Tag : Ltspice IRF 520 N Mosfet simulation of switching, problem very low drain current

Thread Starter

Fredrik3159

Joined May 2, 2020
2
Lecture of datasheet of part IRF520 :
absolute maximum ratings :
Drain Source voltage : 100 V
Gate-Source voltage : 20 V
Id (T=25°C) (under Vgs=10 V) 5 A
R DS resistance 0.23 ohm

Problem : I have set my simulation scenarios to transient with 50 periods of pulses of control voltage of the circuit above-left-bottom (V1). The relative low pulse frequency should have no effect on switching losses. In fact, when the simulation results are displayed, the gate command is also a pulse between 1.5V and 12V and Vd=12V, Ids should eventually rise to approx 11V/100 ohm=0.1A but it definitely not goes beyond 1.4 mA. Why ?
 

Attachments

ronsimpson

Joined Oct 7, 2019
2,261
Please post your file. I don't want to redraw it.
You are not turning on the MOSFET well. The Gate needs to be 10 volts above the Source. The Source voltage is 0V to 12V.
 

Thread Starter

Fredrik3159

Joined May 2, 2020
2
I had attached a wrong image file:. I post now the correct circuit as image and asc file.
For the generic Mosfet I will update it by the 520. I had considered there were few differences between this and the 520.2022-07-31 (6).png2022-07-31 (6).png
 

Attachments

ronsimpson

Joined Oct 7, 2019
2,261
There are a number of things wrong.

I tried to assign a real part number to M1 but it did not work right. I deleted M1 which was not working. Add a MOSFET and gave at a part number. (60 volts part any part just pick one) Now the MOSFET works. When I deleted M1 there was a strange connection under the part. Not needed. It might have shorted out something.

MOSFETs are turned on by a voltage from Gate to Source. Not from Gate to Ground. Your gate goes up to 12V and it takes about 7V G-S to turn on the part, so the Source only goes up to 5 volts. (see post #3)

Q2 & Q5 are going to try to short out the 12V supply.
 
Last edited:

eetech00

Joined Jun 8, 2013
3,330
Lecture of datasheet of part IRF520 :
absolute maximum ratings :
Drain Source voltage : 100 V
Gate-Source voltage : 20 V
Id (T=25°C) (under Vgs=10 V) 5 A
R DS resistance 0.23 ohm

Problem : I have set my simulation scenarios to transient with 50 periods of pulses of control voltage of the circuit above-left-bottom (V1). The relative low pulse frequency should have no effect on switching losses. In fact, when the simulation results are displayed, the gate command is also a pulse between 1.5V and 12V and Vd=12V, Ids should eventually rise to approx 11V/100 ohm=0.1A but it definitely not goes beyond 1.4 mA. Why ?
If you want good results, then use good models instead of ideal devices.

I didn't test everything, just corrected the mosfet issue.

An incorrect mosfet symbol was used (nmos4). I replaced it with "nmos".
To use a .subckt model file with the nmos symbol, change the nmos symbols' "prefix" attribute to X then specify the model name in the "value" attribute. Use the ".inc" directive on the schematic to specify the location of the subckt file.

The model file is atttached.

1659324831122.png
 

Attachments

Papabravo

Joined Feb 24, 2006
19,023
Not necessarily true.
You should use real models for all the active devices (diodes, BJTs, MOSFETs), as the generic models sometimes give odd results.
I 2nd that notion. Generic models for a BJT and a diode with a tweak or two might be used for some purposes. If the purpose of simulation is understanding, then you should use real device models exclusively unless you have the knowledge to do something different. Like Feynman with respect to understanding quantum mechanics, there are only a very few people in the world who know how to tweak SPICE device models with any degree of skill. FYI - I don't yet understand SPICE models well enough to do that.
 

Alec_t

Joined Sep 17, 2013
13,077
I think M1 would be better used as a low-side switch, and the current-sense feedback via Q5 could go through a resistor to the bases of Q2/3 instead of to the M1 gate.
 
Top