I tried to design a frequency to current converter in phase domain using Ken's phase noise paper. The block will take the phase output of the VCO as input and give a current as output, which I will sum with the charge pump current. You can see the code below.

When I run a transient simulation using spectre, the ouput current is between -9mA and -11mA, whereas I set it to be between -1mA and 1 mA. I gave the frequency to the output as well and saw that required 9G-11G is calculated.

In the simulation, spectre gives warnings in at 10e-24 stating that minimum time step is used and solution can be in error. And in the begining of the simulation, current output goes to -9mA and continues as expected afterwards. What can be the reason for this initial error and how can I fix it? Can it be a bug in verilogA or did I use a wrong coding style?

Emre


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


discipline phase
     potential Angle;
enddiscipline

nature Frequency
     abstol = 1m;
     access = FF;
     units = "Hz";
     blowup = 2e10;
endnature

discipline freq_current
     potential Frequency;
     flow Current;
enddiscipline

module F2Iconv(Out,Fout_osc,In);

output Out; current Out;
input In; phase In;

output Fout_osc; freq_current Fout_osc;

parameter real Imin=-1e-3;                            // minimum output current
parameter real Imax=1e-3 from (Imin:inf);                      // maximum output current
parameter real Fmin=9G from (0:inf);            // minimum input frequency (Hz)
parameter real Fmax=11G from (Fmin:inf);      // maximum input frequency (Hz)

parameter real n = 0 from [0:inf); // white output current noise (A2/Hz)
parameter real fc = 0 from [0:inf); // flicker noise corner frequency (Hz)

parameter real Iinit=0;     // initial output value.

real Freq, Iout;             // computed frequency & output voltage.


analog begin
 @(initial_step) begin
    Freq=0;
    Iout=Iinit;
 end


     Freq =ddt(Theta(In))/ `M_TWO_PI;               // compute the frequency,
                                         
                             // and inversely proportional output current.
 
Iout= ((Freq - Fmin) / (Fmin - Fmax))*(Imax - Imin) + Imax;

I(Out) <+ Iout;    
                   // Drive computed current to output node.
I(Out) <+ white_noise(n, "wpn") + flicker_noise(n*fc, 1, "fpn");

FF(Fout_osc) <+ Freq;

end
endmodule

Thank you Geoffrey, I think your definition is exactly to the point, because freq jumps to 9GHz after 0, which is the frequency that I'm designing for.

I put just a resistor to the ground to see the effect and another strange thing is the current changes proportional to that resistance. When I put capacitors, it complains and give blowup error.

Is there a solution to this problem? How can I avoid this big jump and define the initial condition correctly?

Emre

You also probably want to change your Frequency nature. The absolute tolerance is too small. It should be around 10^-6 of the maximum you expect to see, so in this case it should be around 1K. And your blow up could be much larger, at least 1K times the maximum you expect, so in this case 1T.

-Ken

Try clipping the output rather than the input. And do you really want that transition function in there? Do you expect Iout to be piecewise constant?

-Ken

It would help if you posted the model and the error message.

-Ken

There are a couple of things to try. First, you might want to try giving ddt a tolerance. If that does not work, try making Freq a node rather than a variable (declare it as freq_current rather than real).

Concerning the output current looking like a voltage .... In fact it is a voltage. This is the result of a blunder made by the committee defining the language. When declaring a discipline, you cannot have a flow unless you also have a potential (that is the blunder, in the original version of the language this was possible, the unfortunate restriction was added by the committee). Thus, if you have a signal flow current, the current is not a flow but a potential. This causes trouble when connecting this terminal to anything electrical, like a resistor. Ideally the simulator should inform you that your disciplines are not compatible, but apparently it does not. It just gives you the wrong answer because the current is being treated as if it is a potential.

Given this situation, you should use "electrical" rather than "current".

-Ken

Thank you both for your suggestions.

Giving tolerance didn't help, but Ken's suggestion on defining Freq as a node was a very clever solution and it solved the main problem. I didn't get any more complains about dynmic quantities' access to output by giving freq directly to the output. At same time, I used freq internally for the rest of calculations and I could use any function, as Freq is a node.

For clipping, I used the style that Geoffrey suggested and it works the best. The only problem is initial value of I(out) is always Imin, because result of ddt() is 0 in the begining. But this time, my feedback loop can recover.

If there is any other way to get rid of that initial zero, which is not the "real" value, it's always welcome. I didn't understand, how transition function can be used for that purpose effectively.

Using electrical also solved the other problem, but this time when I connected a capacitor in series with the resistor, to realize the filter, the simulator had problems in finding the dc operating point, as there is no dc path to the ground. I connected a resistance to ground to solve the problem, but I didn't like this solution, because it alters the voltage at that node and additon to the filter. If there is a more sophisticated solution that you can come up, I would like to hear it.

Emre

You could always tell the simulator to skip the dc solution phase of its transient analysis.

-Ken