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.

LMZ31530 Unencrypted Pspice model on your web

Other Parts Discussed in Thread: TINA-TI, LMZ31530

I tried translating the LMZ31530 unencrypted model on your web to TINA-TI.
However the error message appeared on "New macro wizard", so I couldn't succeed.
Please let me know any idea to solve.

Best Regards,
Kohei Sasaki

  • Sasaki-san,

    It looks like the PARAMS statement is missing from the unencrypted PSpice model. You can fix this by correcting the following:

    IS:

    .SUBCKT LMZ31530_TRANS SENSE+ PGND_0 PGND_1 PGND_2 PGND_3 PGND_4
    +PGND_5 PGND_6 PGND_7 PGND_8 PGND_9 VADJ INH SS_SEL PWRGD
    +PWRGD_PU AGND PH_0 PH_1 PH_2 PH_3 PH_4 PH_5 PH_6 PH_7 V5V
    +ILIM VIN_0 VIN_1 VOUT_0 VOUT_1 VOUT_2 VOUT_3 VOUT_4
    +VOUT_5 VOUT_6 VOUT_7 VOUT_8 VOUT_9 PVIN_0 PVIN_1 PVIN_2 PGND_10 PGND_11
    +PGND_12 PGND_13 PGND_14 PGND_15 PGND_16 PGND_17 PGND_18 FREQ_SEL

    Should Be:

    .SUBCKT LMZ31530_TRANS SENSE+ PGND_0 PGND_1 PGND_2 PGND_3 PGND_4
    +PGND_5 PGND_6 PGND_7 PGND_8 PGND_9 VADJ INH SS_SEL PWRGD
    +PWRGD_PU AGND PH_0 PH_1 PH_2 PH_3 PH_4 PH_5 PH_6 PH_7 V5V
    +ILIM VIN_0 VIN_1 VOUT_0 VOUT_1 VOUT_2 VOUT_3 VOUT_4
    +VOUT_5 VOUT_6 VOUT_7 VOUT_8 VOUT_9 PVIN_0 PVIN_1 PVIN_2 PGND_10 PGND_11
    +PGND_12 PGND_13 PGND_14 PGND_15 PGND_16 PGND_17 PGND_18 FREQ_SEL
    +PARAMS: SS=0 FAST=1 VOUT_SET=0

    The last line should be added so that TINA-TI will create the parameters for use. The VOUT_SET is for steady state operation (set it to your output voltage desired) as is the SS variable (0 for Startup, 1 for Steady State). The FAST parameter will speed up startup when set to 1 (use 0 for full startup[ simulation).

    I am attaching the .TSM file I created once these changes were added.

    LMZ31530_TRANS.TSM

  • Britt-san,

    I tried your attached .TSM file. However simulation was failed.

    Could you check attached .TSC file?

    LMZ31530.TSC

    Best Regards,

    Kohei Sasaki

  • Sasaki-san,

    You may have to adjust the simulation parameters to get the simulation to run. Every circuit is different and the default parameters may not work well with your particular circuit. I have updated a few parameters and the simulation works correctly. Please see the attached .TSC file. The changes can be seen with the Analysis-->Set Analysis Parameters... The changes are marked in red.

    LMZ31530_up.TSC

  • Britt-san,

    I could confirm simulation with your attached file.
    However I couldn't simulation when I changed component value. And after that, I couldn't simulation although I returned component value to original value.

    In fact, I changed resistor value of SS time setting.
    How can I change Analysis parameters?

    Best Regards,
    Kohei Sasaki

  • Sasaki-san,

    I have run all three values with the attached .TSC file. Remember that you have to set FAST to 0 to see any impact of the SS resistor on the simulation. If you leave FAST=1, you will see an impact, but the values will not match the datasheet values. I ran these tests with FAST=0.

    Please note that you can change the Simulation parameters in the Analysis-->Set Analysis Parameters... pop up window in TINA-TI. You may have to select View All if the short list comes up. If the short list comes up, click on the Hand icon and select View All. Here are the settings I used for all three simulations:

    Any time you change the schematic, you may have to adjust the simulation parameters. I have not optimized these parameters for a wide range of use, but found the simplest set that would allow the simulations for the SS resistor to run correctly. Please also note that I changed the length of the simulations for each simulation run from 3m - 61.9K, 5m - 161K, and 7m for 436K.

    1731.LMZ31530_up.TSC

  • Britt-san,

    About the file which you attached in previous answer,

    Output voltage rises up, however output ripple and variation is large level. I think this output waveform is not normal.
    What do you think about this?

    Best Regards,
    Kohei Sasaki

  • Sasaki-san,

    Change the TR maximum time step to 20n, the TR max iteration number to 100, and the DC relative error to 3m.

    Please note that you may have to change these values to get the circuit to converge if there are changes to the circuit.

    You and your customers will need to be able to understand and make these kinds of changes to the simulation parameters. All simulators use a set of simulation parameters that will determine the trade off between accuracy and speed of the simulation.