• State Resolved
  • Locked Locked
  • Replies 5 replies
  • Answers 3 answers
  • Subscribers 47 subscribers
  • Views 222 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

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.

TIPD131: Pspice

yang fan
Prodigy 60 points
Part Number: TIPD131

Tool/software:

I want to perform a Monto Carlo analysis in Pspice. I found that there is something wrong about opax333's macro model, even a bias analysis will be stucked in Pspice, the ciucuit as below, I suppose macro model of opax333 because other circuit can be simulated correctly, I hope someone could help me to figure out it.

  • 0
    TI__Mastermind 22587 points

    Yang,

    1. in your simulation profile select "options".
    2. Under "options" look for ABSTOL.  Set ABSTOL = 1n, default is 1p.
    3. I saw a similar issue in this solved it.
    4. Below is a PSpice Quick-start that shows how to do Monte Carlo.
    5. Also below is a guide for adjusting convergence parameters such as ABSTOL.

    pspice for TI - 10-6-2021.pdf

    PSpice for TI Convergence v1.2 3-16-2023.pptx

    best regards, Art

  • 0 in reply to Art Kay
    Prodigy 60 points

    Hi, Art

    Thank you for your guidence. I have solved question of convergence . But a new question arise, in circuit below, V4 can be from 0.4v to 2.4v to make simuluation successful, but value below 0.4V still cause Spice stucked, datasheet of opax333 show input voltage can be -0.1v to 2.8v, but it's not true in this circuit, Could you please help me figure it out?

    Best regards, Yang

  • 0 in reply to yang fan
    TI__Mastermind 22587 points

    Yang,

    Try adjusting the simulation profile "Options" section.  Set PTRANABSTOL= 1E-5 and PTRANVNTOL = 1E-4.  I saw the same thing you are seeing and this resolved the issue.

    I hope that change solves your problem.  Best regards, Art

  • 0 in reply to Art Kay
    Prodigy 60 points

    Hi Art,

    Following your advice, circuit could be simulated properly, just it take 10s to perform a basic bias analysis, although I alter settings according to PSpice for TI Convergence v1.2 3-16-2023.pptx, time of convergence is still longer than same circuit in TINA apparently.

    But when I peform DC Sweep and Monte Carlo analysis,  convergence  speed is normal.

    Best regards, Yang

  • +1 in reply to yang fan
    TI__Mastermind 22587 points

    Yang,

    Once the operating point is found that is re-used for additional simulations.  I think that is why the convergence speed is normal for the DC sweep / Monte Carlo.  I will contact the modeling team to let them know about the convergence limitations so that they can optimize this in the future.  I will call this closed now as you are able to do your required simulations.

    Best regards, Art