• State TI Thinks Resolved
  • Locked Locked
  • Replies 3 replies
  • Answers 2 answers
  • Subscribers 40 subscribers
  • Views 304 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.

TIDA-01168: Question Regarding Output of Boost Mode

Joseph Wong2
Prodigy 40 points
Part Number: TIDA-01168
Other Parts Discussed in Thread: LM5170-Q1

Hello all, 

My group has attempted in creating the power stages of the TIDA-01168 in the TINA simulation software.  We based the schematic off of figure 18 in the TIDA-01168 datasheet.  

Our group was wondering if the output of the boost mode in the following schematic is supposed to be shown as below.  The buck mode of the circuit functions in the continuous mode, but the boost seems to be discontinuous.  We're unsure if the schematic is being done correctly or not.  

Any help or suggestions on what to look for in simulations would be greatly appreciated!

Thanks,

Joseph Wong

http://www.ti.com/lit/ug/tiducs2b/tiducs2b.pdf - TIDA-01168 datasheet for reference

bidirectionalDCDCbuck_2Phase_2-4-2020.TSC

  • 0
    TI__Intellectual 1450 points

    Hello Joseph, 

    Thank you for reaching us on the e2e forum. I am the author of the design and will try to help with your problem.

    I ran the simulation you provided without any problems. That's a good start. Well done!

    I assume that by "discontinuous current" you mean the current flowing to the 48-V supply. The following plot comes from your simulation. I added the AM2 current probe for completeness.

    The behavior you observe is not a discontinuous mode. Discontinuous mode (DCM) occurs when the current (AM2) through the storage inductor (L1) drops to zero. You can see that this does not happen. Also HO1, LO1 signals are complementary. This is not true for the DCM.

    The problem, why you see such madness, is the 48-V supply. You're practically connecting two supplies against each other. The first is the DC/DC converter and the second one is the V5 supply. The balance current between these two is just the result of the dynamic serious impedance of the DC/DC converter. 

    Let's replace the supply V5 by a 2.2ohm resistor.

    As you can see, the output (AM1) is nearly DC current exactly as expected. 

    The LM5170-Q1 device is a current controller. It is intended for energy transfer between two batteries. For this reason, it does not implement an error amplifier for the voltage feedback. If you want to just control the current between two power supplies (with the sink and source capability), you do not need the external error amplifier (opamps). The external amplifier is useful for charging LiIon/LiPol/LiFe/Pb accumulators. These cells require a constant current/constant voltage (CC/CV) charging profile. You can clamp the voltage on the ISETA pin to the required value which sets the charging current for the CC phase. The output voltage set by the reference and resistor divider sets the end voltage for the CV phase.

    I believe you and your colleagues could be also interested in our PowerStage Designer:

    http://www.ti.com/tool/POWERSTAGE-DESIGNER

    This tool is free of charge and works offline. It shows ideal waveforms for various topologies.

    I hope this helps. 

    Best regards, Jiri Panacek

  • 0 in reply to Jiri Panacek85
    Prodigy 40 points

    Hello Jiri, 

    Thank you so much for the information!  I relayed it to my group and we all appreciate the help very much.

    We did have a question regarding the 48V power supply; if we wanted to keep the 48V battery there, would there still be a way to make the circuit work or would we have to replace the supply with a resistor no matter what?  Our adviser recommended us to ask you if we could attempt using an actual battery circuit rather than the given TINA battery component to make it work without putting in the resistor. 

    Again, we're trying to stay similar if not exact to the figure 18 in the datasheet as shown below.

    Correct me if I'm misunderstanding, but those P48V_NF and P12V pins are supposed to be the batteries right?  

    Again, thank you for your help and time for answering our questions!  

    Thanks,

    Joseph Wong

  • 0 in reply to Joseph Wong2
    TI__Intellectual 1450 points

    Hi Joseph, 

    I am happy it helped. Honestly, I always use a resistor and just a one power supply for such simulations. Nevertheless, I found and interesting solution here:

    http://e2e.ti.com/support/tools/sim-hw-system-design/f/234/t/747186?TINA-Spice-battery-source

    You can benefit from the fact that components in TINA can have unrealistic properties. Also, consider adding a series resistor to simulate the internal resistance of a battery. 

    You're right that P12V and P48V_NF go to battery terminals. The latter goes to the filter that you don't need in the simulation (the suffix _NF means "not-filtered").  

    Good luck!

    Jiri