LTspice Tutorial: Part 6
__Creating LTspice__^{®}__
MOSFET models__
LTspice Tutorial 4
explained that there are 2 different types of SPICE
model: those defined by the simple .MODEL statement
and those defined by the more complex .SUBCKT
statement. The .MODEL statement defines simple
components such as diodes, transistors, MOSFETs etc
with a list of predefined characteristics given to
us by the writers of SPICE programs. The more
esoteric components such as op amps, comparators etc
were defined by a more general .SUBCKT model.
When SPICE (not
LTspice) was first created, the programmers gave the
user a specific number of characteristics to define
certain components. In the case of the MOSFET, this
included the gate source turn on voltage, the
transconductance, the resistance of the gate, source
and drain connections etc. These are known as Level
1 parameters and define the most important
parameters of the MOSFET. In later years, the MOSFET
manufacturers wanted to further characterise their
MOSFETs and not be restricted by the fixed list of
parameters given to them by the writers of SPICE.
They therefore turned to the .SUBCKT definition to
allow them to expand the list of parameters. These
are known as Level 2 and Level 3 parameters and
describe characteristics of the MOSFET not defined
in the original SPICE definition of a MOSFET.
However in making the model more complicated, they
slowed down the simulation time of the MOSFET.
LTspice therefore uses
the simpler .MODEL statement to define the
characteristics of a MOSFET. If using a 3rd party
MOSFET model results in very slow simulation
performance, it is probably because the model is
defined using the .SUBCKT model and includes many
parameters that are not necessary in getting an idea
of the circuit performance.
To create an LTspice
model of a given MOSFET, you need the original
datasheet and the pSPICE model of that MOSFET.
The parameters needed
to define a MOSFET in LTspice are as follows:
Rg
Gate ohmic resistance
Rd
Drain ohmic resistance (this is NOT the RDSon, but
the resistance of the bond wire)
Rs
Source ohmic resistance.
Vto Zero-bias
threshold voltage.
Kp – Transconductance
coefficient
Lambda Change in drain current with Vds
Cgdmax Maximum gate to drain capacitance.
Cgdmin Minimum gate to drain
capacitance.
Cgs Gate to
source capacitance.
Cjo
Parasitic diode capacitance.
Is
Parasitic diode saturation current.
Rb
Body diode resistance.
Rg, Rd and Rs are the
resistances of the bond wires connecting the die to
the package.
Vto is the turn on
voltage of the MOSFET.
Kp is the
transconductance of the MOSFET. This determines the
drain current that flows for a given gate source
voltage.
Lambda is the change
in drain current with drain source voltage and is
used with Kp to determine the RDSon.
Cgdmax and Cgdmin are
the minimum and maximum values of the gate drain
capacitance and are normally graphed in the MOSFET
datasheet as Crss. The capacitance of a capacitor is
inversely proportional to the distance between its
plates. When the MOSFET is turned on, distance
between the gate and the conducting channel of the
drain is equal to the thickness of the insulating
gate oxide layer (which is small) so the gate drain
capacitance is high. When the MOSFET is turned off,
the gate drain region is large, making the
gate drain capacitance low. This can be seen on the
plot of Crss.
Cgs is the gate source
capacitance. Although it changes slightly with gate
source voltage, LTspice assumes it is constant.
Is is the parasitic
body diode saturation current.
Rb is the series
resistance of the body diode.
The
Fairchild FDS6680A MOSFET is defined in LTspice by
the line
.model FDS6680A
VDMOS(Rg=3 Rd=5m Rs=1m Vto=2.2 Kp=63 Cgdmax=2n
Cgdmin=1n Cgs=1.9n Cjo=1n Is=2.3p Rb=6m
mfg=Fairchild Vds=30 Ron=15m Qg=27n)
Note: the
characteristics Vds, Ron and Qg are actually ignored
by LTspice. These are only added to aid the user to
compare MOSFETs.
Therefore an example
template MOSFET model is
.model XXXX VDMOS(Rg=
Rd=5 Rs=1 Vto= Kp= Cgdmax= Cgdmin= Cgs= Cjo= Is= Rb=
)
We are now going to
construct a MOSFET model for the SUM75N06 and
SUM110N04 low ON resistance MOSFETs from Vishay
SUM75N06
datasheet
Original
SUM75N06 Model
SUM110N04
datasheet
Original
SUM110N04 Model
The SUM75N06 has a
moderately low ON resistance and a moderately low
Qg, so is suitable as the top FET in a synchronous
buck converter. The SUM110N04 has a high Qg but
lower ON resistance, so is suitable as the bottom
FET in a synchronous buck converter (see
Buck Converter Design).
**SUM75N06:**
**
Characteristic** |
**
Source** |
**
Value** |
Rb |
another
SPICE model |
1.5 Ohms |
Rd |
SPICE
model |
0 Ohms |
Rs |
SPICE
model |
25m Ohms |
Vto |
Datasheet |
2V |
Kp |
Datasheet |
75 S |
Lambda |
SPICE
default value |
1 |
Cgdmax |
Datasheet
Crss curve |
1200pF |
Cgdmin |
Datasheet
Crss curve |
150pF |
Cgs |
SPICE
model |
2000pF |
Cjo |
SPICE
model |
1200pF |
Is |
SPICE
model |
1pA |
Rb |
SPICE
default value |
0 Ohms |
The final SPICE model
can be downloaded here:
SUM75N06
LTspice model
**SUM110N04:**
**
Characteristic** |
**
Source** |
**
Value** |
Rb |
another
SPICE model |
1.5 Ohms |
Rd |
SPICE
model |
0 Ohms |
Rs |
SPICE
model |
0.86m Ohms |
Vto |
Datasheet |
1.85V |
Kp |
Datasheet |
180 S |
Lambda |
SPICE
default value |
1 |
Cgdmax |
Datasheet
Crss curve |
3000pF |
Cgdmin |
Datasheet
Crss curve |
900pF |
Cgs |
SPICE
model |
14.5nF |
Cjo |
SPICE
model |
4.9nF |
Is |
SPICE
model |
33.4pA |
Rb |
SPICE
default value |
0 Ohms |
The final SPICE model
can be downloaded here:
SUM110N04
LTspice model
The SPICE models can
then be testing using these test jigs:
RDSon test jig
To test the RDSON of
the MOSFET import the model into the LTspice test
circuit. Check the datasheet to see how the RDSOn
has been tested. It will be characterised with a
certain gate-source voltage and a certain drain
current.
Run the simulation.
Probe the drain voltage. Probe the drain current.
Edit the Drain current icon to read **V(drain)/Id(M1)**.
This changes one of the axes to read ON resistance.
You may have to change the parameter Kp slightly to
match the datasheet performance.
Switching Time Test Jig
To test the switching
time of the MOSFET import the model into the LTspice
test circuit. Check the datasheet to see how the
switching times have been tested. They will be
characterised with a certain gate drive voltage,
gate drive resistance and drain voltage and the
response time will be characterised when the drain
current ramps to a certain level.
Run the simulation.
Probe the gate voltage. Probe the drain current.
Zoom in on the rising edge of the gate/drain
waveforms. Left click on the Drain current axis and
rescale the axis to measure slightly over the
current desired drain current. The timings can now
be measured. Rise time is normally measured over
10% to 90% of the desired voltage swing. You may have to change the
model capacitances slightly to meet datasheet performance.
LTspice is a registered trademark of Linear
Technology Corporation |