The Designer's Guide Community
Forum
Welcome, Guest. Please Login or Register. Please follow the Forum guidelines.
Mar 28th, 2024, 1:38am
Pages: 1
Send Topic Print
use frequency as variable in SP simulation (Read 2441 times)
Ian
Junior Member
**
Offline



Posts: 27

use frequency as variable in SP simulation
Nov 20th, 2008, 7:14am
 
Dear all,

I'm simulating a transmission line with the model (e.g., the series resistance) only valid at a specified frequency. When I wanna do a swept frequency simulation (e.g., SP), I need to vary the frequency in the model as well. The question is how to access the 'frequency' variable in SP simulation?

Actually I met similar problem before when I want to specify the frequency dependent series resistance for the lossy inductor (i.e., 2*pi*freq*L/Q) in the SP simulation.

Any tips? Thanks.

Ian  
Back to top
 
 
View Profile   IP Logged
pancho_hideboo
Senior Fellow
******
Offline



Posts: 1424
Real Homeless
Re: use frequency as variable in SP simulation
Reply #1 - Nov 20th, 2008, 3:45pm
 
Ian wrote on Nov 20th, 2008, 7:14am:
When I wanna do a swept frequency simulation (e.g., SP), I need to vary the frequency in the model as well.
The question is how to access the 'frequency' variable in SP simulation?

What simulator do you intend to use ?

If you use Agilent ADS engine in RFDE or ADS native, you can use 'frequency' variable directly
in any analyses such as ac, sp, hb, envlp and tran. But you have to pay attention to causality issue for envlp and transient analysis.

If you use Cadence Spectre, you can not use 'frequency' variable even in small signal analyses such as ac, xf, sp and noise.
As workaround in Cadence Spectre, write frequency table of Y/Z parameters then use nport.

http://www.designers-guide.org/Forum/YaBB.pl?num=1225399560/0#3
Back to top
 
« Last Edit: Nov 21st, 2008, 2:12am by pancho_hideboo »  
View Profile WWW Top+Secret Top+Secret   IP Logged
Ian
Junior Member
**
Offline



Posts: 27

Re: use frequency as variable in SP simulation
Reply #2 - Nov 21st, 2008, 4:45am
 
Thanks, pancho_hideboo.

Unfortunately, I'm using Cadence SpectreRF. Seems I have to do single frequency point simulation for now.

Ian
Back to top
 
 
View Profile   IP Logged
sheldon
Community Fellow
*****
Offline



Posts: 751

Re: use frequency as variable in SP simulation
Reply #3 - Nov 22nd, 2008, 4:46am
 
Ian,

  Could you work around the issue by creating some variable,
voltage/current, proportional to the frequency? It would require
adding an additional terminal to your model in order to sense
the variable and modifying the model to replace frequency with
the variable, see the attached example. I have used this trick
when I needed to know the frequency in order to calculate
inductance, Q, ... from s-parameters. If your model is written
in Verilog-A, you could probably include the calculation in the
model.

                                                            Best Regards,

                                                               Sheldon
Back to top
 
View Profile   IP Logged
pancho_hideboo
Senior Fellow
******
Offline



Posts: 1424
Real Homeless
Re: use frequency as variable in SP simulation
Reply #4 - Nov 22nd, 2008, 5:28am
 
As another essential problem in Cadence Spectre, we can not define Z(omega)=R(omega)+j*X(omega).
In Agilent ADS simulator on RFDE or ADS native, we can write such complex impedance using "freq" variable directly.
There is no method to define complex impedance in Verilog-A.
Back to top
 
« Last Edit: Nov 22nd, 2008, 7:31am by pancho_hideboo »  
View Profile WWW Top+Secret Top+Secret   IP Logged
Peruzzi
Community Member
***
Offline



Posts: 71

Re: use frequency as variable in SP simulation
Reply #5 - Nov 22nd, 2008, 10:07am
 
pancho_hideboo wrote on Nov 22nd, 2008, 5:28am:
... we can not define Z(omega)=R(omega)+j*X(omega).
...
There is no method to define complex impedance in Verilog-A.


In Verilog-A you can express the complex impedance in terms of differential or integral equations for current and voltage.  Would this be okay for your application?

Best regards,

Bob Peruzzi
Back to top
 
 
View Profile   IP Logged
pancho_hideboo
Senior Fellow
******
Offline



Posts: 1424
Real Homeless
Re: use frequency as variable in SP simulation
Reply #6 - Nov 22nd, 2008, 7:29pm
 
Peruzzi wrote on Nov 22nd, 2008, 10:07am:
In Verilog-A you can express the complex impedance in terms of differential or integral equations for current and voltage.

Verilog-A is oriented to time-domain simulator and time-domain expression although it can work in small signal analyses such as AC, XF, SP and Noise.
There are still many bugs in Verilog-A for small-signal analyses.

If X(omega) are expressed as combinations of k*(omega**n) and k/(omega**n),
we can write j*X(omega) by using differential and integral equations. This is time-domain expression.

But for more generic X(omega), how to define or write using Verilog-A ? Here we need frequency-domain expession ability.
Such generic X(omega) naturally appear in microwave theory.

Only one frequency-domain expression in Verilog-A is rational Laplace expression. But this is equivalent to time-domain expression of differential and integral equations. For very limited style of X(omega), we can use frac-pole.

I have ADSsim on RFDE where frequency domain expressions are available, so I don't have to insist on using Cadence Spectre which require different tricky methods for each problem.
Back to top
 
« Last Edit: Nov 23rd, 2008, 6:27am by pancho_hideboo »  
View Profile WWW Top+Secret Top+Secret   IP Logged
jbdavid
Community Fellow
*****
Offline



Posts: 378
Silicon Valley
Re: use frequency as variable in SP simulation
Reply #7 - Dec 18th, 2008, 8:06pm
 
Those complex values are either Small signal quantities or  Base-band equivalent values..

these are useful in RF systems analysis, so you should put that part of your design in an RF system simulator like ADS  or matlab, and link that to the actual circuit (specified in a model valid for both large and small signals) running in spectre.
RFDE allows Spectre/ADS/Ptolemy co-simulations, and the simulink interface allows spectre&simulink to work together.

Of course this has been a request for years and years.. and probably NOT something solved in a spice-type simulator any time soon.

Jbd
Back to top
 
 

jbdavid
Mixed Signal Design Verification
View Profile WWW   IP Logged
pancho_hideboo
Senior Fellow
******
Offline



Posts: 1424
Real Homeless
Re: use frequency as variable in SP simulation
Reply #8 - Dec 18th, 2008, 10:49pm
 
jbdavid wrote on Dec 18th, 2008, 8:06pm:
Those complex values are either Small signal quantities or  Base-band equivalent values..
these are useful in RF systems analysis,

No, you are misunderstanding.
I don't mention equivalent lowpass model which is called as baseband model in Cadence where only complex envelope I(t)+j*Q(t) are concerned.
And both Ptolemy and Simulink are time domain simulator in signal flow model(not energy conservative system), although they can treat s-parameter box as complex coefficient FIR model.

I'm mentioning about Analog RF simulation of wireless or high speed wired application in full transistor level circuits.

Also a start of this thread is regarding small signal analyses such as AC, XF, SP and NOISE.

jbdavid wrote on Dec 18th, 2008, 8:06pm:
Of course this has been a request for years and years.. and probably NOT something solved in a spice-type simulator any time soon.

At least, a convolution of Agilent ADSsim is superior than Cadence Spectre as a spice-type simulator.
And feature of convolution of Agilent ADSsim is that it is not restricted to NPORT.

Cadence has insisted on rational fitting(linear macro model fitting) about s-parameter in transient analysis
and denied convolution for long long time.
But recently, Cadence recommend user to use convolution and don't recommend rational fitting.
Rather Cadence is denying rational fitting now.
http://www.designers-guide.org/Forum/YaBB.pl?num=1174585355/1#1
Back to top
 
« Last Edit: Dec 19th, 2008, 6:12am by pancho_hideboo »  
View Profile WWW Top+Secret Top+Secret   IP Logged
Pages: 1
Send Topic Print
Copyright 2002-2024 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.