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.

  • TI Thinks Resolved

THS4522 PSPICE model has an error

Prodigy 105 points

Replies: 4

Views: 1262

Hi,

I have your THS4522 PSPICE model (ths4522.lib, Date: 10/03/2016) and am trying to simulate it in PSPICE.  I also tried LTSpice.  I have found what I believe to be a problem.  PSPICE fails with the error "INTERNAL ERROR -- Overflow, Convert".  LTSpice is a little more helpful:

Fatal Error: Unknown parameter "#IND"
in line:
"b:u2:i0:i32:i5:§eitailmin u2:i0:i32:i5:itailmin 0«::::0» v= -1.#IND *v(u2:i0:vcc_int,u2:i0:vee_int)+ -1.#IND "

I've traced it to subckt GmTail (line 602) which is included as a component starting at line 118:

Line
118 XI5 NET026 NET8 0 NET080 VEE VCC NET043 GmItail PARAMS: Choice=1 Gm=1.98838E-01
119 + ITAILMAX_X1=3 ITAILMAX_Y1=76e-3 ITAILMAX_X2=5 ITAILMAX_Y2=76e-3 ITAILMIN_X2=5
120 + ITAILMIN_Y2=77e-3 ITAILMIN_X1=5 ITAILMIN_Y1=77e-3

Subckt GmTail includes the calculation:

644 .PARAM ITAILMIN_SLOPE =
645 + { ( ITAILMIN_Y2 - ITAILMIN_Y1 ) / ( ITAILMIN_X2 - ITAILMIN_X1 ) }

which of course results in division by 0 since ITAILMIN_X2 = ITAILMIN_X1 = 5.

1)  Could you fix this error so it simulates?

2)  What simulator are you testing with that allows division by 0?

3)  It would be nice to have the option of have a simple model for simulating the AC and transient response (quick simulation, low probability of convergence problems).

Thanks

Eric

 



  • Hello Eric,

    I will have to investigate this. I tried the TINA-TI reference design from the link on the web and I get results for both transient and AC small signal.

    Regards,
    Loren
  • In reply to Loren Siebert 1:

    Loren,

    Thanks, I appreciate the attention to this problem.  As mentioned, I used the model provided for PSPICE ( mentioned here http://www.ti.com/product/THS4522/toolssoftware  and  found here http://www.ti.com/product/THS4522/toolssoftware ) and simulated it in PSPICE and LTSPICE but not TINA-TI.  Regardless, I believe the result of division by 0 in the model is an error regardless of the simulator used.

    I look forward to seeing the resolution to this problem.

    Thanks very much,

    Eric

  • In reply to Eric Boler:

    Hello Eric,
    Thanks for bringing this to our attention. Loren and I do all our testing on TINA-TI and do not have access to other simulators. I have forwarded your issue to the "Tools and Modeling" team who create the SPICE macromodels. They should be able to resolve the error you found.

    On a side note TINA-TI is a little more forgiving on errors and may be defaulting the divide by zero to some "small value". The other simulators are more rigorous and are flagging this error.

    -Samir
  • In reply to Samir Cherian:

    Hello Eric,


    Thanks for your input. Yes, we will fix this. Meanwhile, you can change the Itailmin_X1 = 3 on the text file.

    Regards,

    Herman

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.