"LTspice 24.0.12 simulates my simple Class-D amplifier, but 24.1.5 fails in transient analysis"

Dear ReneOST ,

Run your simulation with

.options debugtran

and study the resulting diagnostic in the log file. This may help you identify the root cause.

Best Regards,
Mathias

Hello Mathias,

Thank you for your quick response!

I have installed the latest version of LTspice with the debugtran option enabled (see the attached file).test_amp3.log

It seems that the solver has several problems with convergence.

Are you familiar with this information?
Wolfspeed LTspice and PLECS Models

https://www.wolfspeed.com/tools-and-support/power/ltspice-and-plecs-models/ 

I might be experiencing similar issues and may not be able to resolve them.

What is your opinion on this?

Thanks,
René

The TPA3116D2 model uses lot's of non-physical diodes that LTspice has trouble with. This has always been the case and is on our to-do list. You can work around it by changing the diode models at the end to:

.MODEL DDEFAULT D(vfwd=1m epsilon=10m ron=1m)
.MODEL DCLIP D(vfwd=0.8 epsilon=10m ron=1m)
.MODEL DCURLIM D(vfwd=0.8 epsilon=10m ron=10u)
.MODEL DBLOCK D(vfwd=0.8 epsilon=10m ron=10u vrev=7 revepsilon=10m)

You should also not use the UIC option of the .tran command.

Best Regards,
Mathias

Hello Mathias,

Thank you, I got the simulation working. Unfortunately, the output voltage increased from 12V to 150V. By reducing the Ron to 1µ, the output voltage was correct again.

I hope for an update to LTspice 24.1.5 that can properly simulate the original manufacturer model. It’s critical to customize the manufacturer's SPICE model, as I don’t know their component behavior.

I will switch back to 24.0.12 for the moment.

Thank you very much for your support.

Best regards,
René

Hello Mathias,

Thank you, I got the simulation working. Unfortunately, the output voltage increased from 12V to 150V. By reducing the Ron to 1µ, the output voltage was correct again.

I hope for an update to LTspice 24.1.5 that can properly simulate the original manufacturer model. It’s critical to customize the manufacturer's SPICE model, as I don’t know their component behavior.

I will switch back to 24.0.12 for the moment.

Thank you very much for your support.

Best regards,
René

This appears to be an interesting test case. I've made some adjustments, it does run in the upcoming LTspice 24.1.6. However, you have to use the alternate solver and increase the iteration limit:

.options itl4=40

The TPA3116D2 is very challenging for the simulator, because it abuses the semiconductor diode model with an extreme emission coefficient to create diodes with zero forward voltage. This requires a lot more iterations. There are also other numerical issues. I'd say it's a very poor model. Any robust model avoids extreme values for easy convergence.

Best Regards,
Mathias

Hello Mathias,

I'm happy to read your message! I will forward your inputs to the ESA team and my students. It’s also interesting to explore how these problems can be solved and what the key elements are.

I'm looking forward to LTSpice 24.1.6+—maybe it will even be able to simulate very poor models without adjustments! :-)

Thank you very much!

Best regards,
René