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 20th, 2008, 7:14am |
Title: use frequency as variable in SP simulation Post by Ian on 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 |
Title: Re: use frequency as variable in SP simulation Post by pancho_hideboo on Nov 20th, 2008, 3:45pm Ian wrote on Nov 20th, 2008, 7:14am:
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 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 |
Title: Re: use frequency as variable in SP simulation Post by sheldon on 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 |
Title: Re: use frequency as variable in SP simulation Post by pancho_hideboo on 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. |
Title: Re: use frequency as variable in SP simulation Post by Peruzzi on Nov 22nd, 2008, 10:07am pancho_hideboo wrote on Nov 22nd, 2008, 5:28am:
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 22nd, 2008, 7:29pm Peruzzi wrote on Nov 22nd, 2008, 10:07am:
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 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 |
Title: Re: use frequency as variable in SP simulation Post by pancho_hideboo on Dec 18th, 2008, 10:49pm jbdavid wrote on Dec 18th, 2008, 8:06pm:
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:
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 |
The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved. |