USER MANUAL (Copy of the chapter of the Application Note - AN1043


This chapter is for those who are already accustomed to SPICE programming
and would like to know the contents of the floppy disk and how to use it.
For those who want to know more about the model, please read the
Application note.

It is format compatible with IBM PC and Macintosh micro computers.
The 3 1/2" disk is for 800Kb Macintosh disk driver (double side)
The 5 1/4" disk is for 360Kb IBM PC compatible disk driver
The 3 1/2" disk is for 720 Kb IBM PC compatible disk driver

 This study has been developed with PSPICE of MicroSim Corp., but since all
the data contained in this disk are ASCII files, they can be read by any word
processor and modified for the context of the user. As you'll notice, the
.PROBE command helps you see the waveforms on the screen. If you do not
have this feature, you can use .PRINT or .PLOT for another output format.
The floppy disk contains different files. The first three are dedicated to the
Motorola power MOSFET library itself. They can be used directly with any
SPICE2G6 compatible version without any change. The other programs may
require some changes if you do not use PSPICE.  But in any case, you can list
them with any editor program and change the syntax to have it compatible
with your own SPICE version: you may have to replace .PROBE by .PLOT and
possibly the syntax of some  calls (e.g. I(X1.RS)).

I-A. The TMOS Library
===================

I-A1. What is On the Disk
++++++++++++++++++++++

TMOS.LIB
This file is the most useful one, using a model with switched capacitors
and requiring no initialization (figure 2). Starting with this disk is advised,
even if it might be a little slow. The schematic for the P-channel model is
given in the Appendix.

TMOSINIT.LIB
This is, from the static point of view, exactly the same as the previous
file, but it is much faster since it does not use the capacitor switches
(figure 3). The drawback is that it requires an initialization step for the
node (6) between CGDMAX and DGD (only for the transient analysis).
The voltage of this node depends on the VDS and VGS voltages at the start
of the simulation. Therefore a utility file called INIT.CIR is provided with
this TMOSINIT library.

INIT.CIR
This SPICE compatible file helps you to compute the initial condition V(8)
to set on node 6 for the given starting VDS. (figure 4)

I-A2. How to Call a Device In the Library
++++++++++++++++++++++++++++++++++++

a. For the TMOS.LIB library you'll need to write in your source program:

.LIB TMOS.LIB    to call the library with switched capacities

X1 MTP25N06 2 1 3    to call the product to be used
       !               !  !  !
       !               !  !  Source
       !               !  Gate
       !               Drain
      Device Part Number available in the library

b. If you use TMOSINIT.LIB you'll need:

.LIB TMOSINIT.LIB  to call the faster but more complex library

X1 MTP25N06 2 1 3 8 to call the product to be used
           !           !  !  !  !
           !           !  !  !  Initialization pin (node 6 between CGDMAX and DG
D)
           !           !  !  Source
           !           !  Gate
           !           Drain
          Device Part Number available in the library

.IC V(8)=2.5   The voltage value of the extrinsic node 8 will be given by the
INIT.CIR program according to the VDS voltage at the initialization phase. If
you do not enter the proper value, it may give you incorrect switching
times.

1-A3. Additional Information on the Library
+++++++++++++++++++++++++++++++++++++++

Both TMOS.LIB and TMOSINIT.LIB have been created so you do not need
to modify them. They work for both DC and transient analysis. The latter
one needs just to be initialized.
One of your concerns at this point of the reading, may be to know what
is given: either the typical values or the maximum ratings. The answer is
clear-these are typical values of today's products measured at 25-C.
The library has been done from the measurements on one or two
products of every part number, and they can be considered  typical of the
product line. These have been checked and stand within the data sheet
limits. The simulation is accurate in the range of 80 to 90 % .
The comparison with the data sheet curves can be done too, but with
some care. Since the user may not have the updated document and the
products may have been improved in the meantime, some differences can be
found between the SPICE simulation and the data sheet curves.
 In the chapter called Parameters Extraction Method (Section IV), we
will see how the library was built and also, how to modify it if the user
wants the maximum values rather than the typical ones.

I-B. Validation Programs or TESTBOX
=================================

This file contains some tools to evaluate the library. You are welcome
to use them and modify them to your own needs. They are component-
manufacturer-oriented, which means they tend more to simulate the data
sheet curves rather than the application, but you'll find some typical
applications circuits too. Please refer to Appendix pages for the description
of the schematic of the following files.

I-B1.  ONCHARAC.CIR
++++++++++++++++++
One of the first curves you find in the data sheets is  On-Region
characteristics. It gives the Drain Current (ID) versus the Drain Source
Voltage (VDS) for different Gate-Source Voltages (VGS). Only a DC analysis
is required for such a test and it requires a very small amount of program
lines. (see Appendix). For other devices, you just need to change the device
part number using the Find/Replace option of your editing program.

For example:
Find: MTP25N06
Replace by: MTP3055E         REPLACE ALL

I-B2.  ID-VGS.CIR
+++++++++++++++
It gives you the transfer characteristic curve: Drain Current (ID)
versus Gate-Source Voltage (VGS) for a given Drain-Source Voltage (VDS
generally equal to 10 volts). This is one more DC test.

I-B3.  RDSON.CIR
++++++++++++++
It gives the ON state resistance for different drain current values.
The ratio VD/ID must be put on the y-axis to get the data sheet curve.

I-B4.  CAPACITY.CIR
++++++++++++++++++
This is the first program out of several using the transient analysis
option of SPICE to check the dynamic response of the TMOS model.
CAPACITY.CIR gives you the capacitance variation curve of the Power
MOSFET. This curve is diffucult to  measure and  requires a rather
sophisticated bench setup (like BOONTON or HP) . Therefore you'll have to
rely on the data sheet curves, even if, in some cases, they are rather rough.

The principle of this test in SPICE is based on the capacitor equation:

i(t) = C(f) dv/dt
If a voltage increase, with a constant dv/dt, is applied on a linear or non-
linear capacitance, the current flowing in it will be proportional to the
capacitance value. It is usually set at 1v/-sec. which gives 1 milliampere
for 1 nano Farad.

Generally the Drain-Gate Voltage (V(2,1)) is put on the x-axis and the
different branch currents on y-axis.

For example:
-in TMOSINIT.LIB, I(X1.CGDMAX) or I(X1.DGD) represents Crss
   (do not forget to give the right initial voltage value)
-in TMOS.LIB, Crss is represented by I(X1.CGDMAX)+I(X1.DGD)
-and in both libraries:
  I(X1.DDS) is the Drain-Source Capacitance
  I(X1.CGS) is the Gate-Source Capacitance
  I(X1.RG) is the Ciss curve

I-B5.  GATECHRG.CIR
++++++++++++++++++
This gives you the Gate Charge versus Gate-to-Source voltage curve. This is
another way to visualize your power MOSFET capacitances: you charge the
gate of the transistor with a constant current of 1 mA. For the load, a
constant current source is used on the drain.

For a capacitance, the charge equations are:
Q = CV and Q = it
If i = Cte = 1 mA, 1 microsecond on the x-axis will be equivalent to 1 nano
Coulomb. Taking into account this unit change, the equivalent data sheet
curve can be obtained.

I-B6.  SWITCHING.CIR
+++++++++++++++++++
This is to check different switching characteristics, either inductive or
resistive, clamped or not clamped (see Appendix).

IMPORTANT: the users must be warned that the equivalent circuit of the
inductive load has to be studied precisely before making any comparison
between simulation and reality. Since power MOSFETs are very fast devices,
sometimes the switching limitation can come from the inductance rather
than from the transistor itself. Poor quality inductances may have rather
low resonance frequency which appears to be more capacitive than
inductive at high frequency and high switching speed. Therefore, if poor
correlation results  please do not blame the TMOS library first, but check
whether your equivalent inductance circuit is good by doing its Bode
diagram.

I-B7.  DGCLAMP.CIR
+++++++++++++++++
This is a typical application for inductive switching. Instead of using an
external power zener to do the clamp, a small signal zener is put between
drain and gate. The TMOS power FET now dissipates the stored energy during
the turn off rather than the power zener. In this application it is very
interesting to see the instantaneous power dissipated into the TMOS device
(ID . VDS). The peak power occurs during turn off. We notice that "ON"
dissipation is negligible.


WARNINGS FOR IBMPC USERS
1. Some spice interpreters might not accept more than 8 characters
as subcircuit names, especially on IBM PC. User will have to rename the
device names to be consistent with this interpreter.

2. Due to memory limitations, probe may not work on IBMPC with the
files included in this disks. The user will have to modify .TRAN & .DC
cards to limit the number of points to be plotted by probe.

PSPICE is a trademark of MICROSIM Corp.
