• State Resolved
  • Locked Locked
  • Replies 8 replies
  • Answers 2 answers
  • Subscribers 48 subscribers
  • Views 5342 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.

OPA171: Altium Pspice (Xspice) model

Bert Hennink24
Intellectual 335 points
Part Number: OPA171
Other Parts Discussed in Thread: TINA-TI, OPA197

Hi,

It has been quite some time ago that I tried to get a working model  for the OPA171 opamp.

I found in the past a model for this opamp but that fails in simulation with Altium Pspice.

Now again I bump in some designs where these opamps might fit in but that I want to simulate also.

get the messages below:

Class    Document    Source    Message    Time    Date    No.

[Warning]    design  XSpice    vccvs1_in\xu1: has no value, DC 0 assumed    14:10:55    6-1-2017    38

[Warning]    design     XSpice    Dynamic Gmin stepping failed    14:10:55    6-1-2017    40
[Warning]    design     XSpice    source stepping failed    14:10:55    6-1-2017    41

As altium users we try to get simulation models for the active parts in our library and this is a part we use in a few designs.

Is there any working model?

I know TI should have Altium available to test a model, because you acquired National Semiconductors a few years ago and at that time Altium was the company wide tool at National.

  • 0
    TI__Mastermind 27715 points

    Hello Bert,

    There is a new model available for the OPA171 which is designed on an updated and improved architecture. It is tested in many different simulators, so compatibility should not be an issue.

    Please download this model here: OPA171.cir

    Let me know if you have any issues simulating with this model in Altium.

    Best regards,

    Ian Williams
    Linear Applications Engineer
    Precision Analog - Op Amps

  • 0 in reply to Ian Williams
    Intellectual 335 points
    Hi This simulation model does not work with the PSPICE in altium
    I get these errors in a working simulation with another opamp replaced by the OPA171 model.
    So still work to do I am affraid.

    Bert

    Class Document Source Message Time Date No.

    [Error] Tempsenor AD590 XSpice Error on line 92: .model r_noiseless\xu5 res(t_abs=-273.15) 11:20:54 9-1-2017 34
    [Error] Tempsenor AD590 XSpice Unrecognized parameter [t_abs] in PSpice Resistor model - ignored 11:20:54 9-1-2017 35
    [Error] Tempsenor AD590 XSpice Unrecognized parameter [-273.15] in PSpice Resistor model - ignored 11:20:54 9-1-2017 36
    [Warning] Tempsenor AD590 XSpice Dynamic Gmin stepping failed 11:20:55 9-1-2017 37
    [Warning] Tempsenor AD590 XSpice source stepping failed 11:20:55 9-1-2017 38
    [Error] Tempsenor AD590 XSpice doAnalyses: Iteration limit reached 11:20:55 9-1-2017 39
    [Warning] Tempsenor AD590 XSpice run simulation(s) aborted 11:20:55 9-1-2017 40
  • 0 in reply to Bert Hennink24
    TI__Mastermind 27715 points

    Hello Bert,

    Upon further investigation, it appears that some standard PSpice parameters for temperature control are not supported by Altium, including T_ABS. Please see the article below for more information.

    Support for PSpice Models in Altium Designer

    Unfortunately, T_ABS is how we define component-level temperature in our architecture to ensure correct noise behavior. I have modified the OPA171 netlist to remove references to T_ABS which should allow simulation in Altium, but noise analyses will be higher than expected.

    Model download:  OPA171_mod.cir

    If you wish to simulate noise, please use our free, fully PSpice-compatible simulator TINA-TI.

    Best regards,

    Ian Williams

  • 0 in reply to Ian Williams
    Intellectual 335 points

    Hi Ian,

    This simulation model works for me.

    Good that you warned about the noise simulation.

    Nice job.

    I will see if there are more TI opamps that we have in our standard library that do not have a spice model yet.

    And see if TI already has a working model.

    Greets

    Bert

  • 0 in reply to Bert Hennink24
    TI__Mastermind 27715 points
    Hello Bert,

    I'm happy that the modified OPA171 model is working for you. Good luck with your simulations, and let me know if I can be of further assistance.

    Best regards,

    Ian Williams
  • 0 in reply to Ian Williams
    Prodigy 20 points

    Hello Ian Williams,

    I was having a problem like this when I tried to simulate the OPA197 in Altium. But using this workaround and removing the R_NOISELESS from the spice model solved my issues!

    Can I be confident about my simulation results? Only the noise analyses will be incorrect or any other analyses would be affected for this modification in the model?
    Thank you!

    Kleber.

  • 0 in reply to Kleber Gouveia
    TI__Mastermind 27715 points
    Hello Kleber,

    With this workaround you can be confident in all your simulation results EXCEPT for noise, which will be higher than the actual device. If you wish to perform noise analysis, I recommend downloading our free simulation software TINA-TI.

    Best regards,

    Ian Williams