The Designer's Guide Community
Forum
Welcome, Guest. Please Login or Register. Please follow the Forum guidelines.
Oct 24th, 2020, 2:11am
Pages: 1
Send Topic Print
Large Signal S parameter Simulation (Read 8483 times)
Fei
Junior Member
**
Offline



Posts: 16

Large Signal S parameter Simulation
Apr 17th, 2004, 11:06am
 
Does anyone know how to set up  large signal S parameter simulations in SpectreRF?

Thanks

Fei
Back to top
 
 
View Profile   IP Logged
Andrew Beckett
Senior Fellow
******
Offline

Life, don't talk to
me about Life...

Posts: 1736
Bracknell, UK
Re: Large Signal S parameter Simulation
Reply #1 - Apr 17th, 2004, 11:34pm
 
It probably depends on what you mean by large-signal s-parameters. Large-signal s-parameters is really an oxymoron, since s-parameters are implicitly small signal.

I'm assuming you mean measuring s-parameters under some large signal bias condition? Well of course, that can be done in SpectreRF - set up whatever large signal bias condition (for example, temperature, supply, presence of blockers, with input in compression, etc, etc) you want, and then run psp.

My understanding from most people who ask for this is that they want to write out a single s-parameter file with information in it indicating the large signal condition followed by the s-parameters themselves - and possibly several conditions (found during a sweep).

There's no direct way of generating this file at the moment,  (there's an enhancement request in for this though), but it can be done using OCEAN - writing a script which does some kind of loop over various conditions and writes all this into a file.

Here's an example of doing this with an ordinary "sp"
analysis in OCEAN:

Code:
simulator( 'spectre )
;design("/user/andrewb/simulation/testsp/spectre/schematic/netlist/netlist")
design("test" "testsp" "schematic")
analysis('sp ?start "10"  ?stop "1G"  ?log "10"
    ?file "sparam.file"  ?datafmt "touchstone"  ?datatype "realimag"
)
results=resultsDir()
outputFile="./sp.file"
outputPort=outfile(outputFile)
foreach(temperature '(-40 27 125)
    temp(temperature)
    run()
    fprintf(outputPort "VAR temp = %d\n" temperature)
    spPort=infile(strcat(results "/netlist/sparam.file"))
    when(spPort
	  while(gets(line spPort)
		fprintf(outputPort "%s" line)
		)
	  close(spPort)
    ) ; when
) ; foreach
close(outputPort)
 



Regards,

Andrew.
Back to top
 
 
View Profile WWW   IP Logged
Fei
Junior Member
**
Offline



Posts: 16

Re: Large Signal S parameter Simulation
Reply #2 - Apr 18th, 2004, 7:12am
 
Thanks for your reply.  I guess this is a fairly common question in Microwave circuit design.  

It means that the input power of the circuit is large enough so that nonlinearity can not be ignored as it is in small signal S parameter analysis.  

Basically, you will have harmonics for a single tone input.  Sometimes it is interesting to know the S parameters for the single tone or harmonics.

I found that there are two possible ways to do the large signal S parameter analysis.

1. Just use regular SP analysis but with large input power;
2. PSS and PSP;

I got results are very similar in both cases.  I don't have too much experience in using Cadence, anyone has more experience please comment on this.

One more question, if the model provided by foundry can be used for large RF signal analysis?  Do one need a seperate large signal model for this purpose?

Thanks

Fei
Back to top
 
 
View Profile   IP Logged
Frank Wiedmann
Community Fellow
*****
Offline



Posts: 671
Munich, Germany
Re: Large Signal S parameter Simulation
Reply #3 - Apr 18th, 2004, 11:52pm
 
SP analysis is a linear analysis (just like AC analysis), so you will not see any nonlinear effects there. For a given bias point, you will get the same results for any input power you specify because with this simulation, the circuit is linearized about the bias point.

In order to see nonlinear effects, you will have to use the PSS/PSP analysis. If you get very similar results to the SP analysis, this means that the nonlinear effects do not have a significant effect on your results.

It depends on the type of the foundry model if this model includes nonlinear effects. For microwave design, there exist model types that only describe the linear behavior of the device (for a specified bias point).
Back to top
 
 
View Profile WWW   IP Logged
Frank Wiedmann
Community Fellow
*****
Offline



Posts: 671
Munich, Germany
Re: Large Signal S parameter Simulation
Reply #4 - Apr 19th, 2004, 1:49am
 
On second thoughts: even in the PSP analysis, the signals at the ports are considered to be small, so that the circuit reacts to them in a linear way. This can be very useful for mixer analysis but is probably not what you have in mind.

I suppose that you want to apply a large signal to port 1, look at the output you get at port 2 at the same frequency and calculate the corresponding S-parameters. I do not know of a direct way to do this in SpectreRF.

A possible method is to set up test configurations as described for example in http://eesof.tm.agilent.com/docs/iccap2002/MDLGBOOK/5SIMULATIONS/5Spice2Spar.pdf..., do a PSS analysis and calculate the results by using the formulas given there (with the voltage components at the frequencies of interest).
Back to top
 
 
View Profile WWW   IP Logged
Andrew Beckett
Senior Fellow
******
Offline

Life, don't talk to
me about Life...

Posts: 1736
Bracknell, UK
Re: Large Signal S parameter Simulation
Reply #5 - Apr 19th, 2004, 1:08pm
 
Frank,

I think you should be able to have a large signal input,
and then also find the s-parameters at the same frequency.
This gives you the small signal transfer function with a
large signal input driving the circuit into compression (or whatever) (doing this with psp).

So you set up your PSS with this large signal input, and then do the psp as normal.

Regards,

Andrew.
Back to top
 
 
View Profile WWW   IP Logged
Frank Wiedmann
Community Fellow
*****
Offline



Posts: 671
Munich, Germany
Re: Large Signal S parameter Simulation
Reply #6 - Apr 20th, 2004, 7:23am
 
Due to the linearization inherent in the psp analysis, this will not give the same results. I have verified this on a simple example.

By the way, Large-Signal S-Parameter Simulation (LSSP) is a built-in analysis type in Agilent's ADS or RFDE (see http://eesof.tm.agilent.com/docs/rfdedoc2003C/pdf/rfdecktsimlssp.pdf).
Back to top
 
 
View Profile WWW   IP Logged
Pages: 1
Send Topic Print
Copyright 2002-2020 Designer’s Guide Consulting, Inc. Designer’s Guide® is a registered trademark of Designer’s Guide Consulting, Inc. All rights reserved. Send comments or questions to editor@designers-guide.org. Consider submitting a paper or model.