Modelica.Electrical.Spice3.Basic

Information

This Package contains the basic components of the SPICE3 models. The first letter of the

name of the component shows the SPICE name, e.g., R_Resistor: R is the SPICE-name of the component

resistor which is used in SPICE-Netlists.

Package Content

Name	Description
Ground	Ground node
R_Resistor	Ideal linear electrical resistor
C_Capacitor	Ideal linear electrical capacitor
L_Inductor	Ideal linear electrical inductor
K_CoupledInductors	Inductive coupling via coupling factor K
E_VCV	Linear voltage-controlled voltage source
G_VCC	Linear voltage-controlled current source
H_CCV	Linear current-controlled voltage source
F_CCC	Linear current-controlled current source

Modelica.Electrical.Spice3.Basic.Ground

Information

Ground of an electrical circuit. The potential at the ground node is zero. Every electrical circuit has to contain at least one ground object.

SPICE does not have an element for the ground node (mass). In SPICE netlists the ground is specified by the node number 0. This Modelica SPICE library demands to describe the ground node by this ground element.

Connectors

Name	Description
p	Ground pin

Modelica.Electrical.Spice3.Basic.R_Resistor

Information

The linear resistor connects the branch voltage v with the branch current i by i*R = v. The Resistance R is allowed to be positive, zero, or negative.

Parameters

Name	Description
R	Resistance [Ohm]

Connectors

Name	Description
p	Positive pin (potential p.v > n.v for positive voltage drop v)
n	Negative pin

Modelica.Electrical.Spice3.Basic.C_Capacitor

Information

The linear capacitor connects the branch voltage v with the branch current i by i = C * dv/dt. The Capacitance C is allowed to be positive, zero, or negative.

Parameters

Name	Description
C	Capacitance [F]
IC	Initial value [V]
UIC	Use initial conditions: true, if initial condition is used

Connectors

Name	Description
p	Positive pin (potential p.v > n.v for positive voltage drop v)
n	Negative pin

Modelica.Electrical.Spice3.Basic.L_Inductor

Information

The linear inductor connects the branch voltage v with the branch current i by v = L * di/dt. The inductance L is allowed to be positive, zero, or negative.

Parameters

Name	Description
L	Inductance [H]
IC	Initial value; used, if UIC is true [A]
UIC	Use initial conditions

Connectors

Name	Description
p	Positive pin (potential p.v > n.v for positive voltage drop v)
n	Negative pin
ICP	Pin to couple inductances via K

Modelica.Electrical.Spice3.Basic.K_CoupledInductors

Information

K_CoupledInductors is a component that allows the coupling of two inductors. K is the coefficient of coupling which must be greater than or equal to zero and less than one.

The usage is demonstrated in the example CoupledInductors.

Parameters

Name	Description
k	Coupling Factor

Connectors

Name	Description
inductiveCouplePin1	Couple pin for inductances
inductiveCouplePin2	Couple pin for inductances

Modelica.Electrical.Spice3.Basic.E_VCV

Information

The linear voltage-controlled voltage source is a TwoPort. The right port voltage at pin p2 (=p2.v) is controlled by the left port voltage at pin p1 (=p1.v) via

    p2.v = p1.v * gain.

The left port current is zero. Any voltage gain can be chosen.

    Ename N+ N- NC+ NC- VALUE

is translated to Modelica:

    Ename -> Spice3.Basic.E_VCV Ename
    (Ename is the name of the Modelica instance)
    N+ -> p2.v
    N- -> n2.v
    NC+ -> p1.v
    NC- -> n1.v
    VALUE -> gain

Parameters

Name	Description
gain	Voltage gain

Connectors

Name	Description
p1	Positive pin of the controlling port
n1	Negative pin of the controlling port
p2	Positive pin of the controlled port
n2	Negative pin of the controlled port

Modelica.Electrical.Spice3.Basic.G_VCC

Information

The linear voltage-controlled current source is a TwoPort. The right port current at pin p2 (=p2.i) is controlled by the left port voltage at pin p1 (p1.v) via

    p2.i = p1.v * transConductance.

The left port current is zero. Any transConductance can be chosen.

    Gname N+ N- NC+ NC- VALUE

is translated to Modelica:

    Gname -> Spice3.Basic.G_VCC Gname
    (Gname is the name of the Modelica instance)
    N+ -> p2.i
    N- -> n2.i
    NC+ -> p1 .v
    NC- -> n1.v
    VALUE -> transConductance

Parameters

Name	Description
transConductance	Transconductance [S]

Connectors

Name	Description
p1	Positive pin of the controlling port
n1	Negative pin of the controlling port
p2	Positive pin of the controlled port
n2	Negative pin of the controlled port

Modelica.Electrical.Spice3.Basic.H_CCV

Information

The linear current-controlled voltage source is a TwoPort. The "right" port voltage at pin 2 (=p2.v) is controlled by the "left" port current at pin p1(=p1.i) via

    p2.v = p1.i * transResistance.

The controlling port voltage is zero. Any transResistance can be chosen.

The corresponding SPICE description

    Hname N+ N- VNAM VALUE

is translated to Modelica:

    Hname -> Spice3.Basic.H_CCV Hname
    (Hname is the name of the Modelica instance)
    N+ -> p2.v
    N- -> n2.v  

The voltage source VNAM has the two nodes NV+ and NV-:

                   VNAM VN+ VN- VALUE_V

The current through VNAM hast to be led through the CCV.

Therefore VNAM has to be disconnected and an additional

node NV_AD has to be added.

    NV_AD -> p1.i
    NV- -> n1.i

On this way the current, that flows through the voltage source VNAM, flows through the CCV.

    VALUE -> transResistance 

Parameters

Name	Description
transResistance	Transresistance [Ohm]

Connectors

Name	Description
p1	Positive pin of the controlling port
n1	Negative pin of the controlling port
p2	Positive pin of the controlled port
n2	Negative pin of the controlled port

Modelica.Electrical.Spice3.Basic.F_CCC

Information

The linear current-controlled current source is a TwoPort. The "right" port current at pin 2 (=p2.i) is controlled by the "left" port current at pin p1(=p1.i) via

    p2.i = p1.i * gain.

The controlling port voltage is zero. Any current gain can be chosen.

The corresponding SPICE description

    Fname N+ N- VNAM VALUE

is translated to Modelica:

    Fname -> Spice3.Basic.F_CCC Fname
    (Fname is the name of the Modelica instance)
    N+ -> p2.i
    N- -> n2.i  

The voltage source VNAM has the two nodes NV+ and NV-:

                   VNAM NV+ NV- VALUE_V

The current through VNAM hast to be led through the CCC.

Therefore VNAM has to be disconnected and an additional

node NV_AD has to be added.

    NV_AD -> p1.i
    NV- -> n1.i

On this way the current, that flows through the voltage source VNAM, flows through the CCC.

    VALUE -> gain 

Parameters

Name	Description
gain	Current gain

Connectors

Name	Description
p1	Positive pin of the controlling port
n1	Negative pin of the controlling port
p2	Positive pin of the controlled port
n2	Negative pin of the controlled port