SSB Phase Noise / SPICE model

Hello all,

Does anyone is able to tell me if the SPICE model file of a BJT transistor (in e.g. 2N2222A or BFR92A) used in a crystal oscillator simulation design and operating at low frequency (10 MHz) is proper for obtaining simulated results of SSB phase noise ? I mean if in case it would result good correlation with the measurement results ?

I have built the electrical representation of the XTAL according to the data from the manufacturer (R1, C1, C0, Fs) and other elements without any problem at the AWR MWO but unable to obtain the results of SSB PN.

Please note that I am looking for the 1/F3; 1/F2, 1/F and F regions; and maybe it will not be possible to replicate all regions, the question remains if the short term and long term correlations will be able to be replicated. I am suspicious the SPICE model is not adequate for such kind of plot results.

Still, if it would not be possible, what would you recommend otherwise ?

Thank you.

Usually the Spice models of those transistors don't have the flicker noise parameters set, and you cannot trust the SSB phase noise simulation in that region.
Anyway, BJTs have pretty good flicker noise, compared to other processes as CMOS or GaAs, so you can live to what you get.

Sadly to say, I fully agree with vfone. All devices in spice when using transient simulation are noise free. You may think to add some voltage and current noise source yourself to see what happens. theoretically tnis is possible, but: A crystal has high Q factor, so you need a very long run time before it stabilizes. Your run time will be even much looooonger because of the addition of the low frequency noise. You are interested in phase noise say about 100 Hz to kHz from the carrier. To get a useful spectrum view of the time domain results, you need run times in order of 0.05s. when using a 10 MHz oscillator, that are 500k RF cycles.

As vfone says, go for a BJT (with flat current gain versus Ic curve). Use metal film resistors, good low noise power supply and make sure that you use a circuit that uses the full quality factor of the crystal, try to avoid collector base saturation.

If you designed a good crystal oscillator, you need a very good setup to measure the phase noise (you may know that already).

Thank you vfone and WimRFP !

I may try implement through this article (**broken link removed**), please see as from slide 102 covering Bipolar Noise.
I already have the oscillator prototype working with very good characteristics, I just need to learn how to model the souces of noise, each one corresponding to a different region.

WimRFP are you in Netherlands ? Ik ook !

The linked paper is talking about many noise modelling details, but as far as I see, it does not presume to determine noise in transient analysis.

I think, you'll be able to find out some noise properties of your oscillator circuit in AC respectively noise analysis.

Hi FvM,

Could you give me an indication where to look for ? Any bibliography it would be OK to start with.

Thanks

Hello Enrico,

I am near Utrecht! To circumvent long simulation runs in transients analysis, there is a workaround to find the sensitivity of your circuit for noise current and voltage.

You may know that the LF noise of the transistor causes the noise sidebands close to the carrier. You can put current and voltage sources at positions where the noise is in real world. When you do a transient simulation with "DC" noise (just a current or voltage offset) you can find d(freq)/d(offset) for that particular source. Once you know the sensitivities, you should be able to map the actual noise spectral densities for the current and voltage noise source (from BJT and passives) to side band noise.

As the FM modulation index due to the noise is very small, you can use a linear transformation (you are in the linear part of the bessel functions). You may reduce the Q-factor of the crystal resonator to reduce simulation time and make a correction for the reduced Q-factor. Halving the Q-factor for the crystal doubles d(freq)/d(offset).

You could do this with AC simulation, but this may mask non-linear effects in the actual oscillator.

If there are (electrolytic) capacitors that behave as a short circuit for the LF noise, you should replace them for DC voltage sources, otherwise you will get bad results.

Unfortunately it's just an idea to determine the noise generated by the oscillator circuit in noise analysis, superimpose it with the sine signal and calculate phase noise. There are some special points to consider, e.g. the gain of the oscillator loop must be reduced for analysis purposes below the stability margin.

@FvM: The required loop gain reduction (so you have to modify the circuit and you can't see influence of BC junction and bias point shift) is the reason that I would prefer transient analysis.

Yes, when nonlinear effects have to considered, either transient analysis or specific models describing the noise and signal intermodulation are necessary. Spice noise analysis can only give noise density as input information in this case. Noise sources in transient analysis would be inplemented as pseudo random sequences I presume?

I wonder if we can approximately ignore nonlinear effects when the oscillator circuit implements amplitude control clearly below the available voltage swing?

If you are sure the swing is well within the maximum available current and voltage swing, you can use AC analysis. So I agree with your point of view. It saves you lots of simulation time.

Regarding the noise sources in transient: I would take a DC source (or DC stepped source) to see how much the frequency changes because of that DC voltage or current shift. Simulating with real LF pseudo random noise will take too much time I think

Hello Again,

I managed to obtain nice results of SSB phase noise from the XTAL oscillator (with high-Q), also accurate output power level and supression for the harmonics. It took me just few seconds to plot the results using the Harmonic Balance Solver from ADS.

The way I overcomed the problem for model the flicker noise (1/F) was adding the AF (Flicker Noise Expoent) and KF (Flicker Noise Coefficient) parameters in a Gummel-Poon model and through equations commanding a current source plugged in between the transistor base to inner emitter terminals, the equation is based on measured values taken from different biasing points and frequency for an specific transistor (2N2222A and BFR92A), which also can be extracted through the IC-CAP software from Agilent.

It required no effort or needs in the work around for loop gain reduction, sensitivity, etc. and the SPICE model is not limited to be used with transient solver only.
I am pretty much satisfied with the results, I was able to obtain good correlation between measurements.

Now I will tackle other slope regions for the noise, which different elements are responsible for. There will be a limit at close-to-carrier region due to the turn-over cutt-off frequency due to the XTAL oven.....but so far I have made a huge progress working by my own.

Regards.