cannot set relative harmonic as a variable

Kevin,

Please read the Guidelines for the Custom IC Design Forum - knowing which version you're using is important - and you also didn't mention which analysis you're running. From a quick test, I found that this works fine with hbnoise, but not with pnoise (in IC6.1.8/ICADVM20.1 ISR29) so my assumption is that you must be talking about pnoise?

There's an existing (recent) change request, CCR 2705778 asking for this, so I would suggest you contact customer support and request a duplicate be filed on your behalf.

As a workaround, if your variable is called "N", then use the Options form on the pnoise Choosing Analyses form, go to the end and in the additionalParams field enter:

relharmnum=N

You can leave the relative harmonic on the main form as 1 (say). What will happen is that it will netlist the relharmnum parameter twice on the pnoise analysis, but because the definition coming from the additionalParams field is netlisted last on the line, that will win. I've tested this, and it works.

Regards,

Andrew

Thanks Andrew, I'll keep in mind on the guidelines

The solution works great in running the simulations, however, there is another challenging now in the plotting. After the sim is done, I pick one case and in the "direct plot form", add "Phase noise" to output, and the problem is that it uses the specific number (as it should ) instead of variable on the output expression for PN, i.e. number 3 in below should varies based on the variable N..

phaseNoise(3 "pss_fd" ?result "pnoiseOut1_pm")

I then manually replaced number 3 in the expression with variable (N or VAR("N")), it doesn't work for cases other than the one where it actually applies

do you have suggestions?

thanks,

Kevin

Kevin,

Rather than using the (sort of) obsolete phaseNoise function (although that should be OK if you're using the "pm" noise output), I'd suggest using:

pn('pnoise)

This knows which relative harmonic was used, and it's what the direct plot form uses.

Oh, hang on. Are you using the "multiple pnoise" checkbox? If so, it then reverts to using the phaseNoise function because it needs to pick the specific output database. That (unfortunately) doesn't seem to work with VAR("N") being used, unfortunately. I'm not entirely sure why (I don't have time to investigate before Christmas) - perhaps you could contact customer support about that. Or not use "multiple pnoise" and use the pn() function instead?

Andrew.

I ended up defining a bunch of PN1 PN2 PN3 .. for different harmonics where I put real number in the phaseNoise() . and only look at corresponding PN_x for specific N. It's not elegant, but seems working

thanks,

Kevin