You don't need to do a parametric analysis to do a sensitivity analysis.
Assuming you have a source called "vds" and "vgs" in your schematic, the following OCEAN script can be used:
Code:analysis('dc ?saveOppoint t )
;analysis('sens ?analyses_list list("dcOp") ?term list("/M0/S" "/M0/G" "/M0/B" "/M0/D") )
analysis('sens ?analyses_list list("dcOp") ?output_list list("M0:ids"))
desVar( "Vds" 1 )
desVar( "Vgs" 0.7 )
temp( 27 )
run()
Then afterwards, do:
Code:selectResults('dcOpSens)
vdsSens=pv("/sens1" "M0:ids,vds:dc")
vgsSens=pv("/sens1" "M0:ids,vgs:dc")
The ?output_list is referencing the ids parameter of the transistor you want to measure the sensitivity to. ADE always produces a sensitivity analysis to
all instance and model parameters (there's no way to be selective about it, unfortunately, despite the fact that this is supported in spectre). The results are presented in terms of pairs of output parameter to input parameter names - in this case I'm checking the sensitivity to the dc parameter on the two voltage sources.
Best Regards,
Andrew.