I’m trying to use Qspice Model Generator to make a model for my MOSFET. I’ve run into some issues that I’m not sure how to solve. So I decided to ask for advice here.
In particular, my MOSFET is Infineon IPB107N20N3G, the datasheet is available here.
First, I filled in the “Preliminaries” tab with parameters from the datasheet:
As can be seen, these two are not the same. The saturation region of the actual model looks correct, but the linear region I think is not correct, as the slope of the lines near the origin is obviously quite different. During my experiments, I came to the conclusion that the problem here may be that, in the case of this MOSFET, the default values for the Rext / (Rext + Rchannel) and Rd / (Rd + Rs) fields do not work very well. In particular, I noticed that the graph becomes more accurate if you change these fields like this:
However, the transconductance value of the model (Kp) then becomes 651, which is kind of far away from the one specified in the datasheet, which is 141
If anyone has any ideas on how to solve this problem and how to proceed, I would be happy to hear..
You can refer to my Device Guideline, where there are two pages in the MOSFET section explaining the relationship between KP and VTO in a pure textbook model through formulas. If all other parameters are removed, KP / 2 represents the drain current at Vgs = VTO + 1; this relationship is purely derived from the formula.
However, in an actual model that includes Rs, Rd, and other parameters, when discussing transconductance (gfs), it becomes a resultant value not inherent to the die but influenced by the package etc… Therefore, your concern no longer revolves around whether KP equals the datasheet gfs.
gfs = delta Id / delta Vgs, which is the slope of Id vs Vgs characteristic, and in simulation you are in general measure it at about 1V higher than VTO.
By putting two cursors into the model you generated, gfs of your model is about 150A/V, with other parameters contributed now.
Thank you very much for your reply and for trying to help!
I tried to look at your guideline that I found on GitHub, but to be honest, I didn’t understand much of it. There are too many concepts that I’m not familiar with. I’ll try to figure it out if there’s no other option, but it seems like a pretty complicated topic.
So, it turns out that the model’s Kp is not exactly the same as the transconductance from the datasheet, right? But if you try to estimate the actual transconductance for this model generated by the Model Generator, it turns out that the number is almost equal to the transconductance from the datasheet. Am I correct? Does this mean I’m on the right track?
Also, what do you think of my approach overall? I.e., I discovered that the model behaves incorrectly in the linear region, and decided to increase the Rext / (Rext + Rchannel) field. Is this the right approach?
Yes, that Kp is a model parameter and you only get that value in ID vs VGS measurement from model without any external parameters like drain resistance, source resistance etc… MOSFET with package and leads, that change its characteristic when measuring these parameters externally. Datasheet transconductance fgs is a value measured “externally” too.
Referring to the model generator HELP, these are recommended values only. Mike explained in his Qspice seminar that these values are generally effective and can work from his experience. Modeling is an experience to change things that you get a model best fit to what you measured, so, you are expected to change parameters with a model you not feeling close enough to your measurement.
In the case of the model generator matching the data sheet characteristic curve, is it better to accept the model results even (as per this discussion) they don’t match the linear portions of the curve or alternatively, “trick” the model generator by entering data points not exactly on the data sheet curves such that the test results match the datasheet?
@KSKelvin Thank you very much for your help and advice! I also see that you are doing a lot for the QSPICE community, which I think is very important and useful work, for which I am also grateful.
Just in case anyone else needs a model for this MOSFET (Infineon IPB107N20N3G), I am publishing the best one I was able to generate. To create it, I used values from the datasheet, and I also increased the Rext / (Rext + Rchannel) to 0.95:
