Plot noise voltages for more than one node

Fundamentally, the noise analysis only supports a single output. This is because the noise analysis has to compute the transfer function from each noise source to the output, and multiply that by the amount of noise in each noise source, and then sum up the output noise powers. To measure the noise at a different node means to do all that work again for a different transfer function.

So spectre itself can do it by having more than one noise analysis in the netlist. 

ADE (in general) doesn't support multiple analyses of the same type - although in some special cases this has been implemented. For example, pnoise and hbnoise support multiple noise analyses, because the cost (time, memory etc) of the preceding pss or hb analysis is quite high, and so you want to be able to share that preceding run for efficiency. For noise analysis, that's less of an issue (although it can be in the case of a circuit with a slow DC operating point).

The workarounds are either to set up multiple tests in ADE XL or Assembler, or you could create a file (analyses.scs - have a .scs suffix) with (say):

noise1 (out1 0) noise start=1 stop=1G
noise2 (out2 0) noise start=1 stop=1G

and then reference this from the Setup->Model Library. I'd suggest stealing the lines from the input.scs from your normal noise setup, and just changing the analysis instance name (the first word) to make them unique. You can mix this with other analyses performed through the ADE UI.

You'd then have to adapt your output access functions in ADE to reference the correct analysis instance name, but it's not too tricky to do this.

There are enhancement requests to get ADE to support multiple analyses of the same type in general, but it needs a reasonable amount of work to ensure that both the analysis setup and the result processing (Direct Plot, calculator etc) all allow  you to easily identify which analysis results you want to retrieve. So it's not happened yet...

Regards,

Andrew.