Home > Community > Forums > Custom IC Design > Spice to Spectre

Email

* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Spice to Spectre 

Last post Tue, Aug 6 2013 11:30 AM by chaosatom. 3 replies.
Started by chaosatom 05 Aug 2013 03:39 PM. Topic has 3 replies and 913 views
Page 1 of 1 (4 items)
Sort Posts:
  • Mon, Aug 5 2013 3:39 PM

    • chaosatom
    • Not Ranked
    • Joined on Mon, Jul 29 2013
    • Posts 8
    • Points 100
    Spice to Spectre Reply

     I have tried to follow these step for getting a diode in spice to appear in spectre, but I get errors:

     1. Convert the SPICE block using spp.

    ---This is the output: 

     simulator lang=spectre insensitive=yes
    subckt x1n4735a ( 1 2 )
    //
    //  The resistor R1 does not reflect
    //  a physical device. Instead it
    //  improves modeling in the reverse
    //  mode of operation.
    //
    r1 ( 1 2 ) resistor r=3e+9
    d1 ( 1 2 ) d1n4735a
    //
    model d1n4735a diode
    + is=7.526e-16              n=0.992                   bv=5.105
    + ibv=0.005                 rs=0.2338                 cjo=129.04e-12
    + vj=.46589                 m=.2767

    2. Open any schematic, select Design -> Create Cellview->From
    pin list, and type in the destination symbol and pin list.

     ----I opened an empty schematic and created a symbol (input and output ports labeled 1, 2)

    3. From the symbol view, choose Design->Save As, and save it as a spectre
    view. Alternatively, use the Library Manager to copy the symbol view to the
    spectre view.

     ----I have copied symbol and view name to spectre. 


    4. Start Artist, and in the Setup -> Model Libraries form, include the path
    to the converted text.

    ---I created another cellview. Instianted the spectre symbol for the diode. Went to model and attacted the file.


    5. Set the model property on the block to be the same as the top-level
    subcircuit name in the converted text. You will probably need to add the
    model property. Just select the block, then choose Edit -> Properties ->
    Objects. Next, Click on the Add button in the User Property section. For
    "name", put "model", "type" should be "string", and you can leave the other
    two fields blank. Under the Local Value on the Properties form, enter the
    name of the top-level subcircuit.

    -------Gave the local value of x1n4735. Ran a DC sweep  

     I get this error:

    p, li { white-space: pre-wra

    WARNING (ADE-1065): No simulation results are available.

    Delete psf data in /ti/home/vipul/cadence/simulation/test_circuit/spectre/schematic/psf.

    generate netlist...

    Begin Incremental Netlisting Aug 5 15:38:09 2013

    Netlist Error: Cannot find any info on instance "I1" in cell-view "Mppt2" "test_circuit" "schematic"

    Netlist Error: Some cell-views used inside this block could not be netlisted in analog context

    End netlisting Aug 5 15:38:09 2013

    ERROR (OSSHNL-514): Netlisting failed due to errors reported before. Netlist may be corrupt or may not be produced at all. Fix reported errors and netlist again.

    ...unsuccessful.

     

    ------ The schematic is empty, so should I put something in there? I am confused. 

     

    • Post Points: 20
  • Tue, Aug 6 2013 3:13 AM

    Re: Spice to Spectre Reply

    You didn't set up the CDF for the cell  x1n4735. In step 5 you added a user-defined property with the model name, which won't be used...

    So, go to Tools->CDF->Edit CDF in the CIW, and set the CDF type to be Base. Set the cell name to be x1n4735, and then add a CDF parameter called "model" which you can give a default value of x1n4735, In the Simulation Information section, set the termOrder for spectre to be "1 2" and that's pretty much all you need.

    BTW, you don't really need to use spp these days - spectre should be able to read SPICE syntax directly (the spp translator hasn't been touched in about 10 years).

    Regards,

    Andrew.

     

    • Post Points: 35
  • Tue, Aug 6 2013 11:15 AM

    • chaosatom
    • Not Ranked
    • Joined on Mon, Jul 29 2013
    • Posts 8
    • Points 100
    Re: Spice to Spectre Reply

    Ok thanks, it works now. 

    I also used this thread:

    http://www.cadence.com/Community/blogs/rf/archive/2009/01/07/tip-of-the-week-how-to-simulate-a-subcircuit-netlist-with-spectre-in-ade.aspx

    I was also making the mistake of editing the CDF of the instantiate cellview. Also, I just used my spice subcircuit model instead of converting to spectre.    

    Vipul 

     

    • Post Points: 5
  • Tue, Aug 6 2013 11:30 AM

    • chaosatom
    • Not Ranked
    • Joined on Mon, Jul 29 2013
    • Posts 8
    • Points 100
    Re: Spice to Spectre Reply
    I got one more question if you don't mind. I can't seem to probe the current of my subcircuit diode. Although I can probe the current from VDC that I am supplying voltage from. I basically see a blank screen if I probe the current of my sub circuit diode. Am I missing something there? Thanks, Vipul
    • Post Points: 5
Page 1 of 1 (4 items)
Sort Posts:
Started by chaosatom at 05 Aug 2013 03:39 PM. Topic has 3 replies.