The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> RF Simulators >> use frequency as variable in SP simulation
https://designers-guide.org/forum/YaBB.pl?num=1227194040

Message started by Ian on Nov 20^th, 2008, 7:14am

Title: use frequency as variable in SP simulation
Post by Ian on Nov 20^th, 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

Title: Re: use frequency as variable in SP simulation
Post by pancho_hideboo on Nov 20^th, 2008, 3:45pm

Ian wrote on Nov 20^th, 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

Title: Re: use frequency as variable in SP simulation
Post by Ian on Nov 21^st, 2008, 4:45am

Thanks, pancho_hideboo.

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

Ian

Title: Re: use frequency as variable in SP simulation
Post by sheldon on Nov 22^nd, 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

Title: Re: use frequency as variable in SP simulation
Post by pancho_hideboo on Nov 22^nd, 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.

Title: Re: use frequency as variable in SP simulation
Post by Peruzzi on Nov 22^nd, 2008, 10:07am

pancho_hideboo wrote on Nov 22^nd, 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

Title: Re: use frequency as variable in SP simulation
Post by pancho_hideboo on Nov 22^nd, 2008, 7:29pm

Peruzzi wrote on Nov 22^nd, 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.

Title: Re: use frequency as variable in SP simulation
Post by jbdavid on Dec 18^th, 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

Title: Re: use frequency as variable in SP simulation
Post by pancho_hideboo on Dec 18^th, 2008, 10:49pm

jbdavid wrote on Dec 18^th, 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 18^th, 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