• State
  • Locked Locked
  • Replies 3 replies
  • Subscribers 63 subscribers
  • Views 240 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.

Original question:

TPS7B81: PSPICE Model?

TPS7B81: TPS7B84-Q1 SPICE Model: VOUT vs Temperature

Alex L
Prodigy 150 points
Part Number: TPS7B81
Other Parts Discussed in Thread: TPS7B84-Q1,

Tool/software:

Hi Team

I tried to simulate TPS7B84-Q1 using the model you provide in the related webpage.
I used OrCAD PSPICE A/D ver 22.1.

Model works fine at 25°C.

When I try to simulate the following very simple circuit using a different temperature setting, output voltage starts to be different from ideal (5V)

For
T=25°C --> Vout=5V
T<25°C --> Vout>5V (e.g. 6.3V @-20°C)
T>25°C --> Vout<5V (e.g. 4.6V @40°C)

Please note that I used standard resistor and capacitor models (TC1=TC2=0)
I also tried to divide both reference resistors by a factor of 10 with no result whatsoever.

I see from comments in tps7b84-q1.lib file:
* Model Usage Notes:
*
(....)
* 2. Quiescent current, noise characteristics and temperature effects are not modeled

All model internal resistors do have TC=0,0

Therefore, temperature effects should not be modeled.
However, I see a strong detrimental effect on temperature in my very simple simulation.

What is causing this issue?
Does the model actually work for T<>25°C?

Best regards

A.L.

  • 0
    TI__Guru 50025 points

    Hi Alex,

    I looked at the model and I'm not sure why there is any temperature variance because I also cannot find anything that should change with the temperature setting. The note in the model would be more accurate if it said that temperature is not tested and not just modeled, because we normally do not test the models over temperature since temperature is not modeled. FYI, we are working to improve the model architecture, and eventually we would like to have everything, including temperature, modeled, but it's a large project that will take time. 

    Regards,

    Nick

  • 0 in reply to Nick Butts
    Prodigy 150 points

    Hi Nick

    The problem is probably in the equations Pspice calculates by default, e.g. the diode equation.

    I tried addding on d_d1 subcircuit the line +TNOM= temperature which the simulation is carried on at.
    That means the diode parameters are specified at tnom, and hence the diodes do perform at the simulation temperature as they would perform at 27°C.

    This way I get an output voltage of about the ideal value (5V), with only a minor discrepancy.
    I then kept the above mentioned line to have a model more or less independent of the simulation temperature,
    which is not my ultimate goal (that would be having temperature dependency for this very model, too), but serves the purpose of keeping the TPS7B81 model in a more complex simulation which has got temperature dependency.

    I would then suggest you to look for hidden parameters and equations that are computed by befault in Pspice and that alter the behaviour of the circuit at temperatures different from the default one.

    Best regards

    Alex

  • 0 in reply to Alex L
    TI__Guru 50025 points

    Hi Alex,

    Understood, and thank you for the insight. 

    Regards,

    Nick