• State TI Thinks Resolved
  • Locked Locked
  • Replies 2 replies
  • Answers 1 answer
  • Subscribers 40 subscribers
  • Views 1213 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.

TINA/Spice/LM3488: LTSpice simulation error

user4877549
Prodigy 50 points
Part Number: LM3488
Other Parts Discussed in Thread: TINA-TI,

Tool/software: TINA-TI or Spice Models

I downloaded spice model of LM3488, and import it into LTSPICE XVII for sepic circuit simulation. 

There is error after running the simulation: "unknown symbol: ss". 

What kind of parameter is this "ss" in LM3488? If I add ".param ss=xx" into the script, what value of xx should I use?

  • 0
    TI__Intellectual 2405 points

    Hi user4877549,

    The SS parameter is being used to simulate steady state test condition. As you can see in PSPICE schematic, it is being defined as global parameter with values either 0 (normal startup) or 1(steady state) condition. If SS = 1, internal REF node goes to steady state value of 1.76 directly and at the same time external inductor has current IC = 1*1=1A and output capacitor has voltage IC = 11.5*1 = 11.5V.

    So to conclude, use SS = 0 for normal startup transient simulation. If you are interested in steady state results only, then use SS = 1, but make sure that correct initial conditions are defined on inductor and capacitor as well.

    .SUBCKT LM3488_TRANS AGND COMP DR FA_SD FB ISEN PGND VIN PARAMS: SS=0

    Please let us know if you face any issues.

    Thanks!!

    Best Regards,

  • 0 in reply to Mahavir Jain
    TI__Intellectual 2405 points
    Sorry for the typo, internal reference is 1.26V