SPICELib.tutorial.circ1

Example 1 of SPICELib tutorial

Information

Example 1

The modeling of the circuit shown in Figure 1 is discussed, and OP, AC sweep and transient analyses are carried out.
The results of the analysis using SPICELib are shown, together with the results obtained using OrCAD PSpice.

Figure 1. Full wave Rectifier.

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): circ1.
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 a resistor, a capacitor, an inductor, a diode and a 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 listed below as shown in Figure 2.
- SPICELib.parts.breakout.Ground
- SPICELib.parts.breakout.Rbreak
- SPICELib.parts.breakout.Cbreak
- SPICELib.parts.breakout.Lbreak
- SPICELib.parts.breakout.PSPICE_diode
- SPICELib.parts.source.VSIN
Figure 2. Inserting the circuit components.
Connect the circuit parts as shown in Figure 1.
Enter the parameter values of the circuit components. See Figures 3-6.
The Boolean parameter HIDDEN_COMPONENT controls the log of the device variables (see SPICELib.analyses package documentation). The circuit's diodes have the same parameters. Therefore, we only show D1's diode parameters.
Figure 3. Voltage source parameters.

Figure 4. R parameters.

Figure 5. C parameters.

Figure 6. D1 parameters.
Save the Schematic model.

Bias Point Analysis (OP)

Create a new model, circ1_OP, and insert it in circ1 package (see Figure 7).
Figure 7. Inserting circ1_OP in circ1 package.
Drag an SPICELib.analyses.OP model into the circ1_OP model (see Figure 8).
Figure 8. Inserting circ1_OP in circ1 package.
Enter the OP analysis parameters (see Figure 9). The meaning of the analysis parameters is discussed in the SPICELib.analyses.OP model documentation. The SOLVE_STATIC parameter determines which of the four algorithms to use for the bias point calculation. The four cases are discussed next.

Figure 9. OP analysis parameters.

STATIC MODEL ITERATION (SOLVE_STATIC := 0)

Set SOLVE_STATIC value equals to zero, as it is shown in Figure 9.
Change to the Dymola Simulation window and translate the model circ1.circ1_OP
Experiment setup. Give to the Stop time parameter an arbitratily large value (Dymola window option: "Simulation/Setup/Stop time"), for example, Stop time equals 10.
Run the simulation. Once it is finished, dslog.txt file contains the analysis results (see Figure 10). Variables of interest are signaled with arrows.
Figure 10. dslog.txt file fragment. SOLVE_STATIC:=0, LOG_RESULTS:=0

STATIC MODEL RAMPING (SOLVE_STATIC := 1)

Set SOLVE_STATIC value equals to one.
Change to the Dymola Simulation window and translate the model circ1.circ1_OP
Experiment setup. Give to the Stop time parameter an arbitratily large value (Dymola window option: "Simulation/Setup/Stop time"), for example, Stop time equals 10.
Run the simulation. Once it is finished, dslog.txt file contains the analysis results (see Figure 11).
Figure 11. dslog.txt file fragment. SOLVE_STATIC:=1, LOG_RESULTS:=0

GMIN STEPPING (SOLVE_STATIC := 2)

Set SOLVE_STATIC value equals to two.
Change to the Dymola Simulation window and translate the model circ1.circ1_OP
Experiment setup. Give to the Stop time parameter an arbitratily large value (Dymola window option: "Simulation/Setup/Stop time"), for example, Stop time equals 10.
Run the simulation. Once it is finished, dslog.txt file contains the analysis results (see Figure 12).
Figure 13. dslog.txt file fragment. SOLVE_STATIC:=2, LOG_RESULTS:=0

DYNAMIC MODEL RAMPING (SOLVE_STATIC := 3)

Set SOLVE_STATIC value equals to three.
Change to the Dymola Simulation window and translate the model circ1.circ1_OP
Experiment setup. Give to the Stop time parameter an arbitratily large value (Dymola window option: "Simulation/Setup/Stop time"), for example, Stop time equals 10.
Run the simulation. Once it is finished, dslog.txt file contains the analysis results (see Figure 13).
Figure 13. dslog.txt file fragment. SOLVE_STATIC:=3, LOG_RESULTS:=0

BIAS POINT ANALYSIS SIMULATED WITH ORCAD PSPICE

Figure 14.

OP calculate with OrCAD PSPICE

AC sweep analysis (AC)

Create a new model, circ1_AC, and insert it in circ1 package (see Figure 15).
Figure 15. Inserting circ1_AC in circ1 package.
Drag an SPICELib.analyses.AC model into the circ1_AC model (see Figure 16).
Figure 16. Inserting circ1_AC in circ1 package.
Enter the AC analysis parameters (see Figure 17). The meaning of the analysis parameters is discussed in the SPICELib.analyses.AC model documentation.

Figure 17. AC analysis parameters.
Change to the Dymola Simulation window and translate the model circ1.circ1_AC
Experiment setup. Give to the Stop time parameter an arbitratily large value (Dymola window option: "Simulation/Setup/Stop time"), for example, Stop time equals 10.
Run the simulation. Once it is finished, dslog.txt file contains the analysis results.

AC SWEEP ANALYSIS SIMULATED WITH ORCAD PSPICE AND SPICELIB

Figure 18. AC sweep analysis simulated with ORCAD and SPICELib and errors.

Transient (time) analysis (TRAN)

Create a new model, circ1_TRAN, and insert it in circ1 package (see Figure 19).
Figure 19. Inserting circ1_TRAN in circ1 package.
Drag an SPICELib.analyses.TRAN model into the circ1_TRAN model (see Figure 20).
Figure 20. Inserting circ1_TRAN in circ1 package.
Enter the TRAN analysis parameters (see Figure 21). 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 21. TRAN analysis parameters.

TRANSIENT ANALYSIS SIMULATED WITH SPICELIB AND ORCAD PSPICE

Figure 22. Transient analysis and error.

Name Description

schematic

circ1_OP

circ1_AC

circ1_TRAN

Name	Description
schematic
circ1_OP
circ1_AC
circ1_TRAN

SPICELib.tutorial.circ1.schematic

Information

Please, see SPICELib.tutorial.circ1 documentation

Modelica definition

partial model schematic 
  parts.breakout.Rbreak R(R=1000);
  parts.breakout.Ground Ground1;
  parts.source.VSIN V1(
    FREQ=50, 
    AMPL=5, 
    AC_MAG=1, 
    DC_VALUE=0.7, 
    OFF=2);
  src.BREAKOUT.PSPICE_diode D1(
    IS=14.11e-9, 
    RS=33.89e-3, 
    N=1.984, 
    VJ=0.3905, 
    M=0.2762, 
    BV=100.1, 
    IKF=94.81, 
    ISR=100e-12, 
    NR=2, 
    IBV=10, 
    CJ0=51.17e-12, 
    TT=4.761e-6);
  parts.breakout.PSPICE_diode D3(
    IS=14.11e-9, 
    RS=33.89e-3, 
    N=1.984, 
    VJ=0.3905, 
    M=0.2762, 
    BV=100.1, 
    IKF=94.81, 
    ISR=100e-12, 
    NR=2, 
    IBV=10, 
    CJ0=51.17e-12, 
    TT=4.761e-6);
  parts.breakout.PSPICE_diode D2(
    IS=14.11e-9, 
    RS=33.89e-3, 
    N=1.984, 
    VJ=0.3905, 
    M=0.2762, 
    BV=100.1, 
    IKF=94.81, 
    ISR=100e-12, 
    NR=2, 
    IBV=10, 
    CJ0=51.17e-12, 
    TT=4.761e-6);
  parts.breakout.PSPICE_diode D4(
    IS=14.11e-9, 
    RS=33.89e-3, 
    N=1.984, 
    VJ=0.3905, 
    M=0.2762, 
    BV=100.1, 
    IKF=94.81, 
    ISR=100e-12, 
    NR=2, 
    IBV=10, 
    CJ0=51.17e-12, 
    TT=4.761e-6);
  src.BREAKOUT.Cbreak C(C=100e-6);
equation 
  connect(R.n, Ground1.p);
  connect(V1.p, D2.p);
  connect(D1.n, D2.p);
  connect(D2.n, R.p);
  connect(D4.n, R.p);
  connect(D1.p, D3.p);
  connect(D3.p, Ground1.p);
  connect(V1.n, D4.p);
  connect(D3.n, D4.p);
  connect(R.p, C.p);
  connect(Ground1.p, C.n);
end schematic;

SPICELib.tutorial.circ1.circ1_OP

Information

Please, see SPICELib.tutorial.circ1 documentation

Modelica definition

model circ1_OP 
  analyses.OP OP(
    redeclare model Circuit = schematic, 
    LogResults=0, 
    TimeScale=0.1, 
    SOLVE_STATIC=0);
end circ1_OP;

SPICELib.tutorial.circ1.circ1_AC

Information

Please, see SPICELib.tutorial.circ1 documentation

Modelica definition

model circ1_AC 
  analyses.AC AC(
    LogResults=0, 
    redeclare model Circuit = schematic, 
    SOLVE_STATIC=0, 
    TYPE_AC_SWEEP=1, 
    END_FREQUENCY=1000, 
    TimeScale=0.01, 
    START_FREQUENCY=1, 
    POINTS_NUMBER=100);
end circ1_AC;

SPICELib.tutorial.circ1.circ1_TRAN

Information

Please, see SPICELib.tutorial.circ1 documentation

Modelica definition

model circ1_TRAN 
  analyses.TRAN TRAN(
    LogResults=0, 
    SOLVE_STATIC=0, 
    redeclare model Circuit = schematic, 
    TimeScale=0.01, 
    TSTOP=0.05, 
    SKIPBP=false);
end circ1_TRAN;

HTML-documentation generated by Dymola Tue Oct 14 18:26:39 2003 .