• State Resolved
  • Locked Locked
  • Replies 18 replies
  • Answers 5 answers
  • Subscribers 64 subscribers
  • Views 633 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.

Original question:

TPS7A39: TPS7A39 Simulation fails to converge when loaded

LM337: No output from current regulator when used in simulation with TPS7A39?

Roger Brooks
Prodigy 50 points
Part Number: LM337
Other Parts Discussed in Thread: , TPS7A39, , LM317

I am trying to add current limiting to the previously submitted design by adding LM317 and LM337 regulators in current-limiting mode.  Both simulate nicely standalone but don't deliver usable results in combination with the TPS7A39.  Ideally I would like to place them inside the output feedback loops of theTPS7A39 for better voltage regulation, but neither this approach nor placing them before the TPS7A39 delivers any usable simulation results at all.  Depending on the simulation parameters, the simulation fails to converge, never finishes or shows kilovolt spikes at the negative input of the TPS7A39. The only configuration that comes close to delivering believable results is putting the current regulators after the (closed loop) TPS7A39 voltage regulator.  However, the LM337 shows no output at all in this configuration, even though it shows a normal output when fed by an ordinary rectifier / capacitor circuit instead of the negative output of the TPS7A39.  I am using the LM337-N from the included PSPICE for TI library, although the finished design should use the LM337L.  The attached project archive should include 3 different designs, but I am uncertain about the relationship between projects and designs. I have also attached a screenshot of the simulation results showing a flat line for the output of the LM337 (purple) in contrast to the expected output delivered by the LM317 (yellow).

Design5-2023-11-11T18-14.zip

P.S. Here is a screenshot of the schematic as insurance:

  • 0
    TI__Mastermind 34785 points

    Hi Roger,

    I am reviewing your question and will reply back within 2 business days (hopefully before then).

    Thanks,

    Stephen

  • 0 in reply to Stephen Ziel
    TI__Mastermind 34785 points

    Hi Roger,

    I have both of your latest simulations running and converging but I needed about an hour to find the missing libraries as my version of PSpice apparently did not have them all.  I'll look further at this tomorrow.

    Thanks,

    Stephen

  • 0 in reply to Stephen Ziel
    TI__Mastermind 34785 points

    Hey Roger,

    I responded to your other E2E thread and I think the issue is resolved.  But if you are still seeing some issues, please reply back and we'll continue to work through them.

    Thanks,

    Stephen

  • 0 in reply to Stephen Ziel
    Prodigy 50 points

    Hi Stephen,

    Unfortunately, this approach is still giving me trouble. I am interested in using the TPS7A39 instead of LM3x7s for voltage regulation as the higher dropout voltage of the LMs leaves me no margin for component tolerances

    For the time being I have given up on putting the current limiters inside the TPS7A39's feedback loops.  That approach would probably subject the TPS7A39 to too much power dissipation, considering that the circuit will be used in a small enclosed space without ventilation.

    Instead I am trying to  place the current limiters before the TPS7A39 in order to get better voltage regulation.  Unfortunately, I am unable to get a simulation. I have tried the various tricks you have suggested in other threads:

    - turning on all autoconverge options

    - increasing the speed level to 5

    - adding a 100us maximum step size

    This is the result:

    In the above dialog, I tried to reduce GMIN to 1e-10 based on the advice in this slide deck, but the change didn't "stick".  After clicking "OK & Resume Simulation", the dialog reappeared with the old value of GMIN (1e-12).

    Except for CSHUNT (which isn't presented in that dialog) the other values had already been relaxed beyond Ian Williams's recommendations, presumably by autoconverge. Nonetheless, I then tried using all of Ian's recommendations (including CSHUNT=1e-15) in the projects simulation profile. This enabled the simulation to finish, but it produced the kilovolt spikes I have mentioned elsewhere:

    I have attached an archive with all options checked, in hopes that will save you the trouble of searching for libraries:

    PowerSupply1-2023-11-18T09-21.zip

    Thanks again for your help!

    Roger

  • 0 in reply to Roger Brooks
    TI__Mastermind 34785 points

    Hey Roger,

    I'm also having issues with Cadence simulating this circuit - I think it's a tool issue somewhere but I'm unable to locate the right knobs to fix this.  I would recommend simulating portions of the circuit (current limiters by themselves, then the LDO with a model that emulates the current limiters as Vin, etc).  Then use EVM's to validate the concepts in the simulations. 

    You may also want to explore another method of limiting the load current as I'm unsure if the current limiter in front of the voltage regulator will work properly.  You can sense the load current using series sense resistors and current sense amplifiers and feed back the result to the FB pin of the LDO.  This may act as a more controlled method to controlling the current instead of choking off Vin from the regulator. 

    Thanks,

    Stephen

  • 0 in reply to Stephen Ziel
    Prodigy 50 points

    Hi Stephen,

    Thanks again for your help.

    I would have liked to have used the TPS7A39 to control current as well as voltage, but didn't find a good  way to do that. The designs I found require the current sensing resistor to be inserted between the load and ground, which isn't feasible in my case, because C12 and C13 are actually stand-ins for Li-ion batteries which this circuit is supposed to charge.  The batteries need to be ground referenced to drive their load, which in turn is referenced to the same ground as the AC input.

    Also, I was afraid that the TPS7A39 might get too hot if it had to carry the entire voltage drop.  Designs that "choke off Vin from the regulator" to limit current are not uncommon (see Figure 22 on p. 8 of the OnSemi LM317 datasheet, or the alternate design we have been discussing).  Other than the simulation problem, is there a downside to this approach I may have missed? Any suggestions you may have for how to  add current regulation to the TPS7A39's FB pins would be welcome.

    Regards, Roger

  • 0 in reply to Roger Brooks
    TI__Mastermind 34785 points

    Hi Roger,

    Have you considered the lithium ion charging IC's that TI manufactures?

    https://www.ti.com/power-management/battery-management/charger-ics/products.html

    Thanks,

    Stephen

  • 0 in reply to Stephen Ziel
    Prodigy 50 points

    Thanks for the suggestion, but I failed to find anything appropriate in your list.  In fact I had already considered this possibility before resorting to the designs you see, without finding anything suitable. The batteries in my design are to provide a symmetric bipolar DC power supply to low-power portable audio electronics housed in very small spaces. The power supply needs to fit on a roughly 1x2 inch PCB and the current should be limited to approximately +/- 80 mA.  Each polarity uses two cells of 140-250 mAh in series to provide supply voltages in the range of +/- 6-8VDC.  The charging circuit is not powered when the audio electronics are in use, but the physical configuration doesn't permit the charging circuit to be disconnected, which is why the regulators are protected by blocking diodes at the output instead of by shunt diodes as recommended in the application notes.

  • 0 in reply to Roger Brooks
    TI__Mastermind 34785 points

    Okay thanks Roger. 

    During turn on, the TPS7A39 will charge up Vout to try and match the turn on of Vref.  This will result in inrush that may exceed the current limiters resulting in a brownout condition on Vin.  This causes an "oscillation" on Vin and the TPS7A39 may never turn on.  The 2.5 ohm in front of the current limiters may also impact the ability of the LDO's to turn on.  I was seeing some of this in the simulation but convergence issues with the software prevented me from finding a good solution, if one exists.  You can try increasing the NR/SS capacitor to slow down the turn on of the TPS7A39, but you'll need a large capacitor to really slow down Vout.

    A more common approach is to control the FB or ADJ pin of the LDO with an external current monitoring circuit.  This way the LDO can still turn on but in a controlled manner without the issues with brownout on Vin.  By having a current limiter circuit control the FB or ADJ pin, you eliminate concerns that brownout may occur on Vin causing the LDO to turn off, then on, in an oscillatory manner.  Instead the current limiter will just force Vout to droop until the load is removed then Vout will go back into regulation.

    We don't have a reference design or application circuit that perfectly fits your application, but hopefully this general guidance can help.

    Thanks,

    Stephen

  • 0 in reply to Stephen Ziel
    Prodigy 50 points

    Hi Stephen,

    Thanks for the explanation.  I take it that the same reservation would not apply to the alternate design using only LM3x7s. My only reasons for trying to use the LM7A39 are that I appreciate the integration of a tracking bipolar supply in one device and I could run into tolerance issues with the exclusive LM3x7 design: it just barely manages +/-8V with nominal values, component tolerances might cause problems.  The 2.5 ohm resistor is just to model the ESR of the plugin tranformer I‘m using.

    I‘ll spend a bit more effort on figuring out a way to implement the current control with the TPS7A39.

  • 0 in reply to Roger Brooks
    Prodigy 50 points

    Based on your explanation of the potential problem with current limiting the voltage regulator input, I have gone back to the version I first wanted, with current limiters inside the voltage regulator's feedback loops.  This isn't as elegant as using analog feedback logic to get the TPS7A39 to do all the work, but it should at least theoretically have the same effect.  As in other reported cases, the simulation looks fine for the positive side but delivers 0VDC negative output, even after applying all of the tweaks to the simulation profile mentioned above. Aside from the flat negative output, the simulation shows nasty power spikes at the startup of the TPS7A39. Are these artifacts of the simulation failure, or do they indicate a problem similar to the one you anticipated for the topology using current limiters before the TPS7A39?

    design5-2023-11-21T21-51.zip

  • 0 in reply to Roger Brooks
    Prodigy 50 points

    I tried adding a primitive current control circuit using the TPS7A39 FB pins (attached) the BJTs should shunt current around the trimpots when their Veb threshold voltage is reached, limiting output current to around 70mA. The simulation claims to complete, but delivers an empty output screen: not even the AC input voltage is shown.  According to this paper, Qbreakn and Qbreakp should have editable SPICE properties, but I didn't find any with "Edit properties". What am I doing wrong?

    powersupply2-2023-11-22T08-23.zip

  • 0 in reply to Roger Brooks
    TI__Mastermind 34785 points

    Hey Roger,

    I was able to run the latest files you provided and show that the positive rail seems to simulate the way you described.  I've added a pulsed current source to act as a load on the positive output, and you can clearly see that the positive rail enters current limit as this current source ramps up (see the red waveforms).  I tried emulating this on the negative rail but I ran into convergence issues, and I ran out of time today before I could resolve them.  However the concept may work as demonstrated by the positive rail results.

    The BREAK spice models have editable properties as you mentioned.  You should be able to right click the component, go to "view pspice model" and it will take you to the breakout.lib netlist.  In prior versions of Cadence you could also use the Model Editor to change the netlist, but I don't know if your version of Cadence comes with this.  Regardless you can edit the spice parameters but it's a good idea to save the new library with a new file name so you don't accidentally overwrite the breakout.lib file, which may be used by other simulations on your machine that you don't want to modify accidentally.  You may then have to import the new .LIB file you create and generate the component.

    Thanks,

    Stephen

  • 0 in reply to Stephen Ziel
    Prodigy 50 points

    The transistor parameters aren't really critical: any complementary pair should do, but thanks for telling me how to find them. Using your parameters I too get a simulation, but it still shows large power spikes during the startup of the TPS7A39. Do you have an explanation?
    Also, the steady state Pd of the regulator is also likely to be too high.  At an output voltage of 5V (about what the batteries would be when discharged) Pd is well over 1W.

    powersupply2-2023-11-23T12-22.zip

  • 0 in reply to Roger Brooks
    TI__Mastermind 34785 points

    Hi Roger,

     In general, the large voltage spikes are simply an issue with the simulator finding the "right" solution and hopefully we can change the simulation settings to fix this. Please give me 2 more business days to review this and respond.

    Thanks,

    Stephen

  • +1 in reply to Stephen Ziel
    TI__Mastermind 34785 points

    Hi Roger,

    Thanks for your patience. I can simulate the latest copy you have provided without any issue.  The initial power spike comes from the initial moment the LDO charges up the output capacitors.  You can use the current probe to probe onto various nets to see where this is coming from, as a troubleshooting aid. 

    I noticed that PSpice did not converge and set Vout = 0 for either converter during initial turn on, which likely made this power spike worse than it otherwise would be.  I used the IC element to set the initial condition of both Vout to 0V, then set the maximum step size to 1us.  You probably cannot run the entire simulation this way without convergence issues but you can zoom in on this artifact just fine.  Now the spike looks more reasonable.

    Thanks,

    Stephen

  • 0 in reply to Stephen Ziel
    Prodigy 50 points

    Stephen,

    Many thanks for your exhaustive analysis! Since the output capacitors are those recommended in the datasheet, I assume that the LDO regulator cab handle them.  However, due to the Pd shown in the simulation, I plan to go back to a version using LM3x7s for current regulation, in order to spread the Pd over different packages.

    Thanks again for your help!

    Roger

  • 0 in reply to Roger Brooks
    TI__Mastermind 34785 points

    Okay thanks Roger - I'll close this ticket but let us know if you need anything else.

    Thanks,

    Stephen