• State Resolved
  • Locked Locked
  • Replies 1 reply
  • Subscribers 38 subscribers
  • Views 4531 views
  • Users 0 members are here
Support feedback
Options
Options
Related

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

Using Spice Model in Cadence icfb

Daniel Sausner
Prodigy 10 points
Other Parts Discussed in Thread: OPA2227

Hi,

I'm not quite sure if this is the right place to ask, but I give it a try:

As a part of my thesis here, I have to simulate some circuits with the analog Cadence environment (icfb) and TISpiceD simulator, containing the OPA2227. I searched the internet and found some people saying that one can use Spice models within icfb using "CDL in...". I tried this, but I'm facing now two problems:

1. The interpreter seems to ignore all RLC-units, I guess the spice file has a incompatible syntax here. Unfortunately I don't know how to fix it. I couldn't find any information about it on the internet. Does anyone know help here (how to do or where to get information)?

2. Due to problem 1. there are only transistors in the resulting schematic, but they all just come with the default parameters. It seems like all the transistor here just come with parameters like gate width etc. while they are being discribed in the netlist with typical Spice parameters like IS, BF etc. Since I couldn't find any transistor in the huge library which could handle those parameters, I'm asking you: is there a "Spice-like" transistor available in the library at all?

It is not necessary for me to build a graphical schematic, so if there is a way to directly use the Spice netlist for simulation, please let me know. Same if you're needing more information.

 

Thanks in advance and kind regards,

Daniel

  • 0
    TI__Expert 3875 points

    Hi Daniel,

    Cadence "CDL in ..." does not comprehend SPICE syntax sufficiently to import an analog block, like an OPAMP. You can, however, create a symbol in icfb for the OPA2227 and have it refer to a text file containing the OPA2227. You can use the following steps:

    1) Save just the .subckt containing your     OPA2227 implementation to a file. Please make the name of the subckt "OPA2227".

    2) Create a symbol for     OPA2227 in icfb. The symbol should have exactly the same number of pins as the subckt in step 1 above.

    3) Please copy the "symbol" view to "TIspiceD". You can do that in the Library Manager. In other words, view name "TIspiceD" should contain the cell symbol.

    4) Please add the following simInfo to the CDF:

        cdfId->simInfo->TIspiceD = '( nil
           namePrefix        "X"
           termOrder         ("TERM1" "TERM2" ... "TERM<n>")
           componentName     "    <Subcircuit Name>"
           netlistProcedure  nil
       )

       where

           ("TERM1" "TERM2" ... "TERM<n>") specifies the terminal
           order. You will want to list the terminal names that appear
           on the symbol in the order in which they occur on the
           subcircuit definition in your text file.

           "<Subcircuit Name>" is the name of the OPA2227 subcircuit in your text file.

       So, as an example, the following simInfo

       cdfId->simInfo->TIspiceD = '( nil
           namePrefix        "X"
           termOrder         ("AVDD" "AVSS" "INP" "INM" "OUT")
           componentName     "    OPA2227"
           netlistProcedure  nil
       )

       will give you

       XI1 AVDD AVSS net1 net2 net3     OPA2227


       where "I1" was the name of the instance on the schematic where
       symbol "    OPA2227" was placed. "net1", "net2", and "net3"
       are the nets connected to pins "INP", "INM", and "OUT" on the symbol, respectively.

       You can modify the CDF by clicking "Tools"->"CDF"->"Edit ..." in
       the CIW. Make sure you are editing the "Base" CDF to ensure your
       changes become permanent.

    5) At this point you should get the instance declaration without a subcircuit definition. You will need to add the file containing the subckt definition as an include in ADE so that it will be netlisted as a .INCLUDE.


    All that said, TI does not provide support for its COT IC design flow (icfb, TIspiceD, etc.) on these forums. Support questions need to go to your university IT/CAD person, who has the option of forwarding it to TI's COT organization. So, please don't post questions related to Cadence/icfb/TIspiceD.


    Hope this helps,
    Michael Krasnicki
     

    -- 
    Michael Krasnicki
    Analog eLab
    Texas Instruments