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.

Format for TINA model

Other Parts Discussed in Thread: TINA-TI, OPA659, OPA657

Hi,

I m trying to implement a circuit which has HSMP 3832 (DIODE) using Tina-TI. But this diode is not available in tina library. When i checked the diode website (  http://www.avagotech.com/pages/en/rf_microwave/diodes/pin/hsmp-3832/   ), under design tools and model, there is a spice model for hsmp 383x. 

The problem is when i tried to download this spice model, i found that its in .htm format. Which i dont know how to import into tina. 

The following is a link from where i downloaded the .htm format of the abpve mentioned diode and the tutorial that i used to check how to import the spice model into tina. 

http://www.avagotech.com/docs/MPUB-756

https://www.youtube.com/watch?v=fHfVsmf6Kvs

Hope someone can help me in this. 

Thanks in advance. 

Livingstone Arjunan.

  • Hi,

    I see the following listed for this diode:

    http://www.avagotech.com/docs/MPUB-756

    HSMP-383x Limited APLAC Model

    D1 uses the standard SPICE diode model, and is described by Is, N, and TT. Rs in the standard model is replaced by the external network of Rmin, Rmax, and Rvar. The parameters are for a single diode (HSMP-3800). Parameters also apply to the individual diodes within multiple diode configurations.

    Parameter unit description value

    Rmax ohm maximum r.f. resistance 5000

    Rmin ohm minimum r.f. resistance 1.5

    K __ resistance curve fitting exponent 0.9327

    A __ resistance curve fitting exponent 0.0183

    L nH connection inductance 2

    C pF diode capacitiance at r.f. frequency 0.2

    Is A diode saturation current 1.49E-09

    N __ diode ideality factor 2.022

    TT nsec transit time (carrier lifetime) 500

    I also see this statement in the part's datasheet:

    A SPICE model is not available for PIN diodes as SPICE does not provide for a key PIN diode characteristic,
    carrier lifetime.
    You could possibly place a diode in TINA-TI and then edit its properties.
    Of the parameters listed above, some of them (i.e. Is, CJO) can be accessed on a diode you place on the schematic (and then Right click on Properties and then type that you can edit):
    The series inductance and resistance: You may be able to place / add externally.
    Carrier Lifetime is obviously not available.
    This may get you close enough.
    Others may have better solutions?
    Regards,
    Hooman
  • Hi Hooman,

    Thank you for the suggestion. I can only add three parameters ( C pF diode capacitiance at r.f. frequency 0.2,

    Is A diode saturation current 1.49E-09,TT nsec transit time (carrier lifetime) 500) from HSMP description. Hope that should be close enough. 

    Thank you,

    Livingstone Arjunan

  • Hi,

    Sorry, I had not noticed that TINA-TI shows "TT-transit time" (carrier lifetime) as an editable diode parameter. I cannot explain why then the PIN diode's datasheet states the following:

    A SPICE model is not available for PIN diodes as SPICE does not provide for a key PIN diode characteristic,
    carrier lifetime.
     
    I had assumed that TINA-TI would contain the same set of parameters as SPICE (which according to the statement above, does not include Carrier LIfetime for a diode- I have not researched / verified that about SPICE).
     
    Hopefully it does work for you.
     
     
    Regards,
    Hooman
  • Hi Hooman,

    I tried to edit those three parameters which i mentioned in my previous message. Here is my cirucit. 5808.sinisa.TSC

    I am using the diodes for switching purpose. VF1 and VF2 are the output which will be switched on and off using the diodes.

    When i tried for ac transfer characteristics analysis, an error pops out- " operation point not found" for Component: U1.D_D31. 

    Can you please help me how to solve this error?

    Thanks in advance. 

    Livingstone Arjunan

  • Hi Livingstone,

    I changed your active device from OPA657 to OPA659 instead and AC Analysis seems to run fine (please check it as I did not verify it- no error messages).

    Here is the modified simulation file:

    6758.5808.sinisa modified 7_14_14.TSC

    Let me know if you think simulation is running well with the new device?

    If so, then I'll forward the fact that OPA657 simulation seems to balk, to the folks in TI responsible for models to get their expert opinion to see if there is anything wrong with the OPA657 TINA-TI model or not?

    Regards,

    Hooman

  • Hi Livingstone,

    I have consulted with TINA-TI experts. They have reminded me that sometimes you may have to modify some of the Analysis parameters to get things to run to completion. Here is their response on this:

    "I am able to run the simulation with OPA657 by relaxing the tolerances slightly. Analysis -> Set analysis parameter -> change gmin slightly. Typically gmin can be set as high as 10n, but in this case since I don't have experience the application etc, I set it to 100p.

    Typically when a simulation cannot be run due non-netlisting issue (convergence, op point etc), one can always relax the Vtol absolute, Vtol relative, Itol and Gmin by about 10x or 1000x from the default value shown in analysis -> set analysis parameter (the top 4 on TINA-TI)"

    Here is your original circuit modified per above where AC Analysis can run fine:

    2474.OPA657 Parameters Modified 7_21_14.TSC

    Regards,

    Hooman