1
\$\begingroup\$

Can someone tell me why my LTSpice circuit can not work properly? As I am pretty new to electronics I might have done a big mistake that's obvious to more experienced people, however I can't find it. Output inductor current Circuit

I tried to build the circuit shown in this video: https://www.youtube.com/watch?v=a0gmhxZ_Zf0

or here: https://3.bp.blogspot.com/-aDaheyhgUeY/V4KEc3jym1I/AAAAAAAADEk/IEFywbTiy_4csigNK5IVBqbn62cvRKH2ACKgB/s1600/Untitled%2Bpicture78.png

I think the circuit itself should be correct, I maybe just built it wrong in spice. Maybe the position of GND in the secondary Inductor is wrong, I thought technically it should work even without, but Spice wanted me to add GND to prevent floating, so I added where I thought it could make sense. Anyway I also tried the other two possible positions as well without any better results. The values I used for the components are just random values, I tried changing them a lot but couldn't see much impact on the output. I chose the series resistance to be 100mOhm for capacitor and Inductors, just telling because this can't be seen in the schematic and might be important.

I hope someone can help me.

Edit: longer pulses, plot of I1 and I2, started at 0 seconds

\$\endgroup\$
6
  • \$\begingroup\$ Could you explain what sort of supply V1 is - all I see is 40 volts. What frequency is it or have you used DC? \$\endgroup\$
    – Andy aka
    Apr 13, 2020 at 13:29
  • \$\begingroup\$ Yes its 40V DC. The aim of this circuit to convert this DC to AC. \$\endgroup\$
    – janoslon
    Apr 13, 2020 at 13:47
  • \$\begingroup\$ Try making the pulses longer and try plotting L1 ad L2 currents. \$\endgroup\$
    – Andy aka
    Apr 13, 2020 at 13:49
  • \$\begingroup\$ I added an additional simulation with longer pulses and plot of currents of L1 and L2. \$\endgroup\$
    – janoslon
    Apr 13, 2020 at 14:08
  • \$\begingroup\$ OK, it doesn't look like commutation is working. Try making R1 100 ohms and repeat. Also, are you aware that you must stagger the drive pulses in time. You can't have them both activate and deactivate at the same time. \$\endgroup\$
    – Andy aka
    Apr 13, 2020 at 14:29

1 Answer 1

2
\$\begingroup\$

First, you have a few design errors: you are driving the gates of the SCRs directly referenced to ground, as opposed to their G-K. The solution is to remove the grounds for the driving sources and connect them to the cathode of each. Then you are using zero values rise/fall times for the sources. You should know that this is not only a physical impossibility, but LTspice defaults to 10% of (Ton+Toff)/2, so what you really have are 100ns rise/fall times.

Then you are trying to use some thyristors at a 500kHz switching frequency. These SCRs are not MOSFETs, they're only good for low switching frequencies. If you reduce it to, say 1kHz, it will work. How well? That is up to you, the designer. But you should know that, if you only wanted to verify the concept of that schematic, you could have discarded the SCRs and used the builtin VCSW (switches, sw). But maybe you want to see SRCs in action, that's also up to you to know.

With these, here's a reworked version:

test

There is some forced dead-time for the driving pulses (Ton=0.98ms), the "transformer" has increased values and added some series resistance (when coupling is on, there is no more a default series resistance, I never understood why was it decided like this), and I've chosen a different SCR (reminisce of the trials before, didn't bother to change it back). The load is also increased, along with added rise/fall times for the driving sources, lower peak pulse values, and greater series resistance. Please note that I haven't bothered, in the least, to calculate usable values for components, I simply used the never-aging ogling.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.