HSRC - Current-Controlled Voltage Source Model

Model Kind

Voltage Source

Model Sub-Kind

Current-Controlled

SPICE Prefix

H

SPICE Netlist Template Format

V@DESIGNATOR %1 %2 0V
@DESIGNATOR %3 %4 V@DESIGNATOR @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 current at the input terminals, dependant on the transresistance of the source.
2. The current-controlled voltage source actually implements two individual devices, as can be seen from the Netlist template. The first is a 0V voltage source, which acts as an ammeter, to measure the current input and then the actual current-controlled voltage source that references it. The direction of positive controlling current flow is from the positive node, through the source to the negative node of the 0V voltage source.
3. The characteristic equation for this source is:

v = hi

where,

h is the transresistance.

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

Examples

Consider the current-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 HLIM
• Gain = 1k.

The entry in the SPICE netlist would be:

*Schematic Netlist: 
VHLIM N7 N10 0V
HLIM N11 0 VHLIM 1k

PSpice Support

1. The following general PSpice model form is supported:

• H<name> <(+) node> <(-) node> POLY(<value>) <controlling V device name> < <polynomial coefficient value> >

2. This device does not support linked model files. The netlist format for a PSpice model in the above form 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 H.
4. The following example generic netlist template format could be used for this model type:

@DESIGNATOR %1 %2 POLY (@dimension) @ControlSource @coeffs

5. The values for the dimension, ControlSource and coeffs parameters are entered on the Parameters tab of the Sim Model dialog.