I'm simulating a VCO at the moment and I want to create a plot which shows
PhaseNoise@100kHz vs. tuning voltage of the VCO. However I'm having trouble
in getting the plot.The simulation is a PSS simulation with PNOISE that uses
a symbolic parameter that tracks with vdd to ensure that vtune does not exceed
the supply voltage. This range is then divided into 30 intervals to simulate PhaseNoise
at different VCO frequencies.
I get the various PhaseNoise plots but if I apply a value measurment @ 100kHz
to the waveforms I only get a single waveform measured.
The generated measurement within the calculator looks like this:
value(value(_drplPmNoise(?modifier "dBc") "vtune" 0.0) 100k)
which indicates that only the waveform with a tuning voltage of 0.0 is considered.
I have extended the list to include more voltages and it works but this approach
has some negative side effects if I change to supply voltage and therefore also the
voltage tuning range of the VCO. As the intervall is tracking with vdd I get different
voltages each time I change the settings for the supply :(
Is there an easy way to tell ADE that I just want a value measurement for all available
graphs without having to specify tons of voltage values ?
That's odd. I don't know how you did the sweep (or which version you were using), but normally the inner sweep should be the frequency sweep of the pnoise analysis, and the outer sweep would have been whatever you set up as the sweep on the PSS analysis form (assuming that's what you did - you really didn't describe the sweep setup) or using Tools->Parametric analysis in ADE.
So it ought to work using
value(_drplPmNoise(?modifier "dBc") 100k)
To remove any ambiguity about which variable you wish to slice though in the value function, you should be able to do:
value(_drplPmNoise(?modifier "dBc") 'freq 100k)
(From the expression I'm assuming you've set up to use "modulated" or "jitter" mode (in FM mode) on the pnoise form).