A few more measurements this evening.
ST's MDmesh II SPICE models are terrible, and their capacitance plots are characteristically wrong:
I had previously measured this,
I've improved the measurement, using a drain charging resistor (100k), extracting C(V) from the waveform. This covers the whole (500V) range.
Coss:
They don't have a SPICE model for this exact part, but the nearby STP21NM50N (which is a somewhat bigger and less well optimized design, now obsolete) gives a figure of 270pF (time equivalent); SPICE says 389pF. It's wrong by the same amount in the opposite direction. :-)
Using the same extraction on the SPICE model (or simply inspecting the code) yields this:
The parameters used for the fit (red) are, CJO 887.8943 pF m 0.267762 VJ 0.942384 V Clin 124.6118 pF which are in the ballpark of the what appears in the code. I can conclude the extraction method works fine.
I like how the SPICE models proudly proclaim "PARAMETER MODELS EXTRACTED FROM MEASURED DATA"...
How about something they actually got right?
(The drain supply was fun: my benchtop HV supply is a pissy little thing, topping out at about 10mA. Function generator wired as pulse generator afforded the low duty cycle, which turned out to be 30us on, ~100ms off. For you analog afficionados, this measurement would be needlessly difficult without a DSO. Not to mention the trace averaging. Nice!)
Anyway, I measured 32nC total Qg, datasheet says 34. Not bad.
The '21 SPICE model measures 68.3nC, datasheet says 65. Also not bad.
Transfer function: extracted from same waveform. Surprisingly close:
SPICE model not so hot:
I wonder if they stopped tabulating g_fs because they had consistency problems measuring it, or something. Their own plots contradict the 12 S figure...
Tim