How to add a flicker noise source to a component ?

Hopefully I can reply now - I had some trouble yesterday.

Anyway, the vsource, isource and port components have a "noisefile" parameter which can be used to add noise. If however you want it to be dependent on the value of the source, you'll probably need to write a VerilogA model since that has noise sources as part of the language (flicker_noise(), white_noise()).

Regards,

Andrew.

 Hi,

OK, I read a little bit about Verilog-A. The functions that you cited (flicker_noise(), white_noise()) are only active in small-signal noise analysis. To clarify, the noise has to be considered as a small-signal in the analysis but the circuit can be analysed with large-signal, isn't it ? So can I use this function in an oscillator phase noise analysis (pnoise after a pss) ? 

With a Verilog-A block, can I use the Spectre simulator or I have to use SpectreVerilog ?

Regards,

Emmanuel

Hi Emmanuel,

VerilogA is supported in spectre, UltraSim and APS - it does not require a digital engine (it also works in AMS and also SpectreVerilog, because the analog solver is in both).

If you use the flicker_noise() and white_noise() functions, they are treated as small-signal noise sources (normally) and so the noise affects the simulation results in any small-signal noise simulation - so that could be noise, sp, pnoise, psp, qpnoise, qpsp, hbnoise analyses. Note that the "p" and "qp" and "hbnoise" analyses are actually small signal analyses, although they are biassed around a large signal solution (from pss, qpss, hb analyses) which captures the circuit's non-linear response to a large signal. They do not however capture the circuit's non-linear response to the noise (normally that's OK, because usually the circuit does not have significant large signal response to the noise).

So yes, you can use them in oscillator phase noise analysis.

It's also possible to use transient noise (enabling the noise sources during a transient). If you do this, your VerilogA noise sources will generate noise during the transient and thus your circuit can have a large signal response to that noise. Note that this is not a terribly efficient way of measuring noise, but it can be useful when you have either non-periodic behaviour or the circuit will distort based on the size of the noise sources (i.e. has a non-linear response to the noise).

Best Regards,

Andrew.

 Hi,

I made a verilog-a block to generate a flicker_noise dependent of the current circulating in the branch :

------------------------------------------------------------------------------------------------------

`include "discipline.h"
`include"constants.h"

module flicker_source(nplus,nmoins,probep,probem);
output     nplus,nmoins;
input       probep,probem;
electrical nplus,nmoins,probep,probem;
 parameter real kf = 1.0;
 parameter real af = 1.0;
 parameter real ef = 1.0;
                
   analog begin
      I(nplus, nmoins) <+ flicker_noise(kf*pow(abs(I(probep,probem)),af),ef);
   end
endmodule

---------------------------------------------------------------------------------------------------------

But testing this block with a simple circuit, a resistor with a current source, I obtain incoherent results. In theory, if I apply a DC current to the resistor, I should obtain a 1/f noise around the DC. And if I apply just the pump at f0, I should obtain a 1/f noise around f0. But, it is not the case. In both cases, I obtain noise around the DC.

When I apply the DC and the pump at the same time, I obtain noise around DC and f0 but with incoherent levels.

Thinking the flicker_noise() function present a problem, I did another test using this function just to generate a constant 1/f noise (not current dependent). Then, I create another verilog-a block to read this fixed noise, read the current flowing through the resistor and multiply these two values to generate the final noise. The result is exactly the same.

My conclusion is that it exists a real problem with the simulator. Maybe, it's impossible to simulate cyclostationnary noise. But I hope I'm wrong and someone can give me the solution.

Regards,

Emmanuel

This ought to be possible - modelling noise and cyclostationary noise is certainly possible. This model isn't actually generating cyclostationary noise, but presumably the circuit is supposed to be translating that noise up in frequency, and the periodic nature of the circuit should result in cyclostationary noise?

Not really that easy to see what's going on without seeing the test circuit you're using. I suggest that if you can't post that here, you contact Cadence Customer Support, when we can work through this in more detail.

Regards,

Andrew.