GSRC - Voltage-Controlled Current Source Model

Model Kind

Current Source

Model Sub-Kind

Voltage-Controlled

SPICE Prefix

G

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

i = gv

where,

g is the transconductance.

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

Examples

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

• Pin1 (positive controlling node) is connected to net N1
• Pin2 (negative controlling node) is connected to net N6
• Pin3 (positive output node) is connected to net GND
• Pin4 (negative output node) is connected to net N5
• Designator is GCM
• Gain = 2.574E-9

The entry in the SPICE netlist would be:

*Schematic Netlist: 
GCM 0 N5 N1 N6 2.574E-9

PSpice Support

1. The following general PSpice model forms are supported:

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