Stats

  • Locked Locked
  • Replies 5
  • Subscribers 126
  • Views 19178
  • 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

How to recover the stopped tran analysis from ADE

archive

Though the Spectre user guide provides method to restart the stopped transient simulation,  It is unclear to me how it is done  in Analog Design Environment (ADE). From the default  ckptclock = 1800 option it is clear that every half an hour the  state will be  saved. Where this  state file is  saved and with what name? How to  recover the analysis from ADE?? Is there possibility to  restart  a very long running simulation daily in the  night and stop in the  next morning for other work and resume the simulation before leaving again??

Thanks in advance for any help.


Originally posted in cdnusers.org by gunturikishore28
  • archive

    The file will be saved in the netlist directory (which is the directory that spectre is run from). You can recover from it by using the recover parameter in transient, or you can use the "Start from checkpoint file" on the Setup->Environment form.

    Better is to use the "saveperiod/saveclock/savetime/savefile" options which have been added in recent versions of spectre (I think MMSIM61 onwards, although it may have been MMSIM60). These save the full "state" of the simulation and so the recovery is much better. Effectively the old checkpoint mechanism doesn't store everything it needs to, and so you can end up with some startup troubles in some cases if you use that approach.

    Best Regards,

    Andrew.


    Originally posted in cdnusers.org by adbeckett
  • kene

    Whr is the documentation on this from within the ADE environment? I can't find it except for the command line. Is there an example somewhere? 

  • Andrew Beckett

    For example, if using MMSIM71, run "cdnshelp" to bring up the documentation system, and then search for "saveperiod" - the first hit is in the "Virtuoso Spectre Circuit Simulator User Guide" in a section called "Creating Saved State Files" - this describes it in some detail.

    If you're using an older version, you may need  to use cdsdoc, or you can look in <MMSIMinstDir>/doc/spectreuser/spectreuser.pdf

    Regards,

    Andrew.

  • HHashempour

    How does recovery option work in ADE-XL across >1 corners? How to specify location of the file for different corners? 

    Thanks for any hint!

    Hamidreza Hashempour

  • Andrew Beckett

    Hi Hamid,

    The simplest would be to use the Options->Save to re-use the same history, and set the save file to just be a local path (in which case it would be in the netlist directory for each corner). If you're re-using the same history, and using the recover option, it will pick up the state file from the same point it had on the previous run.

    That said, this is hard to scale for multiple runs, because recover doesn't append to the existing results waveform database; it starts afresh from the timepoint in the previous state file. So your measurements may not work properly...

    Getting this to all work properly and cleanly with ADE XL (or Explorer/Assembler) is far from trivial, and would require a fair bit of work from R&D to support. Even merging the results wouldn't be that straightforward, because the end point of the previous simulation may overlap with the start point of the new simulation.

    Regards,

    Andrew.

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.