Stats

  • Locked Locked
  • Replies 1
  • Subscribers 126
  • Views 2978
  • 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

Virtuoso - how can I create an instance from a .inc HSPICE file?

Alex2kdl
Hi, I am facing a problem with Virtuoso that I can't seem to solve. I am designing a circuit that uses a new component. This component has two terminals and I have an HSPICE .inc file that describes it as a sub circuit. The file is of the following format: .SUBCKT COMPONENTNAME n+ n- .PRINT R(component) . ++(.PARM, behvioral sources, MAX, MIN, etc are used here) . .ends COMPONENTNAME I would like to create a schematic instance for the component so that I can easily use it. How do I do this? I suppose that I have to create a new cellview of name COMPONENTNAME and I also suppose that I will have to include the .inc file in Analog Environment. How do I get the cellview to "point" to the .inc file, though? Could anybody refer me to some tutorial or help file? Also, is it sufficient to select "Use SPICE netlist reader" in analog environment to get Spectre to properly process the .inc HSPICE file? Thanks a lot! -Alex

  • Hi Alex

    You can do it as follows:

    a. Create a cell that has a symbol with 2 pins n+ and n-
    b. Copy the symbol view as "spectre" view
    c. In ciw, go to "Tools->CDF->Edit" and select the newly created cell. Set to "base" cdf.
    d. Go to "Simulation Information" section and select "Spectre" as the simulator
    e. Set the name of the subckt as the value for "componentName"
    f. Ensure that "termOrder" is the same order as the netlist
    g. Add "simulator lang=spice" as the first line in the netlist
    h. In ADE-L, go to "Setup->Model files" and add the netlist as one of the model files

    You can now use the symbol in your schematic for simulation. COS solution 11208254 explains the above steps.

    Actually "spice netlist reader" or more commonly known as "spp" is just used to pre-process a spice netlist and convert it to a spectre netlist. It will not really help in your case because you still need a way to represent the netlist in your schematic. The usage of spp is also no longer necessary because spectre can read in a spice netlist directly.

    Best regards
    Quek

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.