How to Test N-MOSFET Spice Model Quickly?

Overview

This note is on how one can perform quick simulation test in Proteus (in fact any electronics simulator) to verify the custom simulation model, pin mapping, and switching behavior of the IPA045N10N3G N-Channel MOSFET.

I am designing a MPPT (Maximum Power Point Tracking) Controller using STM32F103 in Proteus, for both simulation and PCB production. I needed IPA045N10N3G N-Channel MOSFET part but after installing its spice model I needed to check the correctness of the MOSFET pins. So I did the following to test the N-MOSFET.

N-MOSFET Test Circuit Configuration

To confirm that the Gate (G), Drain (D), and Source (S) pins are properly mapped and not swapped, the following test circuit was constructed:

N-MOSFET Test Circuit

  • Component Under Test: Q2 (IPA045N10N3G)

  • Gate (G): Connected to a DC Voltage Generator set to $10\text{ V}$ (exceeding the gate-source threshold voltage $V_{GS(th)}$ to fully turn on the MOSFET).

  • Drain (D): Connected in series with a $10\ \Omega$ load resistor (R4) to a DC Voltage Generator set to $12\text{ V}$.

  • Source (S): Connected directly to Ground ($0\text{ V}$).

IPA045N10N3G Spice Model


* ============================================================================
* IPA045N10N3G - SPICE3f5 macro-model of Infineon OptiMOS 3 IPA045N10N3 G
* (100 V, 4.5 mOhm max, TO-220 FullPAK)       Pin order: D G S
* Elements used: MOSFET level 1, R, C, D only (no .PARAM, no B sources).
*
* Fitted to datasheet Rev 2.4 (typical values, 25 C):
*   Rds(on) 3.9 mOhm @ Vgs=10 V, Id=64 A       Vgs(th) 2.7 V @ 150 uA
*   Rg 1.4 ohm   Ciss 6320 pF   Coss 1210 pF   Crss ~41 pF (@ Vds=50 V)
*   body diode Vsd ~0.9 V, Vbr 100 V
* Note: level-1 has no sub-threshold current, so VTO=2.7 V is the on-set point.
* Simplifications: capacitances are constant (real Cgd/Cds rise at low Vds),
*   no temperature dependence, no package inductance, no avalanche model.
*   Cgd is a compromise value so switching time / Miller plateau are realistic.
* created by ee-diary.net
* ============================================================================
.SUBCKT IPA045N10N3G D G S
RG   G  G1  1.4
M1   D1 G1  S1 S1 MIPA W=1 L=1
.MODEL MIPA NMOS (LEVEL=1 VTO=2.7 KP=39 LAMBDA=0 CGSO=0 CGDO=0 CGBO=0)
RD   D  D1  0.25E-3
RS   S  S1  0.15E-3
CGS  G1 S1  6.0E-9
CGD  G1 D1  250E-12
CDS  D1 S1  0.9E-9
DBODY S1 D1 DBD
.MODEL DBD D (IS=1E-11 N=1.05 RS=0.6E-3 BV=100 IBV=1E-3 CJO=0 TT=60E-9)
.ENDS IPA045N10N3G

Simulation & Expected Results

  1. MOSFET Activation: When the simulation runs, applying $10\text{ V}$ to the Gate creates a conductive channel between the Drain and Source.

  2. Voltage Drop: Because the MOSFET switches ON with a very low drain-source on-resistance ($R_{DS(on)}$), it creates a low-resistance path to ground.

  3. Verification:

    • Pass: The voltage measured at the Drain node drops near $0\text{ V}$ (while almost the entire $12\text{ V}$ drops across the $10\ \Omega$ resistor, drawing roughly $1.2\text{ A}$). This confirms the pin ordering (G, D, S) is accurate.

    • Fail: If the Drain voltage remains near $12\text{ V}$ or the current readings are abnormal, the pin mapping in the SPICE/Proteus model configuration needs to be corrected.

How to Test N-MOSFET Spice Simulation Model Quickly

Video Tutorial



Related:


Post a Comment

Previous Post Next Post