From: Muranyi, Arpad ([email protected])
Date: Mon Sep 18 2000 - 13:15:28 PDT
Abe,
Thanks for your explanation and the quotes from Ron Kielkowski.
However, I have to argue with him then. Not knowing what else
he says in his book (I am not sure whether he spells out some of
his assumptions or not), reading these words as they are I
must say that he is incorrect all the way through. (He may
be correct given some assumptions, but not in general).
1) SPICE transistor level models do NOT "represent devices at
the most basic simulation level possible". I could think of
a future(?) simulator which simulates a transistor by the
electron behavior in the crystal structure of the material(s)
that it is made from. "Most basic" will always be as low level
as our knowledge is about particles, which is currently even
lower than electrons and crystal structures. Is there any mention
in SPICE models how electrons bump into each other in the material?
No. For that reason I don't agree that SPICE represent devices at
the most basic level.
2) Simplification is not necessarily related to accuracy. Think
about a math example: a^2+2ab+b^2 = (a+b)^2 It is probably much
simpler and faster to calculate the result of the right side than
the left side of the above equation. Is one of them less accurate
than the other? Similarly, simplifying a transistor model from its
geometric description (SPICE) to an electrical description (behavioral)
does not have to mean that the latter one is less accurate. It all
depends on how the simplification is made and whether something was
omitted during the simplification process. If things are omitted,
I would rather call the "simplification" compromising. Now, hold
on tightly: Even SPICE transistor level models contain omissions!
Just think how many of the higher order effects are missing in the
earlier MOSFET models (level=3) vs. newer models BSIM4, for example.
So I would be very careful to say that SPICE transistor models are
the king. It all depends on how much effort the model maker puts
into them too, just as it is with behavioral models.
3) The Op-amp example is a perfect one. We know very well how to
characterize them for gain, input and output impedance, frequency
and phase response, distortion, noise, etc... An Op-amp circuit
can be modeled behaviorally very well with a few fairly simple
expressions. Even though I haven't done it (because I work with
digital circuits), I am fairly confident that these expressions can
be formulated so that the response of these expressions will be
right on top of the original transistor level model's response.
Will this behavioral model be faster? Most likely yes. Will it
be less accurate? Not necessarily.
And I agree, there are always exceptions. I could tell you an example
where a behavioral model was slower than the original transistor model
if they wouldn't have to kill me if I did so. And on top of that,
chances are that it still was not as accurate as the original
transistor level model. However, I found out from the guy who
implemented the simulator engine that the reason for that was in
the architecture of the simulator and/or model. Simulators are
optimized for certain things to speed them up. These optimizations
may work in some cases but not in others. I am just guessing, but
I feel that accuracy may also be optimized for certain situations
in simulators. So there are a lot of ifs and buts, but the bottom
line in my opinion is that the relationship that behavioral models
are faster but less accurate then their transistor level equivalents
is not true in general. It all depends on the model maker.
(And remember, IBIS files are not IBIS models, they just contain the
data for the model which resides in the simulation tool. But I don't
want to start IBIS vs. SPICE here, so that's the last I will say on
that).
Sincerely,
Arpad Muranyi
Intel Corporation
================================================================
-----Original Message-----
From: abe riazi [mailto:[email protected]]
Sent: Monday, September 18, 2000 12:10 PM
To: '[email protected]'
Cc: '[email protected]'
Subject: RE: [SI-LIST] : Macromodel Creation
Arpad:
Thanks for your response.
When I wrote that SPICE transistor level models are most accurate but also
most time consuming to simulate, I did not mean that it is "always" true and
there can be exceptions. but it will hold true in many cases. Ron
Kielkowski (Reference 1, PP. 5 - 7) presents good definitions and examples
in support of this point:
1. TRANSISTOR LEVEL MODEL: "represents devices at the most basic simulation
level possible. In many cases, the transistor-level model is the most
accurate model possible for simulation. On the downside though, the
transistor-level model also takes the most time to simulate."
2. MACROMODEL: " A macromodel is a collection of electrical components which
form a simplified representation of the modeled circuit. Many macromodels
contain dependent controlled sources to help simplify the structure of the
model. Being simplified means that the macromodel is often easier to
construct than transistor level model, and the macromodel often simulates
much faster than the transistor level model. But these two elements come at
the expense of a small loss in accuracy."
3. BEHAVIORAL MACROMODEL: "The highest level in modeling hierarchy is the
behavioral macromodel. Behavioral macromodels contain a collection of ideal
electrical or mathematical components. Often behavioral macromodels contain
a collection of ideal electrical or mathematical components which are used
to describe a function of the circuit. Being at the top of the hierarchy
means the behavioral model usually simulates faster than any other type of
model, but often this increased speed comes from a loss in accuracy".
As an example, the transistor level model of an Op Amp can have about 19
transistors (plus some passive components), the macromodel of the Op Amp
consists of only two transistors and four diodes (plus some passive
components and dependent controlled sources). The Op Amp behavioral model
contains much simpler input and output blocks.
Based on above definitions and examples, in many cases the transistor level
models are the most complex (and accurate representation of the device) but
at the price of being most time consuming to simulate.
Best Regards,
Abe
-----Original Message-----
From: Muranyi, Arpad [SMTP:[email protected]]
Sent: Monday, September 18, 2000 10:36 AM
To: 'abe riazi'; '[email protected]'
Subject: RE: [SI-LIST] : Macromodel Creation
Abe,
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
slower.
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
it faster.
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
automatically slower.
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
suggest.
Arpad Muranyi
Intel Corporation
============================================================================
-----Original Message-----
From: abe riazi [mailto:[email protected]]
Sent: Friday, September 15, 2000 7:17 PM
To: '[email protected]'
Subject: [SI-LIST] : Macromodel Creation
Dear Scholars:
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).
2. Macromodels.
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
curves.
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
ascertain Cp.
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
capacitance meter).
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
macromodel generation.
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
curves.
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
.INCLUDE EXAMPLE.MOD
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
.ENDS CMACRO
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
frequency domain.
Reference 1. R. M. Kielkowski, "SPICE Practical Device Modeling",
McGraw-Hill, Inc. 1995.
Thanks for your comments and with best regards,
Abe Riazi
ServerWorks
2251 Lawson Lane
Santa Clara, CA 95054
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. 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
****
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. 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
****
**** To unsubscribe from si-list or si-list-digest: send e-mail to
[email protected]. 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 - 14:29:31 PDT