Stats

  • Locked Locked
  • Replies 5
  • Subscribers 125
  • Views 2171
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

MMSIM 6.2 - Spectre question

yoyega

Hi,
I am 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.saveall.PHC.scs and  netlistTRAN022.1x1.saveselected.PHC.scs. The only difference between these files is the following options statement:

(in netlistTRAN022.1x1.saveall.PHC.scs)
saveOptions options save=all pwr=all currents=all useprobes=yes

(in netlistTRAN022.1x1.saveselected.PHC.scs)
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?

 Thanks,

Pedro

  • 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).

    Regards,

    Andrew.

  • 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...

     Thanks,

    Pedro

  • You may need to switch the output format from the default SST2 to PSF to see performance improvement on the 'spectre results reader' side of things. I had to write a special Makefile-driven extraction procedure for one of our designers to get around this problem using 'simvisdbutil' from the IUS tools. Another thing to try (if all you're interested in is viewing, not post-processing the results) is to open the results in simvision. That's where the SST2 format originated so it tends to read those results in more efficiently. Andrew.

  • See sourcelink solution 11264780

    If using IC5141, then you'll need to do:

    setenv PSF_WRITE_CHUNK_MODE_ON true

    Regards,

    Andrew.

  •  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...

     

    Regars,

    Pedro

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.