Capacitor (Semiconductor) Model

Model Kind

General

Model Sub-Kind

Capacitor(Semiconductor)

SPICE Prefix

C

SPICE Netlist Template Format

@DESIGNATOR %1 %2 &VALUE &MODEL ?LENGTH|L=@LENGTH| ?WIDTH|W=@WIDTH| ?"INITIAL VOLTAGE"|IC=@"INITIAL VOLTAGE"|

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.

Parameters (definable within model file)

The following is a list of process-related parameters that can be stored in the associated model file:

Notes

1. The value for the Initial Voltage only applies if the Use Initial Conditions option is enabled on the Transient/Fourier Analysis Setup page of the Analyses Setup dialog.
2. You can specify either a direct value for the capacitance OR enter values for the capacitors' length and width. In the case of the latter, a value for the capacitance will be calculated, in conjunction with parameter information stored in the model.
3. The equation used to calculate the capacitance from geometric data is:

CAP = CJ(LENGTH - NARROW)(WIDTH - NARROW) + 2CJSW(LENGTH + WIDTH - 2*NARROW)

4. If a direct value for capacitance is not specified, the model name and length must be supplied in order for the geometric-based capacitance value to be calculated.
5. The link to the required model file (*.mdl) is specified on the Model Kind tab of the Sim Model dialog. The Model Name is used in the netlist to reference this file.
6. Either the direct capacitance value OR the geometric data used to calculate it can be entered, but not both.
7. Where a parameter has an indicated default (as part of the SPICE model definition), that default will be used if no value is specifically entered. The default should be applicable to most simulations. Generally you do not need to change this value.

Examples

Consider the semiconductor capacitor in the above image, with the following characteristics:

• Pin1 is connected to net N1
• Pin2 is connected to net VN
• Designator is C1
• The linked simulation model file is CAP.mdl

If a value for the capacitance was entered directly, say 100 pF, and no other parameters were specified on the Parameters tab of the Sim Model dialog, then the entry in the SPICE netlist would be:

*Schematic Netlist:
C1 N1 VN 100pF CAP

Consider now, instead of entering a direct value for the capacitance, the following parameters were defined in the Sim Model dialog:

• Length = 10u
• Width = 1u

The entry in the netlist would be:

C1 N1 VN CAP L=10u W=1u

The value for the capacitance will be calculated accurately using the geometric data specified and any further parameter definitions in the model file (CAP.mdl).

PSpice Support

To make this device model compatible with PSpice, the following additional model parameters are supported and can be entered into a linked model file (*.mdl) for the device:

Where a parameter has an indicated default, that default will be used if no value is specifically entered.

The format for the PSpice model file is:

.MODEL ModelName CAP(Model Parameters), 

where:

• ModelName is the name of the model, the link to which is specified on the Model Kind tab of the Sim Model dialog. This name is used in the netlist (&MODEL) to reference the required model in the linked model file.
• Model Parameters are a list of supported parameters for the model, entered with values as required.

For an example of using a PSpice-compatible capacitor model in a simulation, refer to the example project Capacitor.PrjPCB.