0

I am working on LTSpice on a project which consists in transferring energy from a PV panel to a load through a transformer, using a controlled bridge at the primary and a diode rectifier at the secondary side of the transformer. I am trying to retrieve the I-V characteristic of the PV panel after the diode rectification, but for that to work it seems that I have to combine a DC sweep analysis (to get the I-V characteristic) and a time analysis (to have the AC square-wave signal that is exchanged between the primary and the secondary side of the transformer).

Is there any way to realize such analysis? Or am I mistaken in what I am trying to accomplish?

I will add a picture of the circuit below.

enter image description here

winny
  • 13,064
  • 6
  • 46
  • 63
Sander
  • 1
  • 1
    Sounds a little odd since a DC sweep is going to open up your smoothing capacitor at the end, not mentioning all your other capacitors. Is R1 your load? Are you trying to see the behavior of `Vout` under various loads? If so, you can `.param` the resistance value and sweep it over a range using `.step`. Alternatively, you can replace the resistor with a current source and set it to PWL to sweep it under various currents changing over time instead. Probably a good idea to flag it as `load` too (checkbox on the right side of the properties window). – Ste Kulov Jun 04 '22 at 04:14
  • @SteKulov I am trying to plot the I-V characterisitc of the PV panel, retrieved after the diode rectifier, for different phase shifts of the control signals in and in2. – Sander Jun 04 '22 at 07:11
  • 1
    But...with the load attached? What's the purpose of finding an I-V curve with R1 already there? Also, what information do you expect these I-V curves to tell you? – Ste Kulov Jun 05 '22 at 05:59
  • The load doesn't have to be attached, it was just a tool for the previous simulation... These curves will tell me which phase shift of the command signals will yield the highest MPP – Sander Jun 05 '22 at 06:30
  • Thx for the info. Okay, so you can only get I-V if your circuit doesn't depend with T. One way to accomplish this is to create a DC equivalent for your circuit at the load (e.g. Thevenin equivalent). Another way is if you assume you are in steady state and can't get nudged out of it with different load currents. Then you can do what I said above and after your circuit stabilizes you can use a PWL current source, something like `PWL(0 0 +1 0 +1 1)` which will wait 1 second first, then sweep up to 1amp during another second of time. Then you can probe `Vout` to get the V for those I's. – Ste Kulov Jun 05 '22 at 06:43
  • If your circuit needs some stabilization time after you adjust the current at the output, then you need to wait a bit and pause for that stabilization time to occur within your PWL. Then when you plot you'll have to take manual datapoints where those "stairsteps" occur, or you can probably automate something using the `.meas` command to spit out a table you can plot directly. – Ste Kulov Jun 05 '22 at 06:44
  • One last tidbit is you should really use actual diode models for your diodes instead of the one with default parameters (i.e. just having the `D`). This will really affect your output, especially at the higher currents. – Ste Kulov Jun 05 '22 at 06:51
  • @SteKulov Ok, thank you, I will try your solution asap. Do you have any recommandation on the diode model that I should use? – Sander Jun 05 '22 at 13:21
  • Whichever matches the diode you actually intend to use in real-life. Or is this a simulation-only exercise? If so, still use something that matches your application specs (max current, reverse breakdown, etc.) even if it's just one of the built-in models within LTspice. If you're rectifying square waves (or really fast sine waves), I would look at something that has the `Vp` parameter defined. That makes sure the reverse recovery effect is properly modeled. – Ste Kulov Jun 06 '22 at 02:04
  • @Sander I see missed this one. Your best bet is to make an averaged model of your converter and then use `.TRAN` analysis with either `.step`, or some `PWL` sources (input or output, as Ste says). Otherwise, you need to ensure that whatever variation you have needs to be much less than the lowes pole of your converter (the output filter), so that the transients come out as clean as possible, and using that with a switching converter is bound to hurt your clock. You might reduce that by using VCSW+D instead of VDMOS (BTW, the VDMOS have built-in antiparallel diodes). – a concerned citizen Jun 10 '22 at 19:29

1 Answers1

0

If this was not a resonant converter, it could be done with reasonable accuracy using a DC sweep (just make one side of the H-bridge 100 % on, and eliminate the core part (2 *20 mH -- connect VL1+ to VL2+ etc.) of the transformer), but since it is a resonant converter, the losses in the switches will depend on the resonant currents and so can't be easily approximated like that.

jp314
  • 18,395
  • 17
  • 46
  • So if I want to retrieve the I-V characterisitc of the PV panel at the output of the rectifier for different phase shifts of the command signals in and in2 it is not possible? Since I have to always set one of the side of the H bridge ON all of the time? – Sander Jun 04 '22 at 06:55