• State Resolved
  • Locked Locked
  • Replies 8 replies
  • Answers 2 answers
  • Subscribers 63 subscribers
  • Views 961 views
  • Users 0 members are here
Support feedback
Options
Options
Related

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.

TPS7A39: TPS7A3901 P-Spice simulation

RAHUL JHA
Prodigy 210 points
Part Number: TPS7A39

Hi Everyone,

I am working on re-engineering project in which I came across the above mentioned part no. We are using this part to convert +/-15 V into +/-9V.

By following the design recommendation mentioned in datasheet, I started the simulation in P-spice tool provided by TI.

Surprisingly I have found that the graph obtained for OUTP and OUTN are showing +/-9 V which is correct but at the OUTP and OUTN pin in circuit it is showing voltages around +3.782 mV and -6 mV respectively.

I don't understand how this can happen. Are these value (+3.78 mV and -6mV) are the output voltages at corresponding pins or it is something else.

I am attaching two images one for circuit and other is a graph.

Please help me out here.

a graph  for your better understanding.

  • 0
    TI__Mastermind 37065 points

    Hi Rahul,

    It looks to me like the negative nets are not actually tied together like we think they are.
    I would tie a physical wire from -9V output to the TPS72301 input pin.
    If this quick check does not solve the issue, please attach your spice model to this forum so I can download it and review it on my end.

    Thanks,

    - Stephen

  • 0 in reply to Stephen Ziel
    Prodigy 210 points

    Hi Stephen,

    Thanks for your kind reply. I did what you had asked for but still facing the same issues. 

    I am attaching my spice simulation file (.DSN) for your reference. Please look into this and help me to find out the problem.

    Thanks,

    Regards,

    Rahul

    LDO spice simulation.zip

  • 0 in reply to RAHUL JHA
    TI__Mastermind 37065 points

    Hi Rahul,

    I received the schematic but there is only the .DSN file.
    Can you zip up the entire project and send it over?  That way I am using the exact same models that you see on your end.
    There should be a way to archive the project which will have all of the necessary files for me to open.
    If you go to File - Archive Project, then archive the files, you can then attach that zip folder to this forum.

    Thanks,

    - Stephen

  • 0 in reply to Stephen Ziel
    Prodigy 210 points

    Hi Stephen,

    As per your request I am attaching the whole project file. Hope you get what you need.

    Regards,

    Rahul

    New.zip

  • 0 in reply to RAHUL JHA
    TI__Mastermind 37065 points

    Hi Rahul,

    I can replicate what you are describing.  It turns out this is operating how Cadence intends for it to behave.
    The issue stems from how Cadence calculates the operating point.  The bias voltage measurement results from the operating point calculation, which is always run prior to any simulation.  The bias voltage measurement is not always the steady state output voltage for the DC converter.  Even when I use the .IC or nodeset parameters, I cannot get this value to change in the simulation.  When I zoom into the results such that all I see is 0 seconds to 5ms, I can see the output change from close to 0V to the steady state voltage.  The actual value at 0 seconds is the reported value in the bias voltage measurement. 

    This brings up a second issue.  The way the original modeler built the spice model causes the simulation to always go from 0V to a steady state output voltage.  In many simulations if you feed the circuitry a DC voltage source, the output of the circuitry will simulate as a steady state value as well. That is not the case with this model.  It will start at 0V then ramp to steady state output voltage regardless of whether you feed it with a DC input or not.

    I hope this clarifies what you are seeing.  The transient simulation is correct and the bias voltage measurement is providing the DC operating point for the simulation, not the steady state output voltage.

    Thanks,

    - Stephen

  • 0 in reply to Stephen Ziel
    Prodigy 210 points

    Hi Stephen,

    Thanks a lot for your detailed explanation. The same thing I also observed when I tried with transient analysis. According to you there are some problems with spice model because of which it is not showing the steady state values. And whatever the value I am getting is corresponding to 0 second.

    As I am getting the correct value of OUTP/OUTN in the graph so I can assume the simulation is correct and there is no need to change anything. Please acknowledge this statement. It will help me to move forward and close this case.

    Is there any way to fix this things (spice model)? 

  • 0 in reply to RAHUL JHA
    TI__Mastermind 37065 points

    Hi Rahul,

    I would say there is no issue, per se.
    Cadence reports the measured BIAS values at time = zero in accordance with the .OP statement. 
    There is no way to modify this that I know if, it gives you the initial condition or initial operating point of the circuit.

    The simulation was designed to perform a startup regardless of DC input supplies.

    So the simulation is correct and you do not need to change anything.

    Thanks,

    - Stephen

  • 0 in reply to Stephen Ziel
    Prodigy 210 points

    Hi Stephen,

    I think my issues is resolve now. Thanks for helping me out here. I really appreciate it.

    Regards,

    Rahul