Stats

  • Locked Locked
  • Replies 20
  • Subscribers 126
  • Views 24502
  • 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

Transient simulation taking too much memory

vshssvs7

Sir,

I have to run a transient simulation of a transistor-level Charge Pump PLL. I have noticed that it is taking too much memory. icfb got shutdown by itself with this message at the terminal:

ERROR: Unable to allocate memory for transition file slice variable transition index level (read).

The simulation was not complete and it shutdown in between. The size of tran.tran.trn is around 40 GB.

Note that I have already done this: In Analog Design Environment, Outputs -> Save All, I have checked "selected" option in "select signals to output (save)" and Outputs -> to be saved -> select on schematic and selected few nets that I wanted to save

But even after doing the above, it is still saving every net (because I'm able to plot those nets) which is the reason for such a huge tran.tran.trn file. What more should I do to stop it from saving every net? (and only save the nets that I select) 

 

  • Sorry sir, I posted that message before I saw your reply.

    I (re)started the simulation again yesterday itself with strobe period as 10n in transient analysis options to reduce the data. The simulation is going on currently. I'm not sure what I checked/unchecked in 'save device currents' line when the problem occured (first time simulation). But currently input.scs file is as follows:

    simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27.0 \

        tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \

        digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \

        dochecklimit=yes checklimitdest=psf 

    tranCheckLimit checklimit checkallasserts=yes severity=none

    tran tran stop=30u errpreset=moderate write="spectre.ic" \

        writefinal="spectre.fc" annotate=status save=selected strobeperiod=10n \

        maxiters=5 

    finalTimeOP info what=oppoint where=rawfile

    designParamVals info what=parameters where=rawfile

    primitives info what=primitives where=rawfile

    subckts info what=subckts  where=rawfile

    asserts info what=assert  where=rawfile

    save vctl 

    saveOptions options save=none pwr=none useprobes=no

    ahdl_include "/cad/tools/cadencetools/IC5141_USR6/tools/dfII/samples/artist/ahdlLib/vco/veriloga/veriloga.va" 

  • Here you have chosen the signals to be output as "none". You really don't want that, because that will save only a single (arbitrarily chosen) signal - it was a historical limitation in spectre that it was hard to turn off the outputs completely, so "none" just picks one at random to get the results small.

    You want "selected". 

    It should only be saving vctl then.

    Andrew.

  • Sir, even though it should save only 'vctl', I'm still able to plot other nets (Results -> Direct plot -> transient signal). Why is that so? (If it didn't save other nets, how is it able to plot them?) I hope you understood my doubt.

    Thanks. 

  • Could someone please reply to my doubt....Even though I want it to save only certain nets, spectre is saving every net clogging my hard disk. I cannot run a transistor level PLL with this problem.....please help.

  • Hi vshssvs7,

    Please note that Cadence AEs respond to questions on this forum often "off hours" and/or in addition to their "regular duties". 

    If this is a critical issue and you need immediate attention, please talk to your University staff and see how to file a Service Request at http://support.cadence.com . (There are specific instructions for university accounts). 

     I cannot reproduce what you are seeing in MMSIM 11.1 and IC 6.1.5 latest ISR. 

    If I only save one net. (save=selected) and

    1. Select Results->Direct Plot->Transient Signal and click on an unsaved net, I get a message in the CIW:

     *Warning* no "VT" data for node "/net8"

    2. If I do not have any signal in the outputs pane selected for plotting, then I cannot use Results->Plot  Outputs->Transient.

    If I only have one signal selected in the Outputs pane, then I can only plot that signal.

    3. Selct Results->Direct Plot->Main Form, I get an error in the Direct Plot form that says: 

    ERROR:  /net8 is not a kept output

     

    Best regards,

    Tawna

  • Respected Madam,

    Thanks for replying. What you mentioned is the "expected" behavior. That's what should happen, but it's not happening in my case. It's able to plot all the signals even though I save only one (or few) nets (which is the reason for huge disk space as it is saving all nets). My friend uses same version of cadence as mine and it works for him as "expected".

    Ok then, I will have to approach my university staff and file a service request.

    Thanks. 

  • Hi Vshssvs7,

    Precisely…I am seeing the expected behavior.  And you are not.  This indicates that there is a problem that needs to be

    investigated by a Cadence Support Application Engineer via a Service Request.  The Community Forum is not going

    to be an effective vehicle to resolve your issue.  My goal is to help you get “up and running” as quickly as possible.

    And that means filing a Service Request.  J

    Best regards,

    Tawna
  • One other thing to quickly check - do any of the files which are included via "include" statements at the top of the netlist contain either "save" statements (e.g. "save *") or options statements which have the save parameter.

    But in general, a service request is the best bet.

    Andrew

  • Thank you Andrew Sir, You did it!

    This is the solution I have been looking from beginning. 

    Long ago I included "cadence.scs" file (from Setup -> Model libraries) to be able to plot device parameters like gm, gds, etc. It has only a single line: save * sigtype=all

    This has caused all the problems. Now I have disabled it and everything is working as "expected".

    Thanks again :) 

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.