Stats

  • Locked Locked
  • Replies 4
  • Subscribers 143
  • Views 15121
  • 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

question about vsource used in Ocean

Carmichaeli

Hi all,

I had a problem when I did a simulation with Ocean Script. I designed a circuit by virtuoso and extracted the spectre netlist, then I remove some voltage source statements from the netlist and make a new stimulus file as input variables containing new vsource statements. By using vpulse in this way, I can get good result. But when vpwl was used, I always got error.

the vpulse statements are all like below and works well:

V0 (net6 0) vsource type=pulse dc=1.800000e+00 val0=0 val1=1.800000e+00 period=28n delay=14n rise=100p fall=100p width=14n

the vpwl statements are all like below:

V0 (net6 0) vsource type=pwl wave=\[ 0 0 100n 0 ]   (or  V0 (net6 0) vsource type=pwl wave=[ 0 0 100n 0 ])

I used these to the same circuit with just different input. It is weird that vpulse works well and vpwl can't work.

----the error message is:

ERROR (SFE-1025): "/homes/cadence/lab2/spi/tb_1.txt" 131:
        Instance `V0': Unexpected value `0' - all required positional
        parameters have already been specified.
    ERROR (SFE-1025): "/homes/cadence/lab2/spi/tb_1.txt" 131:
        Instance `V0': Unexpected value `0' - all required positional
        parameters have already been specified.
    ERROR (SFE-1025): "/homes/cadence/lab2/spi/tb_1.txt" 131:
        Instance `V0': Unexpected value `1e-07' - all required positional
        parameters have already been specified.
    ERROR (SFE-1025): "/homes/cadence/lab2/spi/tb_1.txt" 131:
        Instance `V0': Unexpected value `0' - all required positional 
       parameters have already been specified. 
--------------------------- 

 I checked all the code but didn't find why I got the "required positional parameters" which "have already been specified".

Can someone help me ? Thanks in advance.

Regards,
Wayne, 

  • Wayne,

    Because your file has the suffix ".txt", it's assumed to be in SPICE rather than spectre syntax. If you want spectre syntax, you'll need to either give the file the suffix ".scs" (which will then assume it's in spectre syntax throughout), or add the line before any spectre syntax starts:

    simulator lang=spectre

    You shouldn't need (or shouldn't have) the backslash before the open square bracket - so wave=[0 0 ...] is what you want.

    Regards,

    Andrew.

  • Thank you for reply, Andrew.

    Yes, it works good now but just a little bit weird. When I use the stimulus file with suffix ".txt" to the "vpulse" simulation, it runs OK (the ".scs" file here is OK too). For these two processes, I just changed the voltage source part (from "vpulse" to "vpwl") without changing any other thing. Why I can't use the suffix ".txt" for the voltage source of "vpwl"?

    Regards,

    Wayne. 

  • Wayne,

    Quite simply, you got lucky with the pulse source. Both statements you showed are in spectre syntax, and the simulator lang=spectre or .scs suffix would have worked for both. Because of the fact that SPICE syntax is pretty inconsistent (compared with spectre, which is a lot more regular), the simple parameter=value form of the pulse source meant that the SPICE parser was still able to unambiguously read the spectre statement despite it not being a normal SPICE way of describing a pulse source. It just fell through to a generic instance recognition and worked. The PWL source requires a vector of time-value pairs enclosed in square brackets and that's enough to cause confusion because it really isn't SPICE syntax or anything like SPICE syntax any more.

    I'd never rely on this luck - always be explicit. If it is in spectre syntax put it in a file with a .scs suffix, or failing that use the simulator lang=spectre directive. That way it is clear and unambiguous.

    Regards,

    Andrew 

  • Thank you so much for your help! It's really useful.

    Best Regards,

    Wayne.

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.