Stats

  • Replies 3
  • Subscribers 130
  • Views 539
  • Members are here 0

Exceeded the blowup limit when running Monte Carlo analysis

aalbason

Hello there,

 

I am running MC analysis and I get this error due to an NPORT component which has the RLC files for a PCB output transmission line parameter model.

 

Error found by spectre at time = 14.0551 ns during transient analysis `tran', during Monte Carlo analysis `mc1'.

    ERROR (SPECTRE-16384): Signal V(NPORT0:int_Rn1) = -1.00013 GV has exceeded the blowup limit for the quantity `V' which is (1 GV). It is likely that the circuit is unstable. If you really want signals this large, set the `blowup' parameter of this quantity to a larger value.

 

To try to work around this since I cannot change the model file, I tried to have a larger blowup quantity and I used the script:

 

VoltQuant quantity name="V" blowup=10e9

 

Which I added to the maestro view under Setup → Simulation Files → Definition Files

 

Then I get an error when I run it again:

 

Error found by spectre during hierarchy flattening.

    ERROR (SFE-1997): "/home/team_proj/workareas/EIC2_LNR28LPP/al.albason/Quantity_Include_Statement.txt" 1: Cannot run the simulation, because VoltQuant in parameter `dc': Unknown parameter `V' has been specified in expression `V' Correct the expression and rerun the simulation.

 

Any advice? Hopefully it is just a minor error on the script used.

 

Thanks,

Alfonso

  • Andrew Beckett

    Alfonso,

    First of all, can you try setting the nport to have method=bbspice ? I don't know which version of Spectre you're using, but this might help ensure that it's a passive model being used. We also have the s-parameter checker (more details on our support site, but in recent IC versions this is available in the Tools menu in the CIW) to check for issues with the s-parameter file (of course, the garbage-in, garbage-out principle holds here...)

    In general, increasing the blowup limit is not that likely to fix things - if it's really got that large it may well just hit your even higher limit. 

    Anyway, I suspect this is a spectre syntax vs spice syntax thing. I'd start by giving your definition file a ".scs" suffix which will mean it's treated as Spectre syntax (the alternative is to put simulator lang=spectre before the quantity line, but the .scs suffix means the file is treated as Spectre syntax by default; .txt will be treated as SPICE).

    Andrew

  • LE202511197417

    The error seems to be due to the V parameter not matching the node name. Check the exact signal name in the NPORT component and update VoltQuant accordingly.

  • aalbason
    in reply to Andrew Beckett

    Hi Andrew,

    I use MMSIM23.10.802 for the Spectre version.

    I still have the nport Interpolation method as linear but as you suspected correctly it is a Spectre syntax error. 
    I renamed the file to ".scs" and the latter error pertaining to the Unknown parameter "V" went away. 

    I will try changing the Interpolation method to bbspice next to see if that also fixes my issue. This is probably the correct method instead of just working around the issue of increasing the blowup quantity.

    Thanks,

    Alfonso

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.