3ph_MMC_Rectifier.qsch (40.4 KB)
Hi all,
does anyone know the cause of the problem in my simulation? when I run it there is always an error, but when I try it in PSIM it works.
For SPICE simulations, I-V discontinuity is one of the major concerns. Firstly, your diode model is incorrect; the diode model name is named “D,” and you should write “.model D D …”. However, it is not recommended to use “D” as the diode model name. Rename it to “Did” or something else to avoid confusion in using a device name D. Diode also as a model name.
With 1 ohm Ron and 1 Gohm Roff, this creates a diode with a steep I-V curve, which poses a challenge for SPICE. This simulation can be run by disabling fastmath (.option fastmath=0) and using 80bits precision math QSPICE80.exe to run the simulation.
Therefore, by correcting the .model for the diode, adding fastmath=0, and removing maxstep from .tran (which is not necessary but speed up simulation), your simulation should run.
Anyway, you should consider not being too aggressive with Ron and Roff for the diode. For example, if you change diode model to .model D D(Ron=1 Roff=10Meg Vfwd=0.7), you can run your simulation with fastmath=1 (QSPICE64.exe).
3ph_MMC_Rectifier-KSK-2311191817.qsch (40.4 KB)
PSIM is a Piecewise Linear (PWL) simulation engine (with a SPICE add-on currently, perhaps?). This type of simulator handles circuit elements with piecewise linear models and is designed to manage discontinuities (or the device modeling is discontinuous). On the other hand, SPICE-based tools like QSPICE handle device non-linearity. In theory, they are quite different, and therefore, for ideal devices, it is usually easier to handle them using a PWL simulation engine. However, QSPICE has been very successful in handling near-ideal devices as a SPICE-based tool. But perhap doesn’t set up devices with extreme discontinuities and stress Qspice to failure.
Thank you sir, the simulation has worked
Thank you sir, I’m still just learning spice simulation, on YouTube no one has added fastmath, trtol and other option functions
I have a command guide in Github, and have section talking about .option and general approach to deal with timestep too small
Qspice/Guideline/Qspice - Command Reference Guide by KSKelvin.pdf at main · KSKelvin-Github/Qspice
1 Like
Thank you Mr. Kelvin
1 Like