If you use IC5141 you can avoid having to use spp to preprocess the data. If you use "spectre +csfe input.ckt" it will parse the SPICE syntax netlist natively. If you use the later MMSIM60 release of spectre, then the new front end (which is what +csfe enables) is on by default.
To do what Ken says, you'd then put this in your netlist:
Code:simulator lang=spectre
save node1 node2 node3
simulator lang=spice
The simulator lang= is needed if the file is not in spectre syntax, or if the file does not have a .scs suffix (.scs implies spectre language mode).
As for the wavescan question, then if you are using wavescan standalone, you have two choices:
1. You can use Settings->Select Data in the results browser window. This will allow you to specify the start and end points as the data is read in (in other words it doesn't even read the data outside these ranges, saving memory). The same menu can be used with swept data to pick the parameter sweep values you want to read.
2. Perhaps a more likely way - use the "trim" function in the calculator.
If you're using wavescan in ADE (in IC5141 or later), then the calculator functions are then not using spectreMDL, but SKILL, and so the calculator function would be "clip". Rather confusingly wavescan standalone has a function "clip" which does clipping in the Y direction (a more sensible name, really).
Regards,
Andrew.