• State Resolved
  • Locked Locked
  • Replies 3 replies
  • Subscribers 37 subscribers
  • Views 8963 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.

LM431 SPICE Model

Chew How Lim
Prodigy 20 points
Other Parts Discussed in Thread: LM431, TINA-TI, TL431

Good day

May I know who can help me to get SPICE model for LM431?

There is no SPICE model available at TI website for LM431.

http://www.ti.com/product/lm431

Thanks

  • 0
    TI__Mastermind 41310 points

    Chew How Lim,

    You might want to consider using the TL431. It has HSpice, PSpice, and TINA-TI models available. The TL431 is very similar to the LM431 and the modes should behave similarily to the LM431.

    Britt

  • 0 in reply to Britt Brooks - Online Design Tools
    Prodigy 20 points

    Thanks for the reply Britt.

    I look into the TL431 SPICE model and it consists for diodes, resistors, current source to model the TL431 zener shunt regulator. 

    Based on the TL431 data sheet, the zener accuracy is from 2.483V (min) 2.495V(typical) and 2.507V(max).

    May I know if the SPICE file able to simulate the worst case analysis across the zener tolerance range?

    As I run my simulation, I only able to obtain one curve (typical reading).

    I am looking for the output variance contributed by the TL431.

    Is this achievable with this TL431 SPICE model?


    .SUBCKT TL431 7 6 11
    * K A FDBK
    V1 1 6 2.495
    R1 6 2 15.6
    C1 2 6 .5U
    R2 2 3 100
    C2 3 4 .08U
    R3 4 6 10
    GB1 6 8 VALUE = {IF(V(3,6)< 0 , 1.73*V(3,6) -1U , -1U)}
    D1 5 8 DCLAMP
    D2 7 8 DCLAMP
    V4 5 6 2
    G1 6 2 1 11 0.11
    .MODEL DCLAMP D (IS=13.5N RS=25M N=1.59
    + CJO=45P VJ=.75 M=.302 TT=50.4N BV=34V IBV=1MA)
    .ENDS
    *$

  • 0 in reply to Chew How Lim
    TI__Mastermind 41310 points

    Chew How Lim,

    The voltage output is set by the V1 value of 2.495V (which is the nominal value). Based on the datasheet, you could change this value to either the min or max value to do a weak/strong corner simulation which may give you insight into your circuits' dependence on the TL431 output voltage. The SPICE models created are only for the nominal condition and do not properly represent a worst case analysis.

    WCA models are extremely time consuming and expensive (if done properly) and normally require information about the application and how the IC is being used before the WCA model is created. The models provided in our product folders are not intended for this use. The intent of the PSpice models provided are for design and performance verification.

    Britt