Stats

  • Locked Locked
  • Replies 1
  • Subscribers 125
  • Views 16098
  • 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

Problem in simulating SPICE model in spectre

farhan89

Hello,
I got a user developed SPICE model for a transistor. He is using LTSpice to simulate the model and everything works fine for him. I created a symbol in Virtuoso 6.16, added spectre stop view in cell view (also all relevant CDF simulation information) and included model path in model library. Now when I try to simulate (MMSIM 13.1) it I don't get warning:
  `I' is not a valid parameter for an instance of `ibis_buffer'.  Ignored.

and error

  ERROR (CMI-2631): Unable to parse IBIS file .
  ERROR (CMI-2731): M0.BIXZ: Model name is not defined for IBIS buffer

  What could be the reason for it? I believe this is because of if..else conditions in behavioral source value calculation?. Kindly see the example of the model below (I couldn't attach the original model because of copyright issue).

**myFunctions
simulator lang=spice

.FUNC myfunc1( A, B, C ) {A + B + C}
.FUNC myfunc2( A, B, C ) {A - B - C}
.FUNC myfunc3( A, B, C ) {A * B * C}

**myModel
subckt myModel X Y Z
.param
+W=100u L=100u
+a1 = 1u
+a2 = 2u
    *Behavioral current source between X and Z node
    BIXZ X Z I=(W/L) * (if(V(Y, Z) <= 0.3, myfunc1(A, B, C), if(V(Y, Z) > 0.3 & V(Y, Z) < 0.7, myfunc2(A, B, C), myfunc3(A, B, C))))
    *resistance between X and Z node
    R X Z 10e9

.ends

P.S: Sorry, I had to change the title and text of the post to make my query more understandable

  • Andrew Beckett

    Spectre does not support LTSpice models; the trouble with "behavioural" SPICE models is that they have a tendency to be somewhat simulator dependent. In the above case, you're just treating the "B" element as how it would be interpreted in a generic SPICE, which tends to follow HSPICE behaviour. In that case a "B" element would be an IBIS buffer, which is not what you have here.

    I did try seeing if the above could be interpreted as a PSPICE model - spectre has support for PSPICE models using pspice_include, but even then it fails (after changing the subckt to .subckt):

    Error found by spectre in `myModel', during circuit read-in.
    ERROR (SFE-400): "forum30.psp" 14: The instance `BIXZ' does not have a
    valid master.

    I've not checked to see if "B" is a valid element type in PSPICE. 

    As was advised before, you may be better off converting this into an equivalent VerilogA model. An earlier version of your post seemed to show using bsource in spectre, but even that is just a convenient way of avoiding the need for a VerilogA model.

    Perhaps you would be better off contacting customer support so we can see the precise model you're using rather than something which you may have broken in the editing.

    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.