i am trying to write a veriloga code for some ac analysis.  i need the keyword for frequency, similarily like $abstime is the keyword for timefor transient analysis.  i looked everywhere, cannot find it.
anyone out there knowing the answer?

thanks,
zoltan

thanks.  i tried all the trivial options with  no success.  

how can i then create a frequency dependent voltage in veriloga for ac simulations?  i´d like to generate a mask for different applications (filters, jitter transfer, jitter tolerance, e.t.c.)   i remember, it was possible for hspice.  it had some pwl voltage source against the frequency.  it´s hard to beleive that there is something that hspice could and veriloga couldn´t handle.

thanks, again

zoltan manyoki

Zoltan,

Now we get to the root problem, which is solvable. I believe you want to do a frequency domain analysis, perhaps a filter or power spectral density analysis, and then overlay a spectral mask to quickly reveal the problem areas. I have had to do this many times myself.

I assume you are using Spectre. I introduce the mask with a Spectre primitive pwl noise source that is not connected to the system in any way. You should be able to introduce the primitive structurally in VerilogA if not explicitly in the top level schematic. You could also use a VerilogA noise table. If you use VerilogA, you will need an additional output port. The noise source simply makes the mask available to the waveform display tool. The mask probably only has a few key points. Enter the frequency versus volts**2 pairs into the noise field for a dc source. Then perform a noise analysis only on the frequencies you entered. If you perform the noise analysis on other frequencies too, the plot will look strange on logarithmic scales because the source linearly interpolates on linear scales, not logarithmic scales. The waveform display tool linearly interpolates on the scales being displayed. Once you have the noise analysis, you can overlay the noise psd with your psd or transfer function of interest.  Be sure you use consistent units and scales. If you do not want to clutter up your circuit with auxiliary sources, or you already have a noise analysis set up, you can use a separate schematic for the mask source and then merge the plots with the waveform calculator. If your spectral mask is a relative requirement, you will need to scale the spectral mask to the spectrum in question. You can easily do that with the waveform calculator.

You're welcome.  

When I have a circuit that takes a while to simulate, I put the noise source in it's own schematic. Run time is not even noticeable then. I use the waveform calculator to overlay the analysis from the noise schematic and the schematic under test.

I think there's a way you can save the nosie waveform and recall it later, which would save even more time.

-Jess