Stats

  • Locked Locked
  • Replies 4
  • Subscribers 125
  • Views 7143
  • 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

ADE Assembler: Get no evaluation for DC sensitivity analysis

StephanWeber

Hi,

I made an Assembler test settup, which include a sens analysis (for dcOP and dc). I define outputs (like not voltage at net Out) and to which elements I need the sensitivity (like V1). I can run this, and using the Results Browser I can get all results (like send to Table or Plot).

However, I I do send to Calculator, it does not work anymore, also sending this to ADE output setup.

I wonder what is going wrong:

Here is setup:

Sim:

dcOp dc write="spectre.dc" save=allpub maxiters=150 maxsteps=10000 \
    annotate=status
dcOpInfo info what=oppoint where=rawfile
dc dc param=Iin start=0 stop=2 lin=20 values=[1m 5m 10m 20m] save=allpub \
    oppoint=rawfile maxiters=150 maxsteps=10000 annotate=status
sens (OutDM OutCM ) to (V1 V2 I22 V8 I13 ) for (dcOp dc )

Outputs:

getData("/sens1:OutCM,I13:dc" ?result "dcOpSens")

getData("/sens1:OutCM,I13:dc" ?result "dcSens")

I wonder about sens1, but also modifying it in the Calculator to sens does not help.

Error message example:

ERROR (VIVA-3002):expression evaluation failed: getData("/sens1:OutCM,I13:dc" ?result "dcOpSens")

ERROR (VIVA-3002):expression evaluation failed: Expression evaluates to nil

ERROR (VIVA-3002):expression evaluation failed: getData("/sens1:OutCM,I13:freq" ?result "dcSens")

Bye Stephan

  • StephanWeber

    Little addition:

    I have two dc analysis active this is the reason for getting sens1. However, removing one dc analysis does not help: I get now "sens" in Send to Calculator, but still it does not work, outside Results Browser.

  • StephanWeber
    in reply to StephanWeber

    I am using Virtuoso 20.1.500 isr31. I tried using the calculator directly, but e.g. geta data leads me only to a text window. This contains the sens analysis, but no further data.

  • Andrew Beckett
    in reply to StephanWeber

    Stephan,

    The issue is that it is mistakenly mapping the name back to a schematic name. Of course, there is no instance in the design called /sens1:OutCM,I13:dc and so it goes wrong.

    You can do two things:

    1. Omit the initial slash to use netlist names: getData("sens1:OutCM,I13:dc" ?result "dcSens")
    2. Use pv() instead - in that case it works with or without the initial slash: pv("/sens1" "OutCM,I13:dc" ?result "dcSens")

    Regards,

    Andrew

  • StephanWeber
    in reply to Andrew Beckett

    Thanks Andrew. I removed the / and it works fine now!

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.