I have used rmsNoise command to calculate the total integrated rms noise over the desired band. But recently I am seeing wierd behaviour with this command and it throws me error:
*Error* rms Noise data not available
simulator lang=spectre global 0 include "....../ahdlLib/quantity.spectre" C0 (VOUT VSS) capacitor c=1p R0 (VOUT VSS) resistor r=1M R1 (VOUT VDD) resistor r=1M V4 (VSS 0) vsource dc=0 type=dc V1 (VDD 0) vsource dc=1 type=dc noise (VOUT VSS) noise start=1 stop=1M
The ocean commands:
openResults("psf") selectResults("noise-noise") rmsnoise.sch = rmsNoise( 1 100K )
I am able to use noiseSummary('integrated) successfully.
Any idea what's going wrong.
The rmsNoise() function expects the "runObjFile" to be present, which won't be the case if the simulation was run standalone.
I don't see an enormously good reason for this. In fact even if you use wavescan/viva standalone on the data, it doesn't work - this is because it uses the ADE "VN2" function to retrieve the noise output.
When you did the openResults, you'll have seen a message such as this:
WARNING (OCN-6096): Could not find runObjFile under .../psf. Calculator data access functions will not work.
and this is the reason why. The good news is that this is fixed in IC615 (I just tested it).
As a workaround, you could use:
procedure(CCSrmsNoise(from to @key result) sqrt(integ(clip(getData("out" ?result result) from to)**2)))
In reply to Andrew Beckett: