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/PMP30104: Simulation error

Part Number: PMP30104
Other Parts Discussed in Thread: TINA-TI, TPS40210, , TLC272

Tool/software: TINA-TI or Spice Models


I am Trying to run the schematic in Tina, the output voltage produced is in mV is not as specified. I am attaching TSC  file. SEPICBoost.TSC

  • Hello Preethi,

    I made some modifications on the schematic and now it's running. It takes long time, so I am not sure it is now working fine. Also the main FET T4 should be selected from a better characteristics.

    Here is a list of modification I made:

    C12 from 1 uF to 100 pF

    R13 from 210 mOhm to 20 mOhm

    R6 from 100 KOhm to 260 KOhm

    Most important: the power supply for OP2 was reversed: please connect pin 8 to net J1 and pin 4 to ground.

    Please let me know if it now runs.

    Best regards,


  • Sir,

    I made the mentioned changes when the transient analysis is carried output boost voltage is only 50V for 12V input.

    and in DC analysis gets an error operating point not found U1.X_TPS40210_OSC_U30.D_D10.

  • Hello,

    Thanks for your response

    I made the mentioned changes when the transient analysis is carried output boost voltage is only 50V for 12V input.

    and in DC analysis gets an error operating point not found U1.X_TPS40210_OSC_U30.D_D10. 

  • Hello Preethi,

    Can you please attach the latest simulation file you are working on?



  • Sir,SPBOOST150.TSC

    Please find the attach TSC file, MOSFET mentioned in PMP30104 is of rating 150V and drain current 21A (BSZ520N15NS3) similar characteristics is not available but I have changed the parameter.

    and also there is no library file of TPS40210 shows empty.

  • Hello Preethi,

    I saw in the simulation file the VCC of OP2 was not connected.

    I run the simulation and I am not sure our model of TLC272 really manages rail-to-rail input (even negative), therefore I supplied both op-amps with +5V and -5V.

    I also reduced the current sensing resistor R13 to 5 milli-Ohm to avoid triggering the overcurrent on main controller.

    Changed also C11 to 470nF. The main FET is now IRFP450, because the original one had too high Vgs(threshold).

    Now the converter looks running a bit smoother, but still, after the soft start is expired, I get shut down in  the controller (the COM pin goes low).

    Can you pleaseSPBOOST150_06_12.TSC check also from your side if you have the same behavior?



  • Hello Sir,

    Thank You Sir, for the response.

    I have run the simulation, the same error of com pin voltage goes low at 2.3ms and after certain delay goes to high remain in the high state for 0.3ms then again goes to low state.

    as the circuit is designed for 400V output voltage the simulation output results getting around 150V only but the circuit runs smoother.

  • Hello Preethi,

    Please find attached the latest simulation file I run.

    Now it reaches 410V and it's stable.

    Before reaching this point, I thought it would be easier to remove the UVLO circuit, connected to DIS/EN pin and the Vout switch (that was not driven).

    Nothing changed, and after making some further simulations, I realized that the currents trough multiplier Schottky diodes where too high, and showing also heavy reverse current. Then I saw that these diodes are huge (80A) and only 45V rated, while I used 150V 1A Schottky.

    I didn't find this diode in the library so I replaced them with 1A 100V diodes (which are still sufficient) and now the simulator runs and Vout reaches 410V.

    Please consider that if you run a simulation with bigger output capacitor, you have to fine tune the current loop, otherwise it will be unstable.

    If you want, you can add again the UVLO circuit, and the section that changes Vout.

    Just let me know if you need further help.

    Best regards,


  • Hello

    Thank you, Sir, I have run the simulation file and getting output results smoothly.

  • Hello Preethi,

    I am glad to know that your simulation is running smoothly.

    Just let me know if you need further support.

    Best regards,