, in the section Options -> Transient, you can try changing the METHOD to Gear. Do not use TRAP, which struggles with oscillation
    • You could increase the size of the smallest resistors and decrease the size of the largest capacitors
    • You could replace the third party models (PMOS and diode) with ideal components, which are found under Place -> PSpice Component -> Modeling Application

    If you would like support with modifying the design, I can reassign this thread to the LM5085 product line. Currently this thread is under the tool PSpice for TI, so I support problems caused by the simulation engine rather than the design. Please let me know if you would like to discuss this further with the LM5085 team.

    Thank you,

    Jackie

  • 0 in reply to Jackie Horn
    Genius 3685 points

    Hi Jackie,

    Kazuya had trouble logging in, so I'm posting this on his behalf.

    Thank you very much for your reply.
    You said that you will try changing RELTOL, VNTOL, ABSTOL, and GMIN, but I would like to know the approximate range of those values.
    Or give me at least three examples that I should try.

    Thank you again and best regards,

    Kazuya. 

  • 0 in reply to Ryu Yamashita
    TI__Expert 5880 points

    Hi Ryu and Kazuya,

    You could try increasing by one order of magnitude to start, or possible two orders of magnitude. I would not recommend increasing beyond 2 orders of magnitude. Please note that this option may cause a reduction in accuracy. As I recommended earlier, the simulation requires many time steps due to the oscillation, which is the main cause for slowness. Further speed increases would likely require changes to the design. 

    Thank you,

    Jackie