Home > Community > Forums > Custom IC Design > Spice3 circuit file simulation by Spectre.

Email
* Required Fields

Recipients email * (separate multiple addresses with commas)

Your name *

Your email *

Message *

Contact Us

Cadence Contacts

Global Office Locator
Find Offices worldwide »

Sales Inquiry
Request for Product information »
Cadence Channel Partners »

Corporate Headquarters
Cadence Design Systems, Inc.
2655 Seely Avenue
San Jose, CA 95134
Phone: 408.943.1234
* Required Fields
First Name *

Last Name *

Email *

Company / Institution *

Comments: *

 Spice3 circuit file simulation by Spectre. 

Last post Sat, Apr 22 2006 6:51 AM by archive. 2 replies.
Started by archive 22 Apr 2006 06:51 AM. Topic has 2 replies.
Page 1 of 1 (3 items)
Sort Posts:

  • Sat, Apr 22 2006 6:51 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,740
    Spice3 circuit file simulation by Spectre. Reply

    How We can simulate our circuit descibed in old spice format as shown below?
    Can we simulate them in Spectre?
    We are using ICFB 5.141 USR3.

    Attached a complete workable spice file for XOR gate. Can Spectre run this file ?

    Kind Regards
    Mayank



    m1000 Vdd A a_n20_44# Vdd pfet w=12u l=3u
    + ad=320p pd=160u as=76p ps=40u

    V1 B 0 PULSE (0 5v 0 0 0 70ns 100ns)
    V2 A 0 PULSE (0 5v 0 0 0 25ns 60ns)
    Vdd Vdd 0 DC=5.0
    .TRAN 5ns 100ns

    .MODEL nfet  NMOS (level=2 LD=0.15U TOX=200.0E-10 NSUB=5.37E+15
    + VTO=0.74 KP=8.0E-05 GAMMA=0.54 PHI=0.6 U0=656 UEXP=0.157 UCRIT=31444
    + DELTA=2.34 VMAX=55261 Xj=0.2U LAMBDA=0.037 NFS=1E+12 NEFF=1.001 NSS=1E+11
    + TPG=1.0 RSH=70.00
    + CGDO=4.3E-10 CGSO=4.3E-10 Cj=0.0003 Mj=0.66
    + CJSW=8.0E-10 MJSW=0.24 PB=0.58

    .MODEL pfet PMOS (level=2 LD=0.15U TOX=200.0E-10 NSUB=4.33E+15
    + VTO=-0.74 KP=2.70E-05 GAMMA=0.58 PHI=0.6 U0=262 UEXP=0.324 UCRIT=65720
    + DELTA=1.79 VMAX=25694 Xj=0.25U LAMBDA=0.061 NFS=1E+12 NEFF=1.001 NSS=1E+11
    + TPG=1.0 RSH=121.00
    + CGDO=4.3E-10 CGSO=4.3E-10 Cj=0.0005 Mj=0.51
    + CJSW=1.35E-10 MJSW=0.24 PB=0.64
    .END



    Originally posted in cdnusers.org by mayank
    XOR.spice.doc
    • Post Points: 0

  • Mon, Apr 24 2006 6:17 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,740
    RE: Spice3 circuit file simulation by Spectre. Reply

    Hi, With 5.1.41 you can turn on the +csfe option to spectre to read spice netlists. unix> spectre +csfe test.ckt Your netlist above will still fail since the rise and fall times of V1 and V2 are 0. Also, you need to change 5v to just 5. Regards, Eric


    Originally posted in cdnusers.org by EricCDN
    • Post Points: 0

  • Wed, May 3 2006 8:58 AM

    • archive
    • Top 75 Contributor
    • Joined on Fri, Jul 4 2008
    • Posts 88
    • Points 4,740
    RE: Spice3 circuit file simulation by Spectre. Reply

    The 5v will only give a warning, but zero rise/fall will give an error (it's meaningless anyway).
    If using MMSIM60, the new front end is on by default, so you can just run spectre on it directly (assuming you've fixed the rise/fall times to something meaningful).

    Regards,

    Andrew.


    Originally posted in cdnusers.org by adbeckett
    • Post Points: 0
Page 1 of 1 (3 items)
Sort Posts:
Started by archive at 22 Apr 2006 06:51 AM. Topic has 2 replies.