• State Resolved
  • Locked Locked
  • Replies 4 replies
  • Subscribers 41 subscribers
  • Views 1448 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.

TINA/Spice: “Trust, but verify” SPICE model accuracy

Prasad Jaiswal
Prodigy 40 points
Other Parts Discussed in Thread: TINA-TI, OPA2137

Tool/software: TINA-TI or Spice Models

This is with reference to series of nice articles written by  regarding SPICE model verification with respect to Datasheet results. I tried to simulate the circuit used as an example by him in his post, but was not getting the expected result. You can read his article and my post in comments section at the link provided below.

It could be some silly mistake I might be doing, but I found article to be useful enough in order to make sure I completely understand it.

I have also attached screenshot of the error I am getting, it also contains the circuit diagram.

Link for article: https://e2e.ti.com/blogs_/b/analogwire/archive/2017/07/27/trust-but-verify-spice-model-accuracy-part-1-common-mode-rejection-ratio-cmrr

  • 0
    TI__Mastermind 39210 points
    Prasad,

    Can you please share your TSC file so we can recreate the issue?

    Just by looking at the snapshot, what I can potentially see as a problem is the divide term that you have. If the denominator goes to zero then the simulator will throw the "Divide by Zero" error. My recommendation would be to add a small value to the denominator, i.e make it (ACM(s) + k). where the magnitude of k is very small compared to ACM(s) for majority of the time in the sim. This way the k term does not impact your sim most of the time and only comes into picture when the denominator tends to zero.
  • 0 in reply to Nikhil Gupta (Product Folder Models)
    Prodigy 40 points

    Hello Nikhil,

    Thanks for you response. This is exactly the point I have raised in the comment section of the article (that Acm is ideally 0 and that could be causing this issue), but I an doesn't seem to be facing this problem.

    Anyways, PFA simulation file.CMRR.TSC

  • 0 in reply to Prasad Jaiswal
    TI__Mastermind 31355 points

    Prasad,

    Your differential setup has no input as the two controlled sources both have zero gain. Please set both to 0.5 (for a total of 1) and try again.

    Regards,
    JC

  • 0 in reply to JC Zhu
    TI__Mastermind 27715 points

    Hi Prasad,

    JC's suggestion is exactly right. If you set the gain of your sources VCVS3 and VCVS1 to 0.5 (500m), you can use post-processing to extract the CMRR without seeing the divide by zero issue. In this case the CMRR of the OPA2137 model is equal to 89 dB, a bit off from the typical spec of 84dB. The -20dB/decade roll-off in the model also doesn't begin until high frequencies, while in the actual part the rolloff starts around 100 Hz. As you can now see, this model is quite old and not as accurate as those for our more recent devices.

    Best regards,

    Ian Williams
    Applications Engineer/SPICE Model Developer
    Precision Amplifiers