Stats

  • Locked Locked
  • Replies 6
  • Subscribers 129
  • Views 4757
  • 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

QRC: how to avoid empty .SUBCKT (re-)definitions in the extracted netlist?

dontpanic

Hi! I am getting simulation errors when trying to use the extracted netlists produced by QRC, because they contain redundant (and empty) definitions for some components. For instance, in a minimalistic cell with a MOM cap I get in the extracted netlist the following definition:

[...]
.SUBCKT cfmom_2t_p80 PLUS MINUS
.ENDS
[...]

As a result, spectre complains when trying to use the extracted netlist view in a testbench:

ERROR (SFE-3263): "path/to/extracted/netlist/cellview/spice.spc": The subckt 'cfmom_2t_p80' is being redefined. Previously, it was defined in line XYZ of `/path/to/pdk/model/card.scs'. Remove or rename either definition.

How can I prevent these empty definitions from being included in the extracted netlists? If I edit the netlist and comment them the simulation proceeds and the results seem to make sense (i.e. the explicit (intended) MOM cap is instantiated along with the extracted parasitics; notice I don't want the MOM cap to be flattened--I want it to be recognized and instantiated so as to use its pdk model).

Thanks and regards, Jorge.

Parents
  • Saloni Chhabra

    Hi Jorge,

    You need an additional argument in your extraction command file.

    output_db -suppress_empty_subckts true

    Regards,

    Saloni

  • dontpanic
    in reply to Saloni Chhabra

    Thanks for your reply, Saloni. I tried using a command file with the contents:

    output_db -type extracted_view -suppress_empty_subckts true

    and running and "extracted view" extraction but the spice netlist (the extview.tmp file under the svdb directory) still includes the empty subcircuit definition. If I use a file with these contents:

    output_db -type spice -suppress_empty_subckts true

    then the produced netlist doesn't include the empty subcircuits, but then I'd need to run QRC 2 times to also get also an extracted view. Do you think it would be possible to get the empty subcircuit suppression in the extview.tmp netlist when doing "extracted view"  extractions?

  • Saloni Chhabra
    in reply to dontpanic

    Hi Jorge,

    I don't understand how you are running the flow..

    What output format are you generating from QRC - spice or extracted view? If it's extracted view, then 'supress_empty_subckt' isn't a supported argument. What are you doing with extview.tmp? It is an intermediate file generated by QRC and isn't intended to be used by the user directly for simulations. extracted view should be specified in the config view (hierarchy editor) for the DUT, and then Spectre will netlist it.

    If you are importing a spice netlist into Virtuoso (using spiceText view), then you will have to generate a spice output from QRC which should allow you to suppress empty subckts.

    Regards,

    Saloni

  • dontpanic
    in reply to Saloni Chhabra

    I am following the article "How to output both an av_extracted view and SPICE netlist in a single Quantus QRC run?". I am trying to debug extracted-view-generation issues in our 16nm flow, so, in this particular case, it would be really useful to have both the netlist and the extracted view generated in a single run. We are trying to migrate from Calibre xRC to QRC, but the generation of correct extracted views is so far probing very challenging.

    Thanks and regards, Jorge.

  • Saloni Chhabra
    in reply to dontpanic

    Okay, apparently, you've bumped into a situation where spice output format and extview.tmp cannot be made equivalent, so you'll have to comment the subckt's if you wish to use extview.tmp.

    Also, I'd suggest you contact Cadence customer support for getting some dedicated support on extracted view generation issues.

    Thanks,

    Saloni

Reply
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.