I am doing a PSS+PNOISE simulation of a circuit in Spectre.
I need to multiply the output voltage of certain terminals with Complex Constant ( exp(j*pi/4)=0.707+0.707i).
This I don't want for post-processing ( which can be easily done using Ocean Script).
I want it on the fly of simulation.
Is there any ways of achieving this in VerilogA.
In general, this is impossible in the simulator. This is a constant phase shift of 45 degrees, and that would be non-causal in the time domain.
It could be done in frequency domain analyses only (e.g. ac and hb, including PSS in hb mode), but not by using Verilog-A. Verilog-A cannot be written in the frequency domain - you'd have to translate it into the time domain, and since there is no time domain representation of such behaviour (except maybe over a narrow band), it can't be done that way.
The way I would do this is to create an s-parameter file representing the complex transfer function, and then use nport with this. Be aware though that simulating it in time domain analyses would either fail or give bad answers, as it is not possible in real life. When creating the s-parameter file, you should make sure there is a dc point which doesn't have a complex transfer function (as that's not possible) to ensure the DC behaviour is correct and it can find an operating point.
There is an internal implementation of a phaseShift for SpectreRF use (in frequency domain analyses), but it's not really in a state that I'd want to post it on the forum.
Why can't you do this in the post-processing tool? That works fine - simply multiple your signal by complex(sqrt(2) sqrt(2)) in the calculator.
In the earlier post you have mtioned regarding phaseShift for SpectreRF.
Is it now in a state to be used by users like us in PAC & PNOISE analysis.
I'm not sure I'd want to post it on the forums - you should contact customer support since we would need to check if R&D are happy to release it to selected customers so that they can give us feedback on how appropriate it is in real life situations.
If you run an ac analysis on a system containing verilogA blocks and use the calculator to implement a multiplier function, is there any way to extract the dc component on the 'multiplier' output? In my example the multiplier inputs have no dc component but the multiplier output will have a dc component. I have simply done a real(VF("/in1")*VF("/in2")) and although I have a result, it does not look correct to me and am wondering about how to fully specify the complex nature of the signals in the calculation.
An AC analysis won't give you the DC component as it is a small-signal analysis and there's no DC component at all. It's doing a small-signal linearisation around the DC operating point, and so the complex values you are getting are representing the magnitude and phase of the signals.
You could get the DC component from the dcOp, but to be honest if you're really trying to implement a multiplier, you probably should be using a PSS or HB analysis (maybe with PAC/HBAC afterwards - not 100% sure what your objective is) as this will take into account the frequency translation and non-linear effects that cause the frequency translation.