Because of the holidays, TI E2E™ design support forum responses will be delayed from Dec. 25 through Jan. 2. Thank you for your patience.

  • State Resolved
  • Locked Locked
  • Replies 4 replies
  • Subscribers 48 subscribers
  • Views 2127 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.

THS4551DGKEVM: latest pspice model can't be simulated with cadence virtuoso 6.1.7

user6260641
Prodigy 20 points
Part Number: THS4551DGKEVM
Other Parts Discussed in Thread: THS4551, TINA-TI

I download the reference from ti website  THS4551DGK TINA-TI Model (Rev. B) and open the tsc file, the save the macro as (pspice) cir file.   Then I simulate the circuits in cadence virtuoso 6.1.7，but cadence simulator spectre report the error during initial setup. The reported error is tb.I0.X_THS4551.R_NOISELESS: 'trise' is too negative, making the model temperature less than 0 k. I post the photo here. 

Also I try the THS4551 TINA-TI Spice Model (Rev. B) model file, the same error was reported. 

With the same circuit, when I used old model ( released on 07/14/2016, version 1.0) which I also download from TI website.  The circuit is simulated smoothly.  Can you help me on this? why the lastest model doesn't work with cadence virtuoso? 

Some basic information of the old model is listed below for remembering.

*
** Released by: WEBENCH(R) Design Center, Texas Instruments Inc.
* Part: THS4551
* Date: 07/14/2016
* Model Type: All In One
* Simulator: TINA-TI
* Simulator Version: 9
* EVM Order Number: N/A
* EVM Users Guide:  N/A
* Datasheet: July 2016
*
* Model Version: 1.0

Thanks,

Morris

  • 0
    Guru 48395 points

    Well this new model template does use that noiseless resistor idea which normally works fine. 

    Not sure about all the changes in the 2019 model from the 2016 one I helped with (I did quite a lot of testing and tuning on that original model), but I do know the new model is not currently producing the correct input noise terms. I got into that trying to use the THS4551 in this next article for AudioXpress on FDA noise driving audio PCM ADC's. The sims with the new model were not matching theory and indeed i extracted its input noise terms to show they are quite low vs physical device. I am proofing that article today where I had use the 2016 model and make a note to the readers of this issue. They might fix the 2019 model soon, but hard to know for sure when. Personally, I would just use the 2016 model as it was pretty good already. I will say we did not get the Vocm noise modelled there to match the measured plot in the data sheet - that will be in the next article and why it matters at low f (trying to do a 2Hz to 50kHz measurement mic interface example) if the feedback ratios are imbalanced. I was recently able to generate that floated input noise model using the 2016 model with an external element and indeed with +/-1% R worst case mismatch that increases the spot noise some below 10Hz. Easy to fix, which will be in the article. 

  • 0
    TI__Genius 15555 points

    Hello Morris,

    The purpose of the noiseless resistor is to set the temperature of the resistors in the model to 0 Kelvin so that these resistors in the model do not generate noise. From the error you posted, it seems that Cadence is having an issue achieving -273.15 C. I would suggest trying to increase the temperature slightly in the model itself. 

    You can do this by going to line 36 of the model which states ".MODEL              R_NOISELESS RES (T_ABS=-273.15)" and increasing the temperature. Please let me know if this fixes the issue.

    Also please use the model that is included in the reference design, this is the latest version. 

    Best,

    Hasan Babiker

  • 0 in reply to Michael Steffes
    Prodigy 20 points

    Thanks a lot. I will update our simulation when you update the model based on 2019 version. 

    Hasan Babiker has help me solv the simulation problem. 

    Thanks all. 

    Morris

  • 0 in reply to user6260641
    TI__Genius 15555 points

    Hello Morris,

    An update for the THS4551 model is planned to be released. For now, you can go into the netlist and change line 385 to:

    .param NVR = 3.3

    Best,

    Hasan Babiker