Stats

  • Locked Locked
  • Replies 7
  • Subscribers 127
  • Views 20101
  • 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

Problem simulating Spice Netlist with Spectre

Oriba

Hello,

Recently i tried to simulate the following Spice netList with Spectre:( by : spectre filename.sp)

 simulator lang = spice
.SUBCKT modelmemristor plus minus PARAMS:

+phio=0.95 Lm=0.0998 w1=0.1261 foff=3.5e-6
+ioff=115e-6 aoff=1.2 fon=40e-6 ion=8.9e-6
+aon=1.8 b=500e-6 wc=107e-3
G1 plus internal value={sgn(V(x))*(1/V(dw))^2*0.0617*(V(phiI)*exp(-V(B)*V(sr))-(V(phiI)+abs(V(x)))*exp(-V(B)*V(sr2)))}
Esr sr 0 value={sqrt(V(phiI))}
Esr2 sr2 0 value={sqrt(V(phiI)+abs(V(x)))}
Rs internal minus 215
Eg x 0 value={V(plus)-V(internal)}
Elamda Lmda 0 value={Lm/V(w)}
Ew2 w2 0 value={w1+V(w)-(0.9183/(2.85+4*V(Lmda)-2*abs(V(x))))}
EDw dw 0 value={V(w2)-w1}
EB B 0 value={10.246*V(dw)}
ER R 0 value={(V(w2)/w1)*(V(w)-w1)/(V(w)-V(w2))}
EphiI phiI 0 value={phio-abs(V(x))*((w1+V(w2))/(2*V(w)))-1.15*V(Lmda)*V(w)*log(V(R))/V(dw)}
C1 w 0 1e-9 IC=1.2
R w 0 1e8MEG
Ec c 0 value={abs(V(internal)-V(minus))/215}
Emon1 mon1 0 value={((V(w)-aoff)/wc)-(V(c)/b)}
Emon2 mon2 0 value={(aon-V(w))/wc-(V(c)/b)}
Goff 0 w value={foff*sinh(stp(V(x))*V(c)/ioff)*exp(-exp(V(mon1))-V(w)/wc)}
Gon w 0 value={fon*sinh(stp(-V(x))*V(c)/ion)*exp(-exp(V(mon2))-V(w)/wc)}
.ENDS modelmemristor

 When doing so, i got the following errors:

 Error found by spectre in `modelmemristor', during circuit read-in.
    ERROR (SFE-1815): "Mem.sp" 2: Missing value for parameter `G1' in
        subcircuit definition `modelmemristor'.
    ERROR (SFE-662): "Mem.sp" 2: Badly formed subcircuit definition
        `modelmemristor'.

I looked a littel bit and tried to change the G1 parameter to the following:

G1 plus internal 0 xx value={sgn(V(x))*(1/V(dw))^2*0.0617*(V(phiI)*exp(-V(B)*V(sr))-(V(phiI)+abs(V(x)))*exp(-V(B)*V(sr2)))}
Exx xx 0 1

But still same Errors..
Can anyway know what is the problem??
My final goal is to attach this netlist to a symbol so i can use it in virtuoso.
Thanks

Parents

  • I tried this in MMSIM11.1 and got a number of problems. Spectre does not support PSPICE syntax (I think this is PSPICE), but Berkeley SPICE instead. So with a few small changes I got it to compile OK (you'll have to test that it actually works OK):

     
    simulator lang=spectre
    ** this function does not exist in spectre, so implement it ourselves
    real stp(real a) {
        return a>0?1.0:0.0
    }
    simulator lang=spice

    ** the SPICE parser in spectre does not support PARAMS: so change to conventional
    ** SPICE syntax
    ** Also change all {} to ''
    .SUBCKT modelmemristor plus minus $PARAMS:
    .PARAM
    +phio=0.95 Lm=0.0998 w1=0.1261 foff=3.5e-6
    +ioff=115e-6 aoff=1.2 fon=40e-6 ion=8.9e-6
    +aon=1.8 b=500e-6 wc=107e-3
    G1 plus internal value='sgn(V(x))*(1/V(dw))^2*0.0617*(V(phiI)*exp(-V(B)*V(sr))-(V(phiI)+abs(V(x)))*exp(-V(B)*V(sr2)))'
    Esr sr 0 value='sqrt(V(phiI))'
    Esr2 sr2 0 value='sqrt(V(phiI)+abs(V(x)))'
    Rs internal minus 215
    Eg x 0 value='V(plus)-V(internal)'
    Elamda Lmda 0 value='Lm/V(w)'
    Ew2 w2 0 value='w1+V(w)-(0.9183/(2.85+4*V(Lmda)-2*abs(V(x))))'
    EDw dw 0 value='V(w2)-w1'
    EB B 0 value='10.246*V(dw)'
    ER R 0 value='(V(w2)/w1)*(V(w)-w1)/(V(w)-V(w2))'
    EphiI phiI 0 value='phio-abs(V(x))*((w1+V(w2))/(2*V(w)))-1.15*V(Lmda)*V(w)*log(V(R))/V(dw)'
    C1 w 0 1e-9 IC=1.2
    ** Spectre does not support exponents with engineering suffixes together
    *R w 0 1e8MEG
    R w 0 1e14
    Ec c 0 value='abs(V(internal)-V(minus))/215'
    Emon1 mon1 0 value='((V(w)-aoff)/wc)-(V(c)/b)'
    Emon2 mon2 0 value='(aon-V(w))/wc-(V(c)/b)'
    Goff 0 w value='foff*sinh(stp(V(x))*V(c)/ioff)*exp(-exp(V(mon1))-V(w)/wc)'
    Gon w 0 value='fon*sinh(stp(-V(x))*V(c)/ion)*exp(-exp(V(mon2))-V(w)/wc)'
    .ENDS modelmemristor

     

    Regards,

    Andrew.

Reply

  • I tried this in MMSIM11.1 and got a number of problems. Spectre does not support PSPICE syntax (I think this is PSPICE), but Berkeley SPICE instead. So with a few small changes I got it to compile OK (you'll have to test that it actually works OK):

     
    simulator lang=spectre
    ** this function does not exist in spectre, so implement it ourselves
    real stp(real a) {
        return a>0?1.0:0.0
    }
    simulator lang=spice

    ** the SPICE parser in spectre does not support PARAMS: so change to conventional
    ** SPICE syntax
    ** Also change all {} to ''
    .SUBCKT modelmemristor plus minus $PARAMS:
    .PARAM
    +phio=0.95 Lm=0.0998 w1=0.1261 foff=3.5e-6
    +ioff=115e-6 aoff=1.2 fon=40e-6 ion=8.9e-6
    +aon=1.8 b=500e-6 wc=107e-3
    G1 plus internal value='sgn(V(x))*(1/V(dw))^2*0.0617*(V(phiI)*exp(-V(B)*V(sr))-(V(phiI)+abs(V(x)))*exp(-V(B)*V(sr2)))'
    Esr sr 0 value='sqrt(V(phiI))'
    Esr2 sr2 0 value='sqrt(V(phiI)+abs(V(x)))'
    Rs internal minus 215
    Eg x 0 value='V(plus)-V(internal)'
    Elamda Lmda 0 value='Lm/V(w)'
    Ew2 w2 0 value='w1+V(w)-(0.9183/(2.85+4*V(Lmda)-2*abs(V(x))))'
    EDw dw 0 value='V(w2)-w1'
    EB B 0 value='10.246*V(dw)'
    ER R 0 value='(V(w2)/w1)*(V(w)-w1)/(V(w)-V(w2))'
    EphiI phiI 0 value='phio-abs(V(x))*((w1+V(w2))/(2*V(w)))-1.15*V(Lmda)*V(w)*log(V(R))/V(dw)'
    C1 w 0 1e-9 IC=1.2
    ** Spectre does not support exponents with engineering suffixes together
    *R w 0 1e8MEG
    R w 0 1e14
    Ec c 0 value='abs(V(internal)-V(minus))/215'
    Emon1 mon1 0 value='((V(w)-aoff)/wc)-(V(c)/b)'
    Emon2 mon2 0 value='(aon-V(w))/wc-(V(c)/b)'
    Goff 0 w value='foff*sinh(stp(V(x))*V(c)/ioff)*exp(-exp(V(mon1))-V(w)/wc)'
    Gon w 0 value='fon*sinh(stp(-V(x))*V(c)/ion)*exp(-exp(V(mon2))-V(w)/wc)'
    .ENDS modelmemristor

     

    Regards,

    Andrew.

Children
No Data

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.