The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> RF Simulators >> How could I sim. VCO + Mixer + LNA in spectre ?
https://designers-guide.org/forum/YaBB.pl?num=1067781345

Message started by Charles CHENG on Nov 2^nd, 2003, 5:55am

Title: How could I sim. VCO + Mixer + LNA in spectre ?
Post by Charles CHENG on Nov 2^nd, 2003, 5:55am

Dear all,

I have a question about the spectre simulation method of the VCO + Mixer + LNA. I hope anyone could help me.

Actually, I have successfully simulated the VCO and Mixer+LNA separatedly using the spectre. Which is using the special function, such as pss, pxf or pnoise etc, to simulated the phase noise, oscillating frequency
in the VCO and 1dB compression point, iip3 or power gain in the Mixer+LNA.

However, how could I simulate the overall circuit, VCO+Mixer+LNA, to get the simulation result such as 1dB compression point, iip3, noise figure etc.?

Best Regards,

Charles

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by Ken Kundert on Nov 3^rd, 2003, 10:38am

Computing the NF of the three blocks combined is straight forward, however computing P1dB or IP3 is not possible because SpectreRF currently does not allow an autonomous circuit, the VCO, to be driven by a large tone, the input signal. However, this is generally not a problem. One does not normally include the VCO when using simulation to predict P1db, iIP3, and NF of the LNA & mixer because the VCO does not substantially affect these performance metrics.

However, having said that, these metrics are affected by the phase noise of the VCO when a large blocker in present. In this case, one would want to co-simulate the LNA, mixer, and VCO. In this situation, the best approach is to simulate the VCO alone, determine its phase noise, and then replace the VCO with a behavioral model that produces the same phase noise but is not autonomous. This procedure is described in Introduction to RF simulation and its application, which can be found at http://www.designers-guide.com/Analysis. Look in 6.3.3 on page 38.

-Ken

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by Charles CHENG on Nov 3^rd, 2003, 10:21pm

Dear Ken,

I am very thanks for your helping. In your reply, you said that the Noise Figure of the LNA+Mixer+VCO is straight forward. However, I don't know how to simulate it. Could you teach me also.

Best Regards,

Charles CHENG

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by Ken Kundert on Nov 4^th, 2003, 4:42pm

To compute noise figure you need a port at the input of the LNA, which would be set to produce a constant-valued (DC) input. You would then perform a PSS analysis to determine the large signal operating point. In this case, it is the oscillator that is setting that operating point. The PSS analysis starts with a transient analysis, you will need to use initial conditions or an input pulse to start the oscillator. Once it is started, set the PSS tstab parameter to give the oscillator sufficient time to settle down. That will allows the PSS analysis to converge without difficulty. Then perform a PNoise analysis. With the port defining the input to the circuit, SpectreRF will naturally compute the noise figure.

-Ken

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by Mark Gehring on Nov 18^th, 2004, 1:04pm

You can however, do the complete simulation of LNA+mixer+real VCO in EldoRF.

Mark

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by Eugene on Jan 4^th, 2005, 6:59pm

I would like to make one very minor side comment about noise figure and Spectre/SpectreRF. The default port temperature is something like 16.8 degrees C. However, the default temperature of the rest of the circuit is 27 degrees C. The temperature difference affects the noise figure measurement only by a few tenths of a dB so you probably would not notice it. I stumbled upon the difference because I wanted to check my noise figure test bench with behavioral models and the test bench did not produce the exact noise figure I specified. Changing the port temperature to 27 degrees produced the exact noise figure I specified in the behavioral model.

(The correct thing to do may very well be to add a temperature parameter to the behavioral model to account for the circuit temperature for which the noise figure is defined, but that is a modeling issue that probably does not belong in this thread.)

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by Frank Wiedmann on Jan 4^th, 2005, 11:33pm

The default port temperature is different from the default temperature of the rest of the circuit because the standard noise temperature is usually defined to be 290 Kelvin (see http://glossary.its.bldrdoc.gov/fs-1037/dir-024/_3560.htm).

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by Eugene on Jan 5^th, 2005, 8:47am

Frank,
Thanks for the link. That's one of the best definitions of noise figure I've seen, especially since it addresses the image frequency. This helps justify the way my group distinguished between noise figures of direct conversion receivers and super het receivers. It seems the correct approach to modeling noise in a behavioral model is indeed to account for the difference between circuit temperature and noise source temperature.
-Eugene

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by milkdragon on Aug 31^st, 2005, 6:28pm

For the NF simulation in SpectreRF, should i change the RF port resistance to 0Ohm. I am asking this because i found out in the noise summary that almost 70% of the noise is dominated by the source of the RF port

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by Jess Chen on Aug 31^st, 2005, 8:36pm

I have never tried setting the port resistance to zero but I am not sure it would be a good idea. The port would only deliver the desired signal level if the port drove a short. For any finite load, you would see double the desired signal.

But why would you want to eliminate the port noise? The port noise is necessary for computing noise figure. If you still want to simulate noise only from the circuit, without any contribution from the port, and you still want to use the port for gain etc., I would eliminate the port noise by setting the port's noise temperature to -273.15 degrees C (zero Kelvin).

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by milkdragon on Sep 1^st, 2005, 8:31am

Thank you for your reply. I do agree with u. I got my LNA NF ~ 1.7dB with Gain of 28dB, and mixer NF ~10dB. However, when i hook them up, the NF is 5dB...... I am thinking if i did something wrong with my setup.

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by milkdragon on Sep 1^st, 2005, 8:38am

Oh, one more thing, anybody tried to simulate Mixer + LNA + divide-by-2 circuit. Could you tell me if you know how to do that

Thank you

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by Jess Chen on Sep 1^st, 2005, 7:16pm

I did some back-of-the-envelope calculations using your numbers. I came up with a noise figure of 1.77dB if I assume that your LNA input is matched but your LNA output is an ideal voltage source and your mixer output is at baseband. If I assume you simulated SSB noise figure instead of DSB noise figure, we add 3dB to get 4.77dB, which is not too far from 5dB. So I think the issue might be a combination of set up (SSB instead of DSB) and doing manual calcuations without accounting for the mismatched baseband output. There's a factor of 4 in the Friis formula associated with the mismatched output and a factor of 1/2 associated with the baseband mixer output.

NF=
10log(10^(1.7/10)+(4/2)*(10^(10/10)-1)/10^(28/10))

+3dB (for SSB mistake) = 4.77dB.

Where is your divide by 2 operation located in the chain?

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by milkdragon on Sep 1^st, 2005, 7:25pm

Thank you,

Actually i put the divider circuit on the LO side, i would like to see if i can simulate the NF with divider also

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by Jess Chen on Sep 1^st, 2005, 9:05pm

If you are using SpectreRF, the divider will have to be a device level model or a clever behavioral model. You can not use a simple behavioral model because it will have hidden state. You would have to use a resettable integrator or a capacitor. A device level model would work but it might slow things down some. Anyway, if your model is SpectreRF compatible, you should be able to introduce the divider as long as you introduce a lower frequency fundamental (half) in the PSS analysis and change your side band options.

Title: Re: How could I sim. VCO + Mixer + LNA in spectre
Post by milkdragon on Sep 2^nd, 2005, 9:45am

Thank you for your suggestion