Stats

  • Locked Locked
  • Replies 2
  • Subscribers 124
  • Views 13964
  • 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

Spice3 circuit file simulation by Spectre.

archive

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
  • archive

    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
  • archive

    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

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.