using MMSIM 6.2 to run some Spectre simulations and I am having some
unexpected problems with the results. I am simulating files
netlistTRAN022.1x1.saveselected.PHC.scs. The only difference between
these files is the following options statement:
saveOptions options save=all pwr=all currents=all useprobes=yes
saveOptions options save=selected currents=selected useprobes=yes
but simulation results for the saved signals are completely different
depending on the scs file I run. As far as I understand, the above
options statements should not change the results of a simulation, only
the signals to be saved to HHDD, am I right?
Do you know which could be the problem?
If you take a look at the spectre output log file, in particular in the circuit inventory, you'll see a difference (I suspect) in the number of iprobes appearing in the circuit. This alters the size of the matrix being solved, and consequently it can affect the convergence. Normally the results may be very slightly different, but if bigger, it is normally indicative of the fact that you may have multiple stable operating points in your circuit (rather like hysterisis in a comparator, but it could be other things).
In the Simulation->Options->Analog you can enter "subcktiprobes=no" in the additional parameters field at the bottom of the form. If you do this it uses an alternative method for measuring currents (although I think if you set useprobes=yes it may stop this and still use iprobes). Is there a particular reason why you're using useprobes=yes? (it's normally only needed for currents in AC-type analyses).
Thank you very much Andrew, it looks like the problem was the useprobes option (I inhereted the script from another designer and, although I didn't need it, I thought that the useprobes option was harmless for my simulations...looks like I was wrong...again...:) ).
By the way, I have another problem. The circuit I am simulating is quite big, and if I use the save=all or save=allpub a file of 50GB is generated as the output of a tran analysis. If I select just a few signals of interest to be saved and use save=selected option the file is much smaller, but still measured in GB (about 7 - 8). The problem is that when I try to view the results with wavescan or ocean, sometimes, the application can not handle such big files. Do you know a way to overcame this problem?...maybe there is a way to separate the saved signals in several files instead of just only one...
See sourcelink solution 11264780
If using IC5141, then you'll need to do:
setenv PSF_WRITE_CHUNK_MODE_ON true
Thank you very much to both for your replies. I'm trying to consult sourlink solution 11264780 but it looks like I have a problem with my log in...I will try to solve it via cadence support...