How can I fix the error in my simulation?

The simplest approach would be to give the model file a suffix other than “.scs”, for example “MODEL.spi”. If spectre reads a file with the suffix “.scs” then it is assumed to be in spectre syntax; anything else is assumed to be in SPICE syntax. 

Alternatively, put the line:

simulator lang=spice 

at the very beginning of your model file. This will tell spectre to switch its language from the default for the given file suffix. 

Regards,

Andrew

Thank you for your exactly reply!

And, I would like to import this model card.

* Beta Version released on 2/22/06

* PTM 130nm NMOS 
 
.model  nmos  nmos  level = 54

+version = 4.0          binunit = 1            paramchk= 1            mobmod  = 0          
+capmod  = 2            igcmod  = 1            igbmod  = 1            geomod  = 1          
+diomod  = 1            rdsmod  = 0            rbodymod= 1            rgatemod= 1          
+permod  = 1            acnqsmod= 0            trnqsmod= 0          

+tnom    = 27           toxe    = 2.25e-9      toxp    = 1.6e-9       toxm    = 2.25e-9   
+dtox    = 0.65e-9      epsrox  = 3.9          wint    = 5e-009       lint    = 10.5e-009   
+ll      = 0            wl      = 0            lln     = 1            wln     = 1          
+lw      = 0            ww      = 0            lwn     = 1            wwn     = 1          
+lwl     = 0            wwl     = 0            xpart   = 0            toxref  = 2.25e-9   
+xl      = -60e-9
+vth0    = 0.3782       k1      = 0.4          k2      = 0.01         k3      = 0          
+k3b     = 0            w0      = 2.5e-006     dvt0    = 1            dvt1    = 2       
+dvt2    = -0.032       dvt0w   = 0            dvt1w   = 0            dvt2w   = 0          
+dsub    = 0.1          minv    = 0.05         voffl   = 0            dvtp0   = 1.2e-010     
+dvtp1   = 0.1          lpe0    = 0            lpeb    = 0            xj      = 3.92e-008   
+ngate   = 2e+020       ndep    = 1.54e+018    nsd     = 2e+020       phin    = 0          
+cdsc    = 0.0002       cdscb   = 0            cdscd   = 0            cit     = 0          
+voff    = -0.13        nfactor = 1.5          eta0    = 0.0092       etab    = 0          
+vfb     = -0.55        u0      = 0.05928      ua      = 6e-010       ub      = 1.2e-018     
+uc      = 0            vsat    = 100370       a0      = 1            ags     = 1e-020     
+a1      = 0            a2      = 1            b0      = 0            b1      = 0          
+keta    = 0.04         dwg     = 0            dwb     = 0            pclm    = 0.06       
+pdiblc1 = 0.001        pdiblc2 = 0.001        pdiblcb = -0.005       drout   = 0.5        
+pvag    = 1e-020       delta   = 0.01         pscbe1  = 8.14e+008    pscbe2  = 1e-007     
+fprout  = 0.2          pdits   = 0.08         pditsd  = 0.23         pditsl  = 2.3e+006   
+rsh     = 5            rdsw    = 200          rsw     = 100          rdw     = 100        
+rdswmin = 0            rdwmin  = 0            rswmin  = 0            prwg    = 0          
+prwb    = 6.8e-011     wr      = 1            alpha0  = 0.074        alpha1  = 0.005      
+beta0   = 30           agidl   = 0.0002       bgidl   = 2.1e+009     cgidl   = 0.0002     
+egidl   = 0.8          

+aigbacc = 0.012        bigbacc = 0.0028       cigbacc = 0.002     
+nigbacc = 1            aigbinv = 0.014        bigbinv = 0.004        cigbinv = 0.004      
+eigbinv = 1.1          nigbinv = 3            aigc    = 0.012        bigc    = 0.0028     
+cigc    = 0.002        aigsd   = 0.012        bigsd   = 0.0028       cigsd   = 0.002     
+nigc    = 1            poxedge = 1            pigcd   = 1            ntox    = 1          

+xrcrg1  = 12           xrcrg2  = 5          
+cgso    = 2.4e-010     cgdo    = 2.4e-010     cgbo    = 2.56e-011    cgdl    = 2.653e-10     
+cgsl    = 2.653e-10    ckappas = 0.03         ckappad = 0.03         acde    = 1          
+moin    = 15           noff    = 0.9          voffcv  = 0.02       

+kt1     = -0.11        kt1l    = 0            kt2     = 0.022        ute     = -1.5       
+ua1     = 4.31e-009    ub1     = 7.61e-018    uc1     = -5.6e-011    prt     = 0          
+at      = 33000      

+fnoimod = 1            tnoimod = 0          

+jss     = 0.0001       jsws    = 1e-011       jswgs   = 1e-010       njs     = 1          
+ijthsfwd= 0.01         ijthsrev= 0.001        bvs     = 10           xjbvs   = 1          
+jsd     = 0.0001       jswd    = 1e-011       jswgd   = 1e-010       njd     = 1          
+ijthdfwd= 0.01         ijthdrev= 0.001        bvd     = 10           xjbvd   = 1          
+pbs     = 1            cjs     = 0.0005       mjs     = 0.5          pbsws   = 1          
+cjsws   = 5e-010       mjsws   = 0.33         pbswgs  = 1            cjswgs  = 3e-010     
+mjswgs  = 0.33         pbd     = 1            cjd     = 0.0005       mjd     = 0.5        
+pbswd   = 1            cjswd   = 5e-010       mjswd   = 0.33         pbswgd  = 1          
+cjswgd  = 5e-010       mjswgd  = 0.33         tpb     = 0.005        tcj     = 0.001      
+tpbsw   = 0.005        tcjsw   = 0.001        tpbswg  = 0.005        tcjswg  = 0.001      
+xtis    = 3            xtid    = 3          

+dmcg    = 0e-006       dmci    = 0e-006       dmdg    = 0e-006       dmcgt   = 0e-007     
+dwj     = 0.0e-008     xgw     = 0e-007       xgl     = 0e-008     

+rshg    = 0.4          gbmin   = 1e-010       rbpb    = 5            rbpd    = 15         
+rbps    = 15           rbdb    = 15           rbsb    = 15           ngcon   = 1          

     

This model card is a SPICE level 54 model, which is a BSIM4 model.

But, in Spectre Circuit Simulator Components and Device Models Reference of Cadence help, BSIM4 is Level-14 Model.

If I want to use this model, is it correct to set the level of the model to level=54, or is it correct to set level=14? (My simulator is Spectre.)

(I am curious if the level value of the red box in the image below is 54 or 14.)

Please tell me about this.

Thank you

yysunj

The level numbers are the HSPICE level numbers, and they are supported too (we don't necessary document the details of all that compatibility). Both work though - the level 49 model you posted first corresponds to bsim3v3, and level 54 corresponds to bsim4. It's clear if you just use these from the spectre log file - it tells you:

Circuit inventory:
              nodes 2
          bsim3v3 1
              bsim4 1

(this was with an instance of both of your models in my netlist; note I had to rename the models to use both since they were both called NMOS).

Andrew

The level numbers are the HSPICE level numbers, and they are supported too (we don't necessary document the details of all that compatibility). Both work though - the level 49 model you posted first corresponds to bsim3v3, and level 54 corresponds to bsim4. It's clear if you just use these from the spectre log file - it tells you:

Circuit inventory:
              nodes 2
          bsim3v3 1
              bsim4 1

(this was with an instance of both of your models in my netlist; note I had to rename the models to use both since they were both called NMOS).

Andrew