From: Muranyi, Arpad (email@example.com)
Date: Mon Sep 18 2000 - 10:35:46 PDT
I would like to comment on the three bullets you listed which put accuracy
and speed into an inverse relationship regarding transistor level and
behavioral models. Simply said this general relationship is NOT TRUE.
You CAN model devices to even a higher level of accuracy behaviorally
than on a transistor (SPICE) level if you like. It all depends on what
parameters you use and what goes into the behavioral model. And this
increased accuracy does not mean that your model will automatically get
Take a transistor, for example. You can describe it with its geometry,
and properties of the materials that it is made from. A SPICE tool then
converts all that information to electrical characteristics. This takes
a lot of equations and calculations. On the other hand, you can describe
the same transistor's characteristics by providing its node voltage and
current relationships directly (with tables, equations, transfer functions,
etc...) which CAN reduce the number of calculations SPICE has to do, making
Now think about the underlying model equations SPICE uses when you do it
the conventional SPICE way. You can have a LEVEL=3 or BSIM4 set of
equations. Which one is more accurate? Most likely the BSIM4, since
it is more recent. However, if your behavioral transistor model DOES
describe something that even BSIM4 cannot, you behavioral model will be
even more accurate. Yet this does not mean that it has to become
What I wanted to illustrate here is that the accuracy of the model depends
on what goes into it. It's speed, however, depends on how the device is
described. These two are not as strongly related as your three points
From: abe riazi [mailto:firstname.lastname@example.org]
Sent: Friday, September 15, 2000 7:17 PM
Subject: [SI-LIST] : Macromodel Creation
While visiting a Barnes & Noble bookstore in San Jose, I purchased a copy of
the "Spice Practical Device Modeling" , by Ron Kielkowski.
What especially appealed to me about this publication was its high emphasis
on model creation. In this book SPICE models are classified according to a
hierarchy which includes:
1. Transistor-level models ( provide highest accuracy, though most time
consuming to simulate).
3. Behavioral Macromodels (fastest to simulate, but least accurate)
Most attention is devoted to Macromodels, because they offer a practical
level of accuracy (less than 5% rms error over operating range) and can be
created in a reasonable amount of time (less than eight hours).
The procedure recommended by Ron Kielkowski for construction of macromodels
consists of the following steps:
i. Review the datasheet to obtain as much information related to model
creation as possible (although, frequently majority of the information given
in the datasheet has little value towards model generation).
ii. Utilize bench-top measurement equipment to produce I-V, C-V and Z-F
iii. From above data extract the desired model parameters.
For a resistor, the Macromodel elements consist of a nominal resistance
Rnom and a parallel capacitance Cp; for an inductor, Lnom (nominal
inductance), Rs (coil resistance) and Cp (winding capacitance); and for a
capacitor, Cnom (an ideal capacitor), RL (leakage resistor), Ls (series
inductor) and ESR (electrical series resistance). These macromodels are
illustrated by Figure 1 (attached gif picture).
In this publication (reference 1), the significance of impedance vs.
frequency plots is emphasized, because:
a. Regarding macromodel of a resistor, the |Z| vs. F graphs aid to
b. For inductor Macromodels, they allow determination of the series
resistance frequency (Frs) and self resonating frequency (Fsrf) from which
values of Lnom and Cp can be calculated via simple formulas.
c. Considering capacitor macromodel, several parameters can be extracted
from the impedance vs. frequency curves, such as ESR (RS) , lead inductance
Ls (calculating Ls involves Fsrf which can be obtained from graph) and Cnom
(the nominal capacitance can be also measured by means of a low frequency
ESR and |Z| vs. F plots have been explained previously in this forum in
relation to PCB power distribution systems, decoupling and bypass
capacitors. They are also included here due to their significance towards
Figure 2 presents two examples of impedance vs. frequency graphs. Such plots
can be created in a number of different ways; here, Microsoft Excel was
employed. In each case the raw data consisted of three columns: current ( I
) , Voltage drop ( V ) and frequency ( F ). The Excel program calculated
another data column (impedance Z = V/I ), and produced the logarithmic
impedance plots. Clearly, ESR strongly influences the shape of |Z| vs. F
Macromodels can be incorporated into SPICE simulation files as subcircuits;
demonstrated by the example below:
Example 1. Encapsulation of a capacitor macormodel CMACRO, having
parameters Cnom, RL, Ls and Rs (ESR).
In the circuit input file example.cir:
X_MACRO 2 0 CMACRO
In the model file example.mod:
.SUBCKT CMACRO 10 20
Cnom 10 30 1000uF
Rs 30 40 0.15ohms
Ls 40 20 5nH
RL 10 30 10meg
Use of macromodels instead of SPICE primitive models can significantly
enhance the accuracy of a high frequency simulation and yield results in
excellent agreement with physical measurements.
Simulation of certain cases (such as high power circuits) require taking
into consideration effects due to temperature variations. Temperature
dependent macromodels can be readily constructed (reference 1).
To summarize, Macromodels assume an intermediate position in the hierarchy
of SPICE models in the sense that they are below the transistor-level models
in accuracy and rank second to behavioral models in simulation speed. They
are in demand by being practical; i.e., can be created in a reasonable
amount of time with an error margin tolerable in many applications.
Impedance vs. frequency plots play a critical role in creation of
macromodels of passive components. These models can be inserted into SPICE
input files as subcircuits. Simulations utilizing macromodels yield superior
results than using ideal SPICE primitives, particularly in the high
Reference 1. R. M. Kielkowski, "SPICE Practical Device Modeling",
McGraw-Hill, Inc. 1995.
Thanks for your comments and with best regards,
2251 Lawson Lane
Santa Clara, CA 95054
**** To unsubscribe from si-list or si-list-digest: send e-mail to
email@example.com. In the BODY of message put: UNSUBSCRIBE
si-list or UNSUBSCRIBE si-list-digest, for more help, put HELP.
si-list archives are accessible at http://www.qsl.net/wb6tpu
This archive was generated by hypermail 2b29 : Tue May 08 2001 - 14:29:30 PDT