[SI-LIST] Re: N-port model limitations in simulators

Hi, Larry,

Yes, a synthesized RCL model would be looked drastically different from 
a physical RCL model, if there is one. However, they would represent the 
same physical part, and, their terminal behavior should be very close, 
if not identical. S-, Y-, Z-parameters are black-box, data models. All 
we can say is their terminal behaviors. They don't have physical 
equations to represent internal structures, thus they don't have the 
property of predictability. However, they do reflect the physical part 
they represent. And from that, you can tell some physical property of 
the system, for instance, transmission line's length, delay, etc.

I agree that a data model (S-, Y-, Z-parameter) should be accompanied 
with a detailed physical description of the structure (a connector, a 
cable, a T-line), and warn the user the conditions and limitations of 
the model. Thus, as long as a data model describes the physical part 
accurately and is used correctly, a circuit simulator should happily 
accept it and faithfully give out corresponding transient behavior. 
Inaccurate model as well as incorrect usage of a model should not take 
us to a conclusion that it is S-parameter's fault.

Hope the above is convincing not confusing.

-- 

Regards,

Yu
===

Apache Design Solutions
1881 Landings Drive
Mountain View, CA 94043
Tel:  (650)237-5410
Fax:  (650)969-4170
Email: yu_liu@xxxxxxxxxxxxx
web: www.apache-da.com




Larry Smith wrote:

>Yu - If you look into the "black box" for S, Y or Z parameter models,
>you will see a bunch of cross coupling terms, i.e. sig1L to sig2L,
>sig3L, sig1R, sig2R, sig3R, etc.  You may even be able synthesize RLC
>components between the terminals that will give an identical transfer
>function.  But those R's, L's and C's bear little resemblance to the
>physical part.
>
>You can pick up a connector, look at it, and know that there should be
>a resistance and inductance between two of the terminals and
>capacitance to another.  You can estimate the impedance in the common
>return path by the dimensions of the conductor.  If you mathematically
>transform the matrix to get rid of the impedance in the return path
>(reduce from 2 reference nodes down to 1 reference node), I believe you
>can still get accurate simulation results, but you loose all intuition
>into the way the physical dimensions of the part affect the electrical
>performance of the model.  It will be difficult (for me anyway..) to
>look into the manipulated model and know if it includes the properties
>needed for SSN analysis or not.
>
>Yes, your near-end far-end rule makes sense.  SI engineers do this
>naturally with transmission line models.  If we drew a circuit topology
>with a 20 inch transmission line, we know better than to hook a
>resistor across the time delay of the element.  The same type of thing
>applies to the S, Y or Z black box.  There will be certain nodes that
>may be grouped together and attached to lumped element circuits and
>others that cannot.  And if you hook a resistor between the wrong nodes
>of the black box, the circuit simulator will give you incorrect
>results, just as if you did the same thing with the transmission line.
>It is not the fault of the circuit simulator, but it his how the models
>were assembled and used.  The point that I am trying to make is that
>you can just look at simple spice models and know this but with S, Y or
>Z models it is not obvious.
>
>After this great discussion on SI-list, I am convinced that the number
>of reference nodes does not confuse the circuit simulator, but is
>highly likely to confuse the person doing the circuit simulation.  The
>simulation code is able to handle what ever problem it is given.  The
>question is whether the person at the keyboard can connect the models
>and interpret the results correctly.
>
>Do the simulated models contain enough information to solve the problem
>the person thinks he is solving?  I am not convinced that S parameter
>models will handle the SSN problem.  I think it depends a lot on how
>the model was developed and how it was hooked up and simulated.  The
>number of terminals and ports for the model has a lot to do with this.
>
>regards,
>Larry Smith
>Sun Microsystems
>
>>Delivered-To: si-list@xxxxxxxxxxxxx
>>Date: Mon, 28 Apr 2003 22:02:36 -0700
>>From: Yu Liu <yu_liu@xxxxxxxxxxxxx>
>>To: Larry.Smith@xxxxxxx
>>Cc: si-list@xxxxxxxxxxxxx
>>Subject: [SI-LIST] Re: N-port model limitations in simulators
>>
>>Hi, Larry,
>>
>>I think you can tell the coupling effects by "looking" at the 
>>S-parameter data: although S- (Y-, Z-)parameter data  are "black box" 
>>models, they represent the terminal behavior of a physical network. In 
>>addition, from S-parameter, you can obtain the more comfortable RLGC 
>>parameters of the system, which may give you some insights of the 
>>network in a more easily understandable way.
>>I agree that since S-parameter is usually used to model the distributed 
>>effects, great care should be taken on how it should be connected with 
>>other parts of the circuit. A typical rule is the "near end/far end" 
>>rule, but sometimes even "near end" should be treated as distributed 
>>part. A circuit simulator can't tell you not connecting the two ends of 
>>a 20-inch long T-line with a lumped simple resistor, but it should 
>>faithfully give you the "wrong" results. I agree that every terminal 
>>should have its accompanied reference, just for the flexiblity of the 
>>usage. However, as Steve pointed out, this may not necessarily improve 
>>the accuracy of the model (no new information is added into the model).
>>
>>-- 
>>
>>Regards,
>>
>>Yu Liu
>>========
>>
>>Apache Design Solutions
>>1881 Landings Drive
>>Mountain View, CA 94043
>>Tel:  (650)237-5410
>>Fax:  (650)969-4170
>>Email: yu_liu@xxxxxxxxxxxxx
>>web: www.apache-da.com
>>
>>
>>
>>Larry Smith wrote:
>>
>>>Joel - Thanks for your note back.  Also, thanks to the several
>>>responders to this thread that Ray started.  The basic question at
>>>stake here is "How do we use S parameter models to represent the
>>>interconnect components, commonly found in our computer systems, in a
>>>circuit simulator?"  Perhaps I am mixing up two processes (modeling of
>>>a circuit component; solving a set of circuit equations), but I think
>>>it is necessary to have a fundamental understanding of both in order to
>>>get correct answers from a circuit simulator.
>>>
>>>For example, a connector vendor may hand you two simulatable spice
>>>models for his connector that are very different in nature.  The first
>>>spice model may use the same reference node for the left and right side
>>>of the connector.  The second model may have an inductance and a
>>>resistance between the left and right reference nodes.  The first model
>>>is valid for waveforms and delay from one side to the other.  The
>>>second is valid for waveforms including the effects of simultaneous
>>>switch noise (SSN) as return current for each signal flows through a
>>>common impedance.  The person doing the simulation has to decide which
>>>model to use and how to use it.  If he hooks the left and right
>>>reference nodes of the second model to spice node zero, he will get
>>>incorrect results.  Here is an example where the person doing the
>>>simulation needs to know something about the assumptions made by the
>>>person who made the model.  In the case of a simple spice model, it is
>>>easy to look into the spice code and figure it out.  However, this is
>>>not true with an S, Y or Z parameter models.
>>>
>>>         ...............                     ...............
>>>         :             :                     :             :
>>> sig1L o-:-LLLL---RRRR-:-o sig1R     sig1L o-:-LLLL---RRRR-:-o sig1R
>>>         :             :                     :             :
>>> sig1L o-:-LLLL---RRRR-:-o sig1R     sig1L o-:-LLLL---RRRR-:-o sig1R
>>>         :             :                     :             :
>>> sig1L o-:-LLLL---RRRR-:-o sig1R     sig1L o-:-LLLL---RRRR-:-o sig1R
>>>         :.............:                     :             :              
>>>                |                    gnd1L o-:-LLLL---RRRR-:-o gnd1R     
>>>               ref                           :.............:            
>>>
>>>          Spice Model 1                       Spice Model 2
>>>
>>>It is possible to transform model 2 into a model with just one
>>>reference node.  Brian Young has a nice discussion on this in his
>>>chapter on inductance.  Through matrix manipulation, the voltage on the
>>>reference node on the right side can be made identical with the
>>>reference voltage on the left side.  The relationship between all the
>>>voltages on the left side remains the same; the relationship of all
>>>voltages on the right side remain the same; and the currents into each
>>>node remain the same.  But, don't look inside the model!  All you will
>>>see is a bunch of equations and parameters (Y or Z).  The parameters in
>>>the black box will be very different for model 1 and model 2 after
>>>model 2 has been converted to have a single reference node.  The
>>>parameters for model 2 will give you SSN information, the parameters
>>>for model 1 will not, but it will be impossible to tell that by
>>>inspection.
>>>
>>>Now, back to the discussion on the number of terminals for N ports.
>>>Suppose we have an S parameter model for this connector that came from
>>>either lab measurements or EM extraction.  If we measured this connector
>>>in the lab, we would probably say that it has 6 ports, 3 on the left
>>>and 3 on the right.  We would attach VNA port 1 between a signal and
>>>it's reference, port 2 between another signal and it's reference and 50
>>>Ohm terminations between the other signal and reference nodes. Many
>>>measurements are required, attaching and reattaching the VNA until all
>>>6 port parameters are obtained.  We would say that the connector has 12
>>>terminals, two for each port.
>>>
>>>Next we need to bring the S parameter model for the connector into a
>>>circuit simulator.  We desire to attach two circuit boards together
>>>with the connector.  Other components in the circuit simulator may
>>>include two sets of 3-coupled-transmission lines, a socket and two
>>>electronic packages that are positioned between two nonlinear circuits
>>>(driver and receiver).  
>>>
>>>The S elements in the circuit simulators that I am familiar with have 7
>>>terminals for the 6 port connector.  Each of the packaging components
>>>may have S parameter models with 7 terminals for the 6 ports.  Some of
>>>the components (transmission lines) are long compared to a wavelength
>>>which invalidates the quasi-static assumption.  Other components 
>>>(connector and possibly the electronic packages) have partial
>>>inductance from the left side to the right.  Each of the components
>>>have issues with voltage uniqueness.  As long as you stay on the left
>>>side or the right side, all voltages have the correct relationship.
>>>But measuring voltages across the component is like measuring voltage
>>>across time or across partial inductance, neither of which is valid.
>>>
>>>We want know the openness of the eye diagram at the receiver after
>>>simulating all of these models cascaded together.  The two choices are
>>>to 1) transform the models to the time domain and do a transient
>>>simulation, or 2) Simulate in the frequency domain and transform the
>>>results to the time domain (but that discussion is beyond the scope of
>>>this thread).  A whole bunch of questions come up for this simulation:
>>>
>>>1) Will the S parameter model for the connector give information about
>>>SSN?  As discussed above, connector model 2 will give SSN information,
>>>even with the 7 terminal version, but you can't tell that by looking at
>>>the model.
>>>
>>>2) How do S parameter models handle impedances in the return path?
>>>This is extremely important for the SSN and crosstalk problems.  It
>>>seems that the measurement technique mentioned above has not obtained
>>>enough information to deal with the return path impedance.  If we
>>>wanted to measure the impedance between the left and right reference
>>>terminals, how would we do it?  Which terminals would we connect the
>>>VNA to?  If we get another reference plane involved, where should it
>>>be located?
>>>
>>>3) How many terminals should an N Port box have in a circuit
>>>simulator?  It might make sense to have a reference point for every
>>>portion of the circuit that is separated from another portion by a
>>>significant time delay or set of partial inductances.
>>>
>>>4) What are the rules for connecting the terminals in the circuit
>>>simulator?  It seems obvious that you would not want to connect a
>>>resistor across the length of a 20 inch transmission line, but is there
>>>anything in the S parameter model that tells us not to do this?  It 
>>>seems that there should be a set of terminals that can have lumped
>>>element models connected between them and another set that cannot.
>>>This would be the groupings mentioned in question 3.
>>>
>>>In summary, I think that in order to make a simulatable circuit model,
>>>you have to know a lot about the environment where it will be used.  In
>>>order to correctly use a circuit model in a simulator, you have to
>>>understand the assumptions that were made when the model was built.
>>>With simple spice RLC models, it is fairly easy to just look at the
>>>models and know.  With S, Y and Z models, I don't think you can tell by
>>>inspection.  The way that a model must be used may have already been
>>>determined by the number of reference nodes that it has.  I am not
>>>convinced that S parameters capture the impedance in the return path
>>>that is necessary for crosstalk and SSN simulations.  This has a lot
>>>to do with the number of terminals assumed when developing the model
>>>and using the circuit simulator.  (Can anybody help me or am I beyond
>>>help??)
>>>
>>>All comments welcome..!  Sorry for the long email.
>>>
>>>regards,
>>>Larry Smith
>>>Sun Microsystems
>>>
>>>PS - I just scanned some of the previous responses on this thread and
>>>have obtained new insights into some of the things mentioned by Ege
>>>Engin, Jian Zheng, Marek Schmidt-Szal and others.  They have already
>>>pointed out many of the issues above.  Perhaps the examples presented
>>>here will make the issues clear to other people.  I could not really
>>>understand the issues until they were associated with a clear example.
>>>
>
>
>




------------------------------------------------------------------
To unsubscribe from si-list:
si-list-request@xxxxxxxxxxxxx with 'unsubscribe' in the Subject field

or to administer your membership from a web page, go to:
http://www.freelists.org/webpage/si-list

For help:
si-list-request@xxxxxxxxxxxxx with 'help' in the Subject field

List archives are viewable at:     
                http://www.freelists.org/archives/si-list
or at our remote archives:
                http://groups.yahoo.com/group/si-list/messages 
Old (prior to June 6, 2001) list archives are viewable at:
                http://www.qsl.net/wb6tpu

Other related posts: