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 RegardsMayankm1000 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
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.
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.