|
|
 |
For Power MOSFET SPICE Models -- version 1.5, October 1996
A. Introduction
A switched capacitor electrical model and an empirical thermal model
have been developed to simulate the Power MOSFET electrical performance
[1] and thermal behavior [2] respectively for almost all devices we support.
Different electrical and thermal models of the devices are contained in
the library, FSDMOS.LIB. (See section on Suggestions and Comments)
To demonstrate the use of the MOSFET libraries, an example of how to
incorporate these two models into the test cirucits have been given. The
device being used in the example is NDS706A.
Subcircuit model NDP706A can be used to perform DC and transient simulations.
When combined with subcircuit 706THMAL, thermal analysis can also be performed.
For TO-220 and TO-263 devices, the thermal models simulate the single
pulsed junction-to-case thermal performance. Besides defining the ambient
temperature, users must account for the case-to-ambient thermal resistance
Rca on their system such as the heatsink and board influence etc. For
reference, the example in section C (ex1_thm.cir) shows a simplified method
for simulating the case-to-ambient thermal response using an RC Thermal
Network. The simulated device in the example is mounted on an ideal heatsink
in which the case-to-ambient thermal resistance is 0°C/W.
For all surface mount devices except TO-263, the thermal models approximate
the single pulsed junction-to-ambient thermal performance and require
users to define the ambient temperature.
For repetitive pulses rather than single pulse application, users should
modify the subcircuit "E_rjc table" by inputting the proper duty
cycle normalized transient thermal resistance curve, which can be obtained
from the data sheet.
For power pulses much longer than the thermal time constant tq, the
model will underestimate the junction temperature because in most practical
applications, the case temperature will not be fixed [2]. See Section
E. Suggestions and Comments below.
B. Files for users' circuit simulations:
- FSDMOS.LIB
- ex1_thm.cir
- ex2_id.cir
- ex3_idvg.cir
- ex4_rds.cir
- ex5_sw1.cir
- ex6_sw2.cir
- ex7_gc.cir
The library files are important for the users' circuit simulations.
The electrical model can be used directly with any SPICE2G6 compatible
version without any changes. ex1_thm.cir is a thermal analysis verification
circuit. All exXXXXXX.cir files are circuits used to verify the electrical
performance of the device.
C. How to incorporate the power MOSFET SPICE models
The power MOSFET you use in your circuit can be represented by the following
commands in the circuit node list.
|
X1
|
3
|
2 |
0 |
NDP706A |
| |
.LIB |
FSDMOS.LIB |
|
These commands call the electrical model for NDP706A from the FSDMOS
library and place it into the circuit. Nodes 3, 2, and 0 are the Drain,
Gate, and Source terminals respectively. Make sure FSDMOS.LIB is in the
search path.
Note: In the current version, the library has been extended to include
the characteristics of the device at different temperatures. In other
words, the variation of threshold voltage, drain-to-source on resistance,
and breakdown voltage with temperature can also be simulated with SPICE
to give a more complete SPICE device model.
Thermal analysis example
The following example illustrates the use of both the electrical and thermal
models. In this example, a thermal analysis on a single pulse event is
simulated. Note the accuracy may vary if tolerance is relaxed to comprise
the convergence problem. In any case, use a smallest possible ".OPTION
RELTOL=".
|
| |
|
Rd |
5
|
4
|
0.15
|
|
| |
| |
|
Vgs |
1
|
0
|
PULSE
|
|
| |
| |
|
+ (0, 10V 100ns 10ns 10ns 10s 100s) |
| |
| |
|
Rg |
1
|
2
|
50
|
|
The following calls the electrical and thermal models: |
| |
|
X1 |
3
|
2
|
0
|
NDP706A
|
| |
| |
|
E_Pin |
50
|
40
|
value = {V(3,0)*I(V_Id)}
|
| |
| |
|
X2 |
50
|
40
|
100
|
706THMAL
|
|
The following illustrates the use of an RC Network to simulate the case-to-ambient
thermal response:
|
|
|
G_Pin |
6 |
10 |
40 |
50 |
1 |
| |
|
|
R_thermal |
6 |
10 |
0.001 |
|
|
| |
| |
+ ; 0.001 defaults ideal heatsink |
| |
|
|
C_thermal |
6 |
10 |
1000 |
|
|
| |
| |
+ ; 1000 defaults ideal heatsink |
| |
|
|
V_ambient |
10
|
0
|
25
|
|
| |
+ ; Ambient temperature = 25 deg |
| .LIB |
FSDMOS.LIB |
|
|
|
| |
.PROBE |
|
V (X2.90,40) |
; Transient Rjc |
|
|
|
+
|
|
V(100) |
; Tj |
|
|
|
+
|
|
V(100,40) |
; Tjc |
|
|
|
+
|
|
V(6) |
; Tc |
|
|
|
+
|
|
V(6,10) |
; Tca |
|
|
|
+
|
|
V(10) |
; Ta |
|
|
|
+
|
|
V(50,40) |
; Power input |
|
|
|
+
|
|
V(2,0) V(3,0) I(V_Id); Vgs, Vds, Id |
| |
| .OPTION ITL5=0 |
| |
| |
.OPTION RELTOL=0.05 |
| |
.TRAN/OP |
10.0us
|
50.0s
|
0
|
0
|
uic
|
| |
| |
.END |
Node designation
| 3 |
Drain terminal |
| 2 |
Gate terminal |
| 0 |
Source terminal, ground, and 0°C thermal reference |
| 40 |
Case temperature and input power reference node of the thermal model
subcircuit |
| 50 |
Power dissipation input node to the thermal model subcircuit |
| 100 |
Junction temperature node of the thermal model subcircuit |
| 6 |
Case temperature node |
| 10 |
Ambient temperature node |
Nomenclature and command explanation
| X1 |
calls the Power MOSFET electrical model NDP706A |
| E_Pin |
calculates the device power dissipation and applies it to the thermal
model subcircuit. Use the DMOS Drain-Source voltage and the Drain
current to calculate power={V(3,0)*I(V_Id)} in this example. Note:
power is represented by voltage in this model. |
| X2 |
calls the thermal model 706THMAL to calculate power, average power,
and junction-to-case temperature. |
| E_Casetemp |
sets the case temperature of the Power MOSFET equal to the sum of
the voltage across the case-to-ambient RC Network and ambient temperature
voltage reference. |
| G_Pin |
redefines the device power dissipation as a current and applies
it to the case-to-ambient RC Thermal Network. |
| R_thermal |
case-to-ambient equivalent thermal resistance 0.001 °C/W represents
a perfect heatsink in the example. |
| C_thermal |
case-to-ambient equivalent thermal capacitance. 1000J/°C represents
a large thermal capacity in this example. |
| V_ambient |
ambient temperature in °C. Ambient is 25°C in this example. |
| .PROBE V(X2.90,40) |
Normalized Transient Thermal Resistance resides at thermal model
subcircuit. Can be used to plot maximum power dissipation and current
handling capability with proper mathematical manipulation |
| V(100) |
shows junction temperature Tj in °C |
| V(100,40) |
shows junction-to-case temperature in °C |
| V(6) |
shows case temperature Tc in °C |
| V(6,10) |
shows case-to-ambient temperature in °C |
| V(10) |
shows ambient temperature Ta in °C |
| V(50,40) |
shows Power input in W |
| V(2,0) V(3,0) I(V_Id) |
show Vgs, Vds, Id |
|
Note: The model is valid for single pulse. However, due to the fact
that the power has been averaged over time for computation, the thermal
response of repetitive pulse may not be very accurate.
D. Verification Programs
In developing the SPICE models efforts have been made to ensure accuracy.
The test circuits listed below are used to verify the accuracy of the
simulations in comparison to the data sheet characterization charts.
ex1_thm.cir - This program can be used to verify the thermal
performance. Users can also change the parameters of the Thermal RC Network
to test their circuit.
ex2_id.cir - This program can be used to verify Id vs Vds and
Vgs.
ex3_idvg.cir - This program can be used to verify Id vs Vgs.
ex4_rds.cir - This program can be used to verify Rds(on) vs
Id.
ex5_sw1.cir - This program can be used to verify the switching
behavior under resistive load.
ex6_sw2.cir - This program can be used to verify the switching
behavior under unclamped inductive load.
ex7_gc.cir - This program can be used to verify all interelectrode
capacitances indirectly through the gate charge characteristics.
E. Suggestions and Comments
- DC sweeping and thermal analysis cannot be performed simultaneously
due to SPICE limitations.
- If convergence errors occur during transient or thermal analysis,
increase the .OPTION RETOL = 0.001 to 0.01 or larger. Also, reducing
the pulse width, transient analysis range, or the finite iteration step
may help resolve the problem.
- The longer the simulation time with respect to the pulse duration
is, the POORER the thermal result will be. This is attributed to the
fact that the thermal model uses the average power in the calculation
while at the same time it averages the simulation time as the total
pulse duration. As a result, the temperature increase due to any subsequent
pulse after the first one will diminish contrary to our expectations.
Nevertheless, the FIRST PULSE JUNCTION TEMPERATURE IS STILL VALID.
F. Reference Material
[1] C. E. Cordonnier, P. Rossel, R. Maimouni, H. Tranduc, D. Allain,
M. Napieralskadouard. "Spice Model for TMOS Power MOSFETs", Application
Note Motorola AN1043/D, 1989.
[2] S. Menhart, "Using SPICE to Calculate MOSFET Operating Temperature",
0-7803-0695-3/92 1992 IEEE, pp. 901-906.
[3] MOSPOWER Applications Handbook, 1984 ed., Siliconix Incorporated.
This application note is intended for those who are familiar with simulation
programs such as SPICE, SPICE2G6, P-SPICE, H-SPICE or other similar simulation
programs. The information contained has been verified to ensure accuracy.
In any event, Fairchild Semiconductor does not assume any responsibility
for the use of any circuitry described, no circuit patent licenses are
implied, and Fairchild reserves the right, at any time without notice,
to change set circuitry or specifications.
|
|
|
|
|
|
Return to Home
