ESRC - Voltage-Controlled Voltage Source Model

Model Kind

Voltage Source

Model Sub-Kind

Voltage-Controlled

SPICE Prefix

E

SPICE Netlist Template Format

@DESIGNATOR %3 %4 %1 %2 @GAIN

Parameters (definable at component level)

The following component-level parameters are definable for this model type and are listed on the Parameters tab of the Sim Model dialog. To access this dialog, simply double-click on the entry for the simulation model link in the Models region of the Component Properties dialog.

Notes

1. This source produces a voltage at the output terminals that is a linear function of the voltage at the input terminals, dependant on the gain of the source.
2. The characteristic equation for this source is:

v = ev

where,

e is the voltage gain.

3. The simulation-ready voltage controlled voltage source component (ESRC) can be found in the Simulation Sources integrated library (\Library\Simulation\Simulation Sources.IntLib).

Examples

Consider the voltage-controlled voltage source in the above image, with the following characteristics:

• Pin1 (positive controlling node) is connected to net N7
• Pin2 (negative controlling node) is connected to net N10
• Pin3 (positive output node) is connected to net N11
• Pin4 (negative output node) is connected to net GND
• Designator is ELIM
• Gain = 1

The entry in the SPICE netlist would be:

*Schematic Netlist: 
ELIM N11 0 N7 N10 1

PSpice Support

1. The following general PSpice model forms are supported:

• E<name> <(+) node> <(-) node> VALUE = { <expression> }
• E<name> <(+) node> <(-) node> TABLE { <expression> } = < <input value>,<output value> >

• E<name> <() node> <() node> POLY(<value>) < <() controlling node> <() controlling node> > < <polynomial coefficient value> >

2. These devices do not support linked model files. The netlist format for a PSpice model in one of the above forms should be specified using the Generic Editor. In the Sim Model dialog, set the Model Kind to General and the Model Sub-Kind to Generic Editor.
3. For the circuit to be parsed correctly, ensure that the Spice Prefix field is set to E.
4. The following are examples of generic netlist template formats that could be used for these model types.

VALUE model

@DESIGNATOR %1 %2 VALUE = {@EXPR}
The value for the EXPR parameter is entered on the Parameters tab of the Sim Model dialog.

TABLE model

@DESIGNATOR %1 %2 TABLE {@EXPR} = @ROW1 ?ROW2|@ROW2| ?ROW3|@ROW3|
Values for the EXPR and ROW parameters are entered on the Parameters tab of the Sim Model dialog. Any number of ROW parameters can be defined, in the format (<input value>, <output value>).

The netlist format could be entered using the following alternative entry:
@DESIGNATOR %3 %4 TABLE { @EXPR } ( @TABLE )

Values for the EXPR and TABLE parameters are again entered on the Parameters tab of the Sim Model dialog. The value for the TABLE parameter is specified in the form:
(<input1>, <output1>)(<input2>, <output2>)...(<inputn>, <outputn>)

POLY model

@DESIGNATOR %3 %4 POLY (@dimension) (%1, %2) @coeffs
The values for the dimension and coeffs parameters are entered on the Parameters tab of the Sim Model dialog.

• For an example of using a PSpice-compatible expression-based voltage-controlled voltage source in a simulation, refer to the example project EVALUE.PrjPCB.
• For an example of using a PSpice-compatible lookup table-based voltage-controlled voltage source in a simulation, refer to the example project TABLE.PrjPCB.
• For an example of using a PSpice-compatible polynomial-based voltage-controlled voltage source in a simulation, refer to the example project EPOLY.PrjPCB.