• State Resolved
  • Locked Locked
  • Replies 4 replies
  • Subscribers 39 subscribers
  • Views 668 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.

PSpice Model

bhushan chittaragi
Prodigy 10 points
Other Parts Discussed in Thread: LM5007, TINA-TI

Hi all,

I am trying to simulate the model of lm5007 in PSpice 16.5 demo/trial version. Please help me the procedure how to simulate in it.

Thanks,

Bhushan

  • 0
    TI__Mastermind 39210 points

    Hi Bhushan,

    You will need to download the PSpice model from the product folder and unzip it. Then from Orcad Capture click on File --> Open --> Design ... and then browse to the .DSN file in the unziped folder. When you open this, this should bring up the schematic along with the simulation profile. You can then run the simulation by simply clicking on PSpice --> Run.

    Note that the trial version may have restrictions on the number of nodes in the circuit so if that is exceeded then you will not be able to run the simulation.

    Best regards,

  • 0 in reply to Nikhil Gupta (Product Folder Models)
    TI__Mastermind 41310 points

    Bhushan,

    There is a Manual.doc file and a What is included text file in the .zip file that will give you guidance for how to use the other files present.

    Britt

  • 0 in reply to Nikhil Gupta (Product Folder Models)
    Prodigy 245 points

    Hi Nikhil,

    Thanks you very much, sometimes while simulating the pspice models I face the more problems like convergence, divide by zero. Do you have any tips or docs please help. In tina-TI i dont know syntax for looking the current in branch.

    Thanks and regards,

    Bhushan

  • 0 in reply to Nagabhushana Chittaragi
    TI__Mastermind 39210 points

    Hi Nagabhushana,

    For TI's Power PSPICE & TINA-TI models, you can use the settings below. This should be a good starting point for most simulations and you can tune it from here for specific convergence errors. Divide by zero errors are a little more tricky. Generally they are a sign that the model may not have been constructed properly. However, sometimes I have seen that error disappear after I close PSpice and restart my machine so it might be a simulator issue as well.

    PSpice Parameter

    TINA Parameter

    Starting Point

    When to change

    ITL1

    DC max. iteration number

    1000-1500

    For DC Bias Point and AC Convergence Issues

    ITL2

    DC min. iteration number

    50 – 100

    For DC Sweep Convergence Issues

    ITL4

    TR max iteration number

    400

    For Transient Convergence Issues

    RELTOL

    DC relative error

    1m

    For DC Bias Point, Transient and AC Convergence Issues

    VNTOL

    DC absolute voltage error

    10u

    For DC   Bias Point, Transient and AC Convergence Issues

    ABSTOL

    DC absolute current error

    10n

    For DC   Bias Point, Transient and AC Convergence Issues

    GMIN

    GMIN

    1p

    Try not to change this if possible

    Maximum Step Size

    TR maximum time   step

    20n

    For Transient convergence issues, missing switching pulses, and similar issues.

     

    Best regards,