Stats

  • Locked Locked
  • Replies 4
  • Subscribers 124
  • Views 6852
  • 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

Spice lib

StreamCX

 I convert my project from 5 to 6 version.

When I try to simulate with old library this message appears.

[URL=http://img708.imageshack.us/i/spice.png/][IMG]img708.imageshack.us/.../URL]

When I write "simulate lang = spice" in My *.scs lib file this appears 

[URL=http://img821.imageshack.us/i/cadenceerror.png/][IMG]img821.imageshack.us/.../URL]

Description of MOS tran with nmos param

[URL=http://img689.imageshack.us/i/facellmodel.png/][IMG]img689.imageshack.us/.../URL]

How can I use this model to simulate project? That lib works in Cadence 5.

 //There is no name like nmos4, pmos4

* Nterest

.model  kn nmos level=2 phi=.65 tox=55n xj=.34u tpg=0
+ VTO=0.5 LD=0.15u  WD=.04u  UO=460
+ NSUB=25E+15
+ CJ=0.0004 
+ GAMMA=1.1
*
.model  kn_nat nmos level=2 phi=.65 tox=55n xj=.34u tpg=0
+ VTO=0.5 LD=0.15u  WD=.04u  UO=460
+ NSUB=25E+15
+ CJ=0.0004
+ GAMMA=1.1
*
.MODEL  Kp PMOS LEVEL=2 PHI=0.65 TOX=55n XJ=0.4U TPG=0
+ VTO=-1.1   LD=.25u WD=.04u  UO=160
+ NSUB=1.1E+15 
+ CJ=3.1E-04
+ GAMMA=0.27
.MODEL  kp_lVt PMOS LEVEL=2 PHI=0.65 TOX=55n XJ=0.4U TPG=0
+ VTO=-1.1   LD=.25u WD=.04u  UO=160
+ NSUB=1.1E+15 
+ CJ=3.1E-04
+ GAMMA=0.27
.model diod d(is=1.0e-12 rs=2 cjo=1p bv=50 vj=.6)
.model diode d(is=1.0e-12 rs=2 cjo=1p bv=50 vj=.6)
*.subckt mkn d g s b
*mkn d g s b kn w=w l=l
*.ends mkn

I try add  .model  kn [b]nmos4[/b] level=2 phi=.65 tox=55n xj=.34u tpg=0
+ VTO=0.5 LD=0.15u  WD=.04u  UO=460
+ NSUB=25E+15
+ CJ=0.0004 
+ GAMMA=1.1

That does not solve the problem.

  • Andrew Beckett

    My guess is that  you have not set:

    setenv CDS_Netlisting_Mode Analog   

    (for csh) or:

    export CDS_Netlisting_Mode=Analog

    for bash/ksh.

    Because of that, the instance lines in the spectre netlist are showing the component name rather than the model name. Rather hard to be sure, because you didn't show the netlist.

    Note also that it's better to show the actual text, rather than a picture - as these are easier to look at and search in future.

    Regards,

    Andrew.

  • StreamCX

    Andrew Becket, 

    I take account of your answer.

    I changed *.scs file to

    simulator lang=spectre

    model nmos4 mos2 type=n phi=.65 tox=55n xj=.34u tpg=0
    + vto=0.5 ld=0.15u  wd=.04u  uo=460
    + nsub=25E+15
    + cj=0.0004  
    + gamma=1.1

    model nmos4nat mos2 type=n phi=.65 tox=55n xj=.34u tpg=0
    + vto=0.5 ld=0.15u  wd=.04u  uo=460
    + nsub=25E+15
    + cj=0.0004  
    + gamma=1.1

    model pmos4 mos2 type=p phi=0.65 tox=55n xj=0.4u tpg=0
    + vto=-1.1   ld=.25u wd=.04u  uo=160
    + nsub=1.1E+15  
    + cj=3.1E-04
    + gamma=0.27

    model pmos4_lVt mos2 type=p phi=0.65 tox=55n xj=0.4u tpg=0
    + vto=-1.1   ld=.25u wd=.04u  uo=160
    + nsub=1.1E+15  
    + cj=3.1E-04
    + gamma=0.27

    model pmos mos2 type=p phi=0.65 tox=55n xj=0.4u tpg=0
    + vto=-1.1   ld=.25u wd=.04u  uo=160
    + nsub=1.1E+15  
    + cj=3.1E-04
    + gamma=0.27

     That works.

    Where can I find basic models of diode?

  • Andrew Beckett

    Not really sure why you had to change the syntax of the model files.

    BTW, I think you edited your last posting in this thread, rather than adding a new one. If you edit a post, there's no email notifier sent to people subscribing. So if you post something which doesn't require an answer, and then edit it to include a new question, it's quite possible nobody will even notice that you've asked a new question.

    If you need diode models, either get them from the foundry you're using (best solution), or if you want something representative, then there are design kits such as the Cadence GPDK (Generic Process Design Kit) for various nodes, as well as some similar university PDKs - e.g. from NCSU.

    Regards,

    Andrew.

  • StreamCX

    That file after I changed cds_netlisting mode to analog  

    simulator lang=spectre

    model kn mos2 type=n phi=.65 tox=55n xj=.34u tpg=0
    + vto=0.5 ld=0.15u  wd=.04u  uo=460
    + nsub=25E+15
    + cj=0.0004  
    + gamma=1.1

    model kn_nat mos2 type=n phi=.65 tox=55n xj=.34u tpg=0
    + vto=0.5 ld=0.15u  wd=.04u  uo=460
    + nsub=25E+15
    + cj=0.0004  
    + gamma=1.1

    model kp mos2 type=p phi=0.65 tox=55n xj=0.4u tpg=0
    + vto=-1.1   ld=.25u wd=.04u  uo=160
    + nsub=1.1E+15  
    + cj=3.1E-04
    + gamma=0.27

    model kp_lVt mos2 type=p phi=0.65 tox=55n xj=0.4u tpg=0
    + vto=-1.1   ld=.25u wd=.04u  uo=160
    + nsub=1.1E+15  
    + cj=3.1E-04
    + gamma=0.27

    model pmos mos2 type=p phi=0.65 tox=55n xj=0.4u tpg=0
    + vto=-1.1   ld=.25u wd=.04u  uo=160
    + nsub=1.1E+15  
    + cj=3.1E-04
    + gamma=0.27

    model diod diode is=1.0e-12 rs=2 cjo=1p bv=50 vj=.6
    model diode diode is=1.0e-12 rs=2 cjo=1p bv=50 vj=.6

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.