SPICELib.tutorial.nandcmos

Nand gate

Information

NAND CMOS

The modeling and transient analysis of the CMOS nand gate shown in Figure 1 is discussed.
The transient analysis plots are shown.

Figure 1. CMOS Nand gate.

Circuit modeling

Start Dymola with Modelica modeling language.
In order to open SPICELib library, select in the Dymola window File/Open and open the file SPICELib/package.mo
Create a new package (select in the Dymola window File/New/Package): nandcmos.
It is going to include the circuit and the analysis models.
Create the circuit model (select in the Dymola window File/New/Model) as follows:
Dymola model window now contains an empty schematic model.
The model circuit is built up using components from the SPICELib.parts package. The model components for n-channel MOS, p-channel MOS and ground can be found in SPICELib.parts.breakout. The model component for a independent voltage source can be found in SPICELib.parts.source. Drag and drop the part models.
- SPICELib.parts.breakout.Ground
- SPICELib.parts.breakout.Spice2MOS1
- SPICELib.parts.breakout.Spice2MOS1P
- SPICELib.parts.source.VPULSE
- SPICELib.parts.source.VCONST
Connect the circuit parts as shown in Figure 1.
Enter the parameter values of the circuit components. See Figures 2-6. N1 and N2 have the same parameters. P1 and P2 also have the same parameters.
The Boolean parameter HIDDEN_COMPONENT controls the log of the device variables (see SPICELib.analyses package documentation).
Figure 2. VDD parameters.

Figure 3. V1 parameters.

Figure 4. V2 parameters.

Figure 5. NMOS parameters.

Figure 6. PMOS parameters.
Save the Schematic model.

Transient (time) analysis (TRAN)

Create a new model, TRAN, and insert it in nandcmos package (see Figure 7).
Figure 7. Inserting TRAN in nandcmos package.
Drag an SPICELib.analyses.TRAN model into the TRAN model (see Figure 8).
Figure 8. Inserting TRAN in nandcmos package.
Enter the TRAN analysis parameters (see Figure 9). The meaning of the analysis parameters is discussed in the SPICELib.analyses.TRAN model documentation. The SKIPBP parameter determines whether skip or not the bias point calculation.

Figure 9. TRAN analysis parameters.

TRANSIENT ANALYSIS

Figure 10 shows the input stimuli. Figure 11 shows the results obtaines with SPICELib and ORCAD PSPICE and in Figure 12 the difference between the results obtained with SPICELib and ORCAD PSpice is presented.

Figure 10. Input stimuli.

Figure 11. Results obtained with SPICELib and ORCAD PSpice.

Figure 12. Difference between the results obtained with SPICELib and ORCAD.

Name Description

schematic

TRAN

Name	Description
schematic
TRAN

SPICELib.tutorial.nandcmos.schematic

Information

Please, see SPICELib.tutorial.nandcmos documentation

Modelica definition

partial model schematic 
  
  parts.breakout.Ground Ground1;
  parts.breakout.Ground Ground2;
  parts.source.VPULSE V1(
    PW=500e-9, 
    AC_MAG=0, 
    DC_VALUE=5, 
    S2=0, 
    S1=5, 
    TD=0e-9, 
    PER=1040e-9, 
    TF=20e-9, 
    TR=20e-9);
  parts.source.VPULSE V2(
    AC_MAG=0, 
    TD=0e-9, 
    DC_VALUE=5, 
    S2=0, 
    S1=5, 
    PW=1000e-9, 
    PER=2040e-9, 
    TF=20e-9, 
    TR=20e-9);
  parts.breakout.Ground Ground3;
  parts.breakout.Spice2MOS1 N1(
    L=2e-6, 
    W=4e-6, 
    CJ=0.0003002, 
    LAMBDA=0.01302, 
    LD=1.526e-7, 
    MJ=0.5, 
    MJSW=0.5, 
    PB=0.7365, 
    TOX=1.6e-8, 
    RS=10, 
    RB=10, 
    CJSW=1.376e-15, 
    GAMMA=0.37, 
    KP=40e-6, 
    PHI=0.6, 
    VTO=1, 
    CGBO=2e-8, 
    CGDO=3.227e-8, 
    CGSO=3.227e-8, 
    AD=1e-12, 
    AS=1e-12, 
    PD=1e-6, 
    PS=1e-6);
  parts.breakout.Spice2MOS1P P1(
    CJ=0.0004138, 
    L=2e-6, 
    LAMBDA=0.01525, 
    LD=1.063e-7, 
    MJSW=0.5, 
    PB=0.7485, 
    TOX=1.6e-8, 
    W=20e-6, 
    GAMMA=0.4, 
    KP=16e-6, 
    PHI=0.6, 
    VTO=-1, 
    CGBO=2e-8, 
    CGDO=2.248e-8, 
    CGSO=2.28e-8, 
    CJSW=1.004e-8, 
    FC=0.5, 
    IS=1e-14, 
    MJ=0.5, 
    RD=10, 
    RS=10, 
    RB=10, 
    RG=10, 
    AD=1e-12, 
    AS=1e-12, 
    PD=1e-6, 
    PS=1e-6);
  parts.breakout.Spice2MOS1 N2(
    L=2e-6, 
    W=4e-6, 
    CJ=0.0003002, 
    LAMBDA=0.01302, 
    LD=1.526e-7, 
    MJ=0.5, 
    MJSW=0.5, 
    PB=0.7365, 
    TOX=1.6e-8, 
    RS=10, 
    RB=10, 
    CJSW=1.376e-15, 
    GAMMA=0.37, 
    KP=40e-6, 
    PHI=0.6, 
    VTO=1, 
    CGBO=2e-8, 
    CGDO=3.227e-8, 
    CGSO=3.227e-8, 
    FC=0.5, 
    IS=1e-14, 
    RD=10, 
    RG=10, 
    AD=1e-12, 
    AS=1e-12, 
    PD=1e-6, 
    PS=1e-6);
  parts.breakout.Spice2MOS1P P2(
    CJ=0.0004138, 
    L=2e-6, 
    LAMBDA=0.01525, 
    LD=1.063e-7, 
    MJSW=0.5, 
    PB=0.7485, 
    TOX=1.6e-8, 
    W=20e-6, 
    GAMMA=0.4, 
    KP=16e-6, 
    PHI=0.6, 
    VTO=-1, 
    CGBO=2e-8, 
    CGDO=2.248e-8, 
    CGSO=2.28e-8, 
    CJSW=1.004e-8, 
    AD=1e-12, 
    AS=1e-12, 
    PD=1e-6, 
    PS=1e-6);
  parts.breakout.Ground Ground4;
  parts.breakout.Ground Ground5;
  parts.source.VCONST VDD(
    OFF=5, 
    DC_VALUE=5, 
    AC_MAG=0);
equation 
  connect(V1.p, N1.g);
  connect(V2.n, Ground2.p);
  connect(N1.d, N2.s);
  connect(N1.s, N1.b);
  connect(P2.d, N2.d);
  connect(P1.s, P2.s);
  connect(P1.s, P1.b);
  connect(P2.s, P2.b);
  connect(P2.g, N2.g);
  connect(P1.g, N1.g);
  connect(N1.s, Ground1.p);
  connect(P1.d, P2.d);
  connect(V2.p, N2.g);
  connect(V1.n, Ground3.p);
  connect(N2.b, Ground5.p);
  connect(VDD.n, Ground4.p);
  connect(VDD.p, P2.s);
end schematic;

SPICELib.tutorial.nandcmos.TRAN

Information

Please, see SPICELib.tutorial.nandcmos documentation

Modelica definition

model TRAN 
  analyses.TRAN TRAN1(
    LogResults=0, 
    redeclare model Circuit = schematic, 
    TimeScale=1e-7, 
    SKIPBP=false, 
    TSTOP=2e-6);
end TRAN;

HTML-documentation generated by Dymola Tue Oct 14 18:26:42 2003 .