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

Question

Hello 
 I successfully simulated a Class-D amplifier with the TPA3116D2 IC using LTspice 24.0.12. 
 I only had to switch the solver to GEAR to achieve convergence in the transient simulation. 
 After updating to LTspice 24.1.5, I can no longer find a setting that allows a successful transient simulation. The simulation stalls after just a few microseconds. 
 
 Can you help me? The simulation setup can be found in the ZIP file. 
 class-d-audio-amp-test_with_ltspice_24.0.12.zip

mborn · Answer

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

mborn · Answer

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

mborn · Answer

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

Popular Forums

Product Forums

Application Forums

Design Center Forums

Highlighted Webinar

Places

Libraries

Latest Webinars

Challenge Yourself!

What's Brewing

Places

Resources

Highlighted Blogs

Latest Blogs

ADI Blogs

Visit ContentZone

Featured Content

View Content By Industry

View Content By Technology

Products Mentioned

Related Questions

Follow-up on TPA3116D2 Simulation in LTspice 0

Thread Details

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