Tonight I left running the simulation and this morning I found this error:
Unable to meet integration tolerances without reducing step size below smallest value allowed (3.55271e-15).
This is my first time using SPICE models, so I may have made some improper settings regarding the MOSFET. However, this error still persists after I carried out troubleshooting, and I am at a loss as to how to resolve it. Could you please help me check the issue? My PLECS file is attached below.
Hello, I would classify this as an application issue. If we run your circuit, the FET currents exceed 200 A, while the device’s pulsed drain current limit is 130 A. You will also note the junction temperature rises above 400 °C before the simulation stops. In this regime the SPICE model is being driven well outside its valid operating range, which leads to non-physical behavior and convergence issues (e.g., time step collapse).
I would recommend using ideal PLECS models first to estimate the expected current levels and then selecting an appropriate device based on those results. Or you can modify your circuit to respect the capabilities of the device.
Thank you very much for your guidance. The simulation works smoothly after I replaced the device model.
I wonder if I could consult you about another issue. I am trying to simulate a three-phase LLC converter with the SPICE MOSFET model in PLECS, yet I have noticed that the simulation speed is quite low. Even the PWM waveforms take more than a minute to display. I would greatly appreciate it if you could share some possible reasons behind this slow performance. My three-phase LLC simulation model is attached here.
A big driver of the slow simulation speed is the 1e9 ohm resistor on the secondary side of the converter. This creates a very small time constant which PLECS must model. Same with the 1e6 resistances for the transformer core loss resistances. For me, even dropping the secondary ground reference resistance to 1e6 accelerates the simulation quite a bit. Sometimes it’s advantageous to add a parallel capacitance to ground as well. Eventually the waveforms in this model start to look kind of off, which I think is due to the underlying SPICE model. Starting simpler with a basic LLC might be a good starting point before trying to simulate the larger more complex system.
Although likely not the main driver for a slow simulation speed in this case, there is much room for improvement on the controls implementation. Everything is based around a 1e-7 sec step size. You should just use the library block for PWM modulation (or you can also use the PWM blocks from the Target Support Packages which have even more advanced features applicable to offline simulation). You also fixed the max step size of the solver to 5e-7 forcing very small steps, which can be relaxed to 1e-3 or higher in a properly implemented model.