• State Resolved
  • Locked Locked
  • Replies 4 replies
  • Subscribers 63 subscribers
  • Views 953 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.

UCC28704 shut down in simulation

Zhenyu
Prodigy 140 points
Other Parts Discussed in Thread: UCC28704, UCC28710

Hi,

I am simulating a simple 24V/12V converter in PSpice 16.6 using UCC28704. The simulation works very well for 1ms, then the UCC shuts itself down. 

The VDD is always 24V. VS current draw, CS voltage range and VS voltage range are all within limit as shown in the following figure. 

(Green: VS pin current. Blue: VS pin voltage. Red: CS pin current)

One strange thing I noticed is that the current draw of the VDD pin is zero during the simulation even when the chip is working for 1ms. I connected a 10M ohm resistor from the pin NTC/SU to ground. 

Can you advise any reason of the device shutting down please? Thanks.

Zhenyu

  • 0
    TI__Mastermind 26700 points
    Hello Zhenyu,

    The UCC28704 nominal turn-on current at VS is 220uA and the top waveform appears to have peaks maybe just at or short of 220uA. It is difficult to see it clearly. I suggest to try reducing the resistor value which sets this current by about 10% to 25% ( and the corresponding divider resistor on VS for the regulation feedback) to be sure to exceed the start-up current threshold (nominal or maximum).

    I'm not sure how the PSpice model works in detail. Maybe it is modeling the maximum current level (-265uA) for this threshold. I also don't know why it is not showing any VDD current. I'll have to bring these issues to the attention of the modelers.

    Regards,
    Ulrich
  • 0
    TI__Mastermind 19290 points
    Hello Zhenyu,

    The IVdd current is not modeled here: the VDD pin is going through a buffer and thus its current is not modeled.
    Model runs for different combination of Vin(min),Vin(max),Iout(min) and Iout(min) and its correct function was tested for those conditions, namely:
    Vin=100V Rl=2.5 Ohm (2A)
    Vin=100V Rl=1k Ohm (5mA)
    Vin=240V Rl=2.5 Ohm (2A)
    Vin=240V and Iload=5mA
    There are many fault dectection circuitry embeded within the model which might be getting engaged due to the varius conditions in your set up( such as Fault_low Line, Fault_OV, Fault_CS and etc).

    If you have changed the relesed testbench which is based on EVM, please make sure your are within the acceptable limits for the part.
    As a sanity check, run your simulation again with suggested EVM values and see if still shuts down.

    Kind Regards,
    Arash Loloee
  • 0 in reply to Arash Loloee
    Prodigy 140 points

    Hello,

    I changed the voltage sensing resistors RS1 and RS2 to let the VS current to be -300uA, but the UCC28704 still shut down in 1~2ms. There was even one time the chip generated a 10us first PWM pulse during startup, letting CS voltage ramping up to 6V, and shut itself down due to overcurrent. 

    I didn't change the TI pspice model. The sample design coming with the pspice model works very well without shutting down. 

    The flyback converter parameters: 

    Input: 24V dc.

    ouput1: 15V, 15mA.

    output2: 15V, 2mA.

    I checked all the fault protection in datasheet, and checked the voltages and currents of VS and CS pins. There was no fault before the chip shuts down. I suspect that my pspice or my laptop is not stable, and try to simulate in TINA. There is no UCC28704 spice model for TINA. I try to import the pspice model to TINA but run into this error " invalid device: $CDNENCSTART. line #34". I try to use available TINA spice models of UCC28710/1/2/3. All report errors during importing. I guess my best option now is to order a sample and try it. 

    Is it possible that a real (not in simulation) UCC28704 can shut down when no fault can be sensed by CS, VS and NTC pins?

    Thanks.

  • 0 in reply to Ulrich Goerke
    Prodigy 140 points
    Thank you for bring the VS current to my attention. I changed the resistors to set the VS current to -300uA. The chip worked longer but still shut down.

    After manually setting the maximum step size to 5ns, the chip now works perfectly in the simulation, though it took six hours to run a 6ms simulation.