SCT070HU120G3AG MOSFET Model

QSPICE
1

Hello QSPICE Community,

I’m experiencing a convergence issue with a specific third-party MOSFET model and would appreciate any guidance.

The Goal: I am trying to use the STMicroelectronics SCT070HU120G3AG model (from the ST website .lib file) in a DCDC converter simulation.

The Problem: When I use this ST model in my converter, the simulation fails, always giving a Fatal error: Timestep too small....

However, if I use a standard QSPICE library part (like the UF3C120040K3S) as a direct replacement, the exact same converter schematic simulates perfectly.

Troubleshooting Already Performed:

  1. Model Syntax Fix: I have already modified the original .lib file to fix the k keyword conflict, as k is a reserved constant in QSPICE.
    Original: .FUNC bvd(k) {7.8+0.0026*k}
    My Fix: .FUNC bvd(k_var) {7.8+0.0026*k_var} No other changes were made to the .lib file.
  2. Standalone Test: To verify the model, I created a separate, simple characterization test bench (.qsch) to plot the switch’s characteristics. In this simple circuit, the SCT070HU120G3AG model (with my k_var fix) works perfectly.

This suggests the model itself can work in QSPICE, but it is failing when interacting with my more complex DCDC converter circuit (likely during a hard-switching event or when the body diode is active).

My Question:

Since the model works in a simple test jig but fails in the converter, what should I try next?

Are there known issues with these complex, behavioral models from ST that require specific .options settings (like method=gear, reltol, or a strict max timestep) to converge in a switching application?

Attachments: I am attaching the .lib file (with my k_var fix) and the simple .qsch characterization schematic that does work. Unfortunately, due to company privacy, I cannot share the full DCDC converter schematic.

Any advice on how to make this model stable for a switching simulation would be extremely helpful.

Thank you.

2

I am not able to attach the files as it says “Sorry, new users can not upload attachments.”

3

Refer to this post to increase your trust level to basic for schematic upload.
MOSFET transistor simulation - QSPICE - Qorvo Tech Forum

It is quite common for complex MFG models to fail with a timestep too small. Consider creating a MOSFET model for your device. The tool can be found in Qspice under File > Model Generator > MOSFET

4

Hello Mr Kelvin,

Thank you.

I tried to use model generator and referred the video of Mr Engelhardt.
Unfortunately I could not find the body diode characteristics curve in the datasheet of SCT070HU120G3AG model and hence I could not go ahead with the model generator approach.
I am attaching the datasheet for your reference.

Is there any work around for this?

sct070hu120g3ag (1).pdf (956.4 KB)

5

Not sure if this can help.

.model SCT070HU120G3AG VDMOS Rs=7.8m Rd=7.8m Rg=1.5 Vto=4.52
+ Kp=0.69 lambda=0.131 RonX=2.24 eta=75m Vtotc=-2m Is=21.9µ
+ N=5.9889 Rb=77.7m Eg=3.26 XTI=3 Cgs=904p Cgdmin=10.7p 
+ Cgdmax=395p Cjo=1.61n tt=4n Tnom=25 mfg="ST" Vds=1.2K Ids=30
+ Ron=78m Qg=37n

for the body diode curve, you have to flip this graph. I use this same curve for both temperatures as to simply the modeling process.

image
image624×566 88.5 KB

1 Like
6

Thank you Mr Kelvin. I will try with this model.