Stats

  • Locked Locked
  • Replies 5
  • Subscribers 124
  • Views 5198
  • 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

How can you create a global net in a Spectre netlist that does not end in !

FormerMember
FormerMember
The model library I have from the foundry has a global signal in the components called PSUB. The foundry says to create a global net PSUB at the begining of the netlist and connect it to ground. The only way to create a global in virtuoso seems to be to give it the ! postscript. When I do this, the names don't match and I still have floating nodes. Is there some way to resolve this besides modifying the whole model library?

  • You could set this up in a stimulus file as:

     global PSUB

    vPSUB (PSUB 0) vsource dc=0

    and then include that file in the Stimulus Files section in the Setup-> Simulation Files... form in ADE.

  • FormerMember
    FormerMember

    I tried this but the simulator gets an error that I think is caused by the fact that I have not been able to stop it from automatically generating a statement:

     global 0

    So, when I try to include the file with the extra global statement there is an error because you can only have one global statement. I think this would work if I could get it to stop generating the global 0 statement.

     Thanks for your help. 

  • This has not been the case for a good 10 years now, so you must be using an ancient version of spectre. If you're getting this error:

     Error found by spectre during circuit read-in.
        "forum.scs" 11: There can be at most one global statement and, if present,
            it must be the first command in the file (after title or language
            directive).

    Then it suggests that you're probably using spectre from IC5141 rather than an MMSIM version. There have been MMSIM60,61,62,70,71,72,101,111,121,131 - i.e. 10 major releases of the simulators since then. 

    Even if you are using IC5141 spectre (which is not advisable) you can switch to the new spectre front end that was not enabled by default in IC5141 by adding +csfe to the "userCmdLineOption" field in Setup->Environment in ADE. This new front end became standard in MMSIM60 (which was released in late 2004), so using an MMSIM version makes most sense.

    If the error you are getting is something else, please state what the error is.

    That said, I've just noticed that the "spectre -h global" documentation still says you can only have one global statement, which is definitely not true (I remember this being fixed, and I've tested it). I'll file a CCR to get the documentaton fixed.

    Regards,

    Andrew.

  • FormerMember
    FormerMember

    Yes the solution above did work. The error I was seeing was related to an earlier attemp I had made to fix the problem that didn't work. I thought I had removed that try, but it was still in the simulation options. When I looked at the netlist and read in the manual that you could only have one global, I assumed that this was the problem.

    Anyway, problem solved.

    Thanks for the help. 

     

  • I gave existing CCR  1075278 a prod to get this corrected.

    Regards,

    Andrew.

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.