• Skip to main content
  • Skip to search
  • Skip to footer
Cadence Home
  • This search text may be transcribed, used, stored, or accessed by our third-party service providers per our Cookie Policy and Privacy Policy.

  1. Community Forums
  2. Custom IC Design
  3. spectre simulation in batch mode with an include spectre...

Stats

  • Locked Locked
  • Replies 2
  • Subscribers 124
  • Views 18982
  • 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

spectre simulation in batch mode with an include spectre-netlist into an input.scs file

samung
samung over 9 years ago

Hello,

I am generating a spectre-netlist file with an ocean batch commandline. This seems to work well.
Then, I try to include this file into an input.scs which gathers models, stimuli, analysis options, measures and ... an include line to this spectre-netlist file.
I have managed in making a spectre simulation of this input.scs, including the content of the spectre-netlist file.

However, my goal is to point to this spectre-netlist file, with something like: include <pathToTheFile>, into the input.scs

Is that possible ? What would be the syntaxe ?

  • input.scs content extract:

** parameters section
simulator lang=spectre
parameters I0=10000e-06
parameters nbcols=32
parameters vdd=10

** models section
simulator lang=spectre
* variables
parameters param1=1
parameters param2=0
* models
include "/home/.../model_corners.scs"
include "/home/model2_corners.scs" section=TC_TR


** netlist section
simulator lang=spectre
include "/home/.../cell.schematic.spectre.netlist"
...

  • cell.schematic.spectre.netlist extract:

subckt bc1m1t_lvt_sh bl sl vpw wl
parameters w1=0.12u
Mnsel (vd wl sl vpw) nlvtlp w=wsel*10e5 l=0.04 nfing=1 mult=1 srcefirst=1 \
mismatch=1 lpe=0 numcos=1 numcod=1 ngcon=1
Im (vd bl state) _mt radius=20e-08 initstate=0 nsmis=0 \
opMode=3
ends bc1m1t_lvt_sh

R1\<0\> (sli\<0\> gslo\<0\>) rm1 w=0.29 l=0.07
R3\<0\> (sli\<0\> lslo\<0\>) rm1 w=0.11 l=0.07
...
Ibc1614 (bli\<14\> sli\<0\> vss wli\<16\>) bc1m1t_lvt_sh wsel=0.30u
...

  • spectre.log:

Error found by spectre during circuit read-in.
ERROR (SFE-1802): "/home/.../cell.schematic.spectre.netlist" 5: Spectre "subckt" statements are not supported in spice language sections. Use "simulator lang = spectre" to introduce Spectre language sections.
ERROR (SFE-1802): "/home/.../cell.schematic.spectre.netlist" 6: Spectre "parameters" statements are not supported in spice language sections. Use "simulator lang = spectre" to introduce Spectre language sections.
...
ERROR (SFE-1025): "/home/.../cell.schematic.spectre.netlist" 118: Instance `Ibc1614': Unexpected value `wli<16>' - all required positional parameters have already been specified.

  • spectre cmdline:

spectre /home/.../input.scs +log /home/.../spectre.log

  • ocean cmdline:

ocean -nograph < /home/.../genNetlist.ocn > /home/.../ocean.log

  • genNetlist.ocn:

load(".cdsinit")
envSetVal("asimenv.startup" "projectDir" `string "/home/...")
simulator('spectre)
design("<library>" "cell" "schematic")
createNetlist(?recreateAll t ?display nil)
exit()

  • ocean .log:

WARNING (ADE-6001): The number of terminals specified in CDF termOrder are more
than the actual number of terminals in the cellview cell-view "cmos040lp_memprimitive" "bc1m1t_lvt_sh" "schematic"
WARNING (ADE-6004): Mismatch was found between the terminals in the cellView and those on the
termOrder property on the CDF. Because of the mismatch, the CDF termOrder will
be ignored. The terminals in the cellView will be netlisted in the alphabetical
order of their names. Eliminate the mismatch if you want the CDF termOrder
property to be used for netlisting.

...

Errors: 0 Warnings: 2
...successful.
compose simulator input file...
Loading devCheck.cxt
...successful.

As said above, if I copy paste the content of the spectre-netlist file into the input.scs, the spectre simulation ends successfully !!

Many thanks for your help,

P.

  • Cancel
Parents
  • Andrew Beckett
    Andrew Beckett over 9 years ago

    This is simple to resolve. Spectre makes the assumption that if a file ends in the suffix ".scs" it is in spectre syntax, otherwise it's in SPICE syntax. So your file with the suffix ".netlist"  (cell.schematic.spectre.netlist) is treated as SPICE syntax when it's actually spectre syntax.

    There are two alternatives:

    1. Rename the file to be cell.schematic.spectre.netlist.scs 
    2. Add the line "simulator lang=spectre" at the top of the cell.schematic.spectre.netlist file to change the language mode

    Regards,

    Andrew

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
Reply
  • Andrew Beckett
    Andrew Beckett over 9 years ago

    This is simple to resolve. Spectre makes the assumption that if a file ends in the suffix ".scs" it is in spectre syntax, otherwise it's in SPICE syntax. So your file with the suffix ".netlist"  (cell.schematic.spectre.netlist) is treated as SPICE syntax when it's actually spectre syntax.

    There are two alternatives:

    1. Rename the file to be cell.schematic.spectre.netlist.scs 
    2. Add the line "simulator lang=spectre" at the top of the cell.schematic.spectre.netlist file to change the language mode

    Regards,

    Andrew

    • Cancel
    • Vote Up 0 Vote Down
    • Cancel
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.

© 2025 Cadence Design Systems, Inc. All Rights Reserved.

  • Terms of Use
  • Privacy
  • Cookie Policy
  • US Trademarks
  • Do Not Sell or Share My Personal Information