Is it possible to introduce non-deterministic noise in HSPICE transient simulations?
Is there any way to generate a PSD? (also HSPICE transient sim)

Thanks,
Robert

I am currently using HSPICE version Y2006.03.
I did find some verilog-A examples in my HSPICE directory, although I've never used this feature.

HSPICE doesn't have transient noise abilities.
In the past I used PERL script adding noise sourses in parallel (or in series) with the circuit elements. They were PWL gotten from Matlab, per source, of course. It was a nightmare... But worked.

Recently I was told about HSPICE-RF. You have to check what it knows to do.

You have to increase the accuracy of your simulation.
Use .option accurate = 1 together with reltol=1e-9 (at most). Try a number of simulations also with reltol of 1e-10, 1e-11 and 1e-12. In this case you will find the trade-off between accuracy and simulation time.

I tried the suggestions of increasing the reltol accuracy to 1e-15 even, but that did not help at all.

So then I contacted Synopsis about this problem, and after a week of research, they finally discovered the source of the problem stemmed from using their Avan-waves viewing tool.  According to Synopsis support, this tool is the freebie viewer that comes with every HSPICE license, and was actually a development project back in the 80s, based on single precision, and therefore will never be updated.  Instead I have to purchase a COSMOS scope license which is another $10k.  My manager is not going for that.

Unfortunately I don't have access to Spectre.  We are a small company, and cannot justify spending the amount of money required for such a tool.  Although, it seems that to get everything we need would cost just about the same after adding in the costs for all the different options.  It would be nice if we could though.

Imtired et al,
                   there is a simpler, more direct way to do transient noise sims: use a pwlfile controlled source in spectre, or a pwl file with a list of time, voltage pairs which may take either random time or voltage values, or random values for both.  I use excel to write these values to a text file for editing in a wordpad for inclusion in the simulation netlist as part of an independent source's pwl definition.

As already mentioned, reltol, vntol etc need to be set correctly to enable the noise contribution to the circuit is above the simulator limits - also, these values can be used constructively to truncate the noise to speed up simulation runs.  For some simulation runs you will find it is more efficient to inject noise using the Thevenin equivalent current as this may make the noise injection to signal ratio smaller, easing the reltol, pivtol etc settings.

In terms of analyzing the results: you can use FFTs to find the PSD but these tend to be processor intensive functions - if you can translate the PSD into an equivalent jitter spec, than you can use eye-diagrams to analyze the data much more efficiently: you can then use "measure" or (a crossing point detector) to build a historgram of the circuits' behaviour.

Even in "noddy-spice" this technique works.  If you don't have an "eye function" you can use:

sweep* (atan(tan(PI(TIME/sweep * delay/sweep - 0.5))))/PI +0.5)

where "TIME" is SPICE's internal time variable, "sweep" is the time across which the waveform repeats, "delay" is the  initial delay  time before the waveform becomes repetitive, and PI is 3.1415926... as usual and for some versions of SPICE will need to be declared as a variable in the .PARAM line.

With a little thought you will find that you don't have to use specialized mixed-mode simulators to do noise analysis in transient sims, simple versions of spice are also capable of doing this.

Cheers,
           SimonH.