LT8228 simulation for boost mode

Hi, ADI Engineer.

I want to ask about how to switch boost mode in LT8228 in the simulation of LTSpice as currently, I want to test and see the simulation of LT8228 in boost mode by using its macro model's test fixture which is Buck 560W (14V 40A) and Boost 480W (48V 10A) Parallel Regulators and the schematic diagram is given below in Figure 1. The simulation is for buck mode actually in Figure 2 but I want to test boost mode.

 Figure 1Buck mode simulation LT8228 Figure 2

Firstly, I tried to switch the V1 to Vout and V2 to Vin like in Figure 3 but then the Vout result is not what it should be which is far lesser in pico voltage value. So, I tried to pull the DRXN pin low to select boost regulation mode after I read the datasheet and I just change the resistor value at UV1 pin to make it lesser than 1.2V so that it can switch to boost mode by just using equation V=IR and Kirchoff Current Law. Still, the voltage output is still the same as the previous one which is pico voltage value like in Figure 4.

  Figure 3

  Figure 4

So, I really need help to do the simulation for LT8228 in boost mode as later I need to develop a boost converter for 4800W (96V 50A) and from what I research that this LT8228 is capable of performing this DC-DC power convertion as it can use Ishare for greater load current and Vout up to 100V. I hope that this question can be replied soon and thank you very much for anyone who responds to this question.

Sincerely,

Zhafran

Third Year Electrical Power Engineering Student

  • +1
    •  Analog Employees 
    on Aug 19, 2020 4:36 PM 6 months ago

    Hi Zhafran,

    My name is Chris Gass and I am the factory application engineer for the LT8228.

    To force boost mode, tie DRXN low. 

    Secondly, your second file is starting the LT8228 with no output voltage. When there is no output voltage, the startup will take longer because the LT8228 first looks to see if V1 side is approximately equal to V2 side. If it is lower, then the LT8228 starts in a start-up mode that will reduce the inrush current to the boost side. So, it will cycle the circuit breaker FETs at a very low duty cycle until V1 is approximately equal to V2. You will need to extend the simulation time signficantly.

    See page 27 and 28 of the datasheet for a more detailed discussion.

    I have attached a file with a simulation example of starting in boost mode with 200 mF of capacitance. It takes almost 70 seconds before boost switching commences. Be sure to download both the .asc and the .plt file. The .plt file will have the format for the plot waveforms. I use the .save command to reduce the number of nodes saved to help save file space as this is a 75 second simulation. 

    Thank you for you time,

    Chris

    LT8228_Boost_Start_Up.zip

  • Thank you very much, Chris. You have a help me a lot. Btw, is it possible for LT8228 to step up 72V to 96V with max load current of 50A as from what I see in the datasheet that LT8228 can do parallelling multiple controller for higher load current but it is possible to reach maximum 50A load current. Anyway, thank you again for your help.

    Best Regards,

    Zhafran

  • +1
    •  Analog Employees 
    on Aug 20, 2020 4:31 PM 6 months ago in reply to Zhafblaze

    Hi Zhafran,

    Yes, it is possible to step up to 72 to 96 V. The part is rated to 100 V. 50 Amps is also possible. Here is a list of things to consider. This list is not all inclusive, just what I can think of at this moment:

    • I don't think you will be able to step up to 96 V from 12 VIN. It is a duty cycle limitation. You need to calculate the duty cycle. It should be possible for 24 VIN or higher.
    • 96 VOUT @ 50 Amps = 4800 Watts. At 24 Vin, that will be about 225 Amps input current if I assume 90% efficiency. If you went with a 6 phase design, your looking at about 37 Amps average current through each phase. You need to calculate peak current to size the inductor properly.
    • Do you need N+1 redundancy? If so, need to factor load current being supported by 5 phases if you do a 6 phase design.
    • Using the ISHARE bus works really well. I have seen current sharing better than 2%. Pay attention to the layout as this trace has to run to all phases.
    • Use the simulation file to assist you in properly choosing the circuit breaker MOSFET. The SOA needs to be closely reviewed.
    • Thermals. What is your thermal plan? A 4800 Watt system that is 90% efficiency means that you have almost 500 Watts of power loss.That breaks down to 62 Watts per phase.
    • There are things you can do to improve efficiency. 90% is just a starting point.

    Thank you,

    Chris