Stats

  • Replies 4
  • Subscribers 132
  • Views 654
  • Members are here 0

Maestro - tran mdl autostop feature is failing

firebolt4

I am trying to stop transient simulation when signal goes high (for now generated from vpwl for test purpose). Followed steps from this support link. Somehow it is failing without printing proper error. Please help. Thanks.

Support: How to use autostop feature in ADE/OCEAN to stop spectre once the given measurements are computed?
URL: support.cadence.com/.../ArticleAttachmentPortal


alias measurement tran_autostop
{
export real rise
run tran
rise=risetime(sig=V(reset), initval=0, inittype='y, finalval=1, finaltype='y, theta1=10, theta2=90)
}
run tran_autostop


ERROR (ASSEMBLER-5011): While simulating run Interactive.2, point 1, test amp_test, received error:
Simulation Error:
Simulator failed to complete the simulation.
The simulator integration (OASIS) has reported an unsuccessful simulation.
While this validity check is dependent on the particular simulator's OASIS integration,
with the default Cadence-provided checks common causes for this failure are:
1. Missing simulation /psf directory containing simulation output files.
2. Simulation output files (e.g., PSF) that do not contain any successful analyses.
Check the simulator's output log for more information.
./runSimulation can be manually run in this directory to check the issue.
For details open log: /<path>/maestro_top/results/maestro/Interactive.2/1/amp_test/psf/spectre.out for the point: (20 1)
For more details, consult the job log file:
/<path>/cds/logs_user/logs0/Job11.log

virtuoso version 6.1.7

Parents
  • JankoK

    Yeah, it's a weird error... did you enable MDL Mode? Perhaps your condition is never met or it is met instantaneously when you lunch the simulation... Try making something simulator friendly, with a gradual ramp... 

    By the way, that example that you referenced is not my favourite... You have another one in the article below, it is more intuitive. This article also explains the other two methods for stopping the simulation.

    Methods to stop transient simulation based on signal value/condition

    Hope this helps!

    /Janko

  • firebolt4
    in reply to JankoK

    Thank you for suggestions. All three methods are not working. I am using ADE GUI.

    1. VerilogA - extraction failed due to error at line  if($cds_analog_is_valid(netName)) begin

    2. MDL - Sim Error without any info

    3. Measure - Not reading file in netlist, hence not stopping sim. 

  • JankoK
    in reply to firebolt4

    I am travelling at the moment so I cannot test it myself. There is a high chance that someone would figure by now that those solutions do not work and report them. You can write a feedback (button at the right side) and inform the author. 

    I just noticed that you are using 6.1.7 (that's like 10 years old now), probably your Spectre version is also very old. Try updating both!

    BR

    /Janko   

  • firebolt4
    in reply to JankoK

    Updated cadence version. I am able to use veriloga & measure statement. But somehow mdl is failing, not sure why. Thanks for suggestions.


    Measure file should be file.scs, not .sp. Otherwise tool fails to read it's path.

    Included it in Test > Simulation Files > Definition Files.

    Also added switch autstop=yes in Transient Options > Misc > additionalParams.

    Sim stopped when vin=0.5V

    //
    simulator lang=spice
    .measure tran cond_stop WHEN V(vin) = 0.5

Reply
  • firebolt4
    in reply to JankoK

    Updated cadence version. I am able to use veriloga & measure statement. But somehow mdl is failing, not sure why. Thanks for suggestions.


    Measure file should be file.scs, not .sp. Otherwise tool fails to read it's path.

    Included it in Test > Simulation Files > Definition Files.

    Also added switch autstop=yes in Transient Options > Misc > additionalParams.

    Sim stopped when vin=0.5V

    //
    simulator lang=spice
    .measure tran cond_stop WHEN V(vin) = 0.5

Children
No Data

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.