Resistor (Semiconductor) Model

Old Content - visit altium.com/documentation

Modified by Admin on Sep 13, 2017

Model Kind

General

Model Sub-Kind

Resistor(Semiconductor)

SPICE Prefix

SPICE Netlist Template Format

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.

Value	value for the resistance (in Ohms).
Length	length of the resistor (in meters).
Width	width of the resistor (in meters). (Default = 1e-6).
Temperature	temperature at which the device is to operate (in Degrees Celsius). (Default = 27°C).

Parameters (definable within model file)

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

TC1	first order temperature coefficient (in Ohms/°C). (Default = 0).
TC2	second order temperature coefficient (in Ohms/°C ² ). (Default = 0).
RSH	sheet resistance (in Ohms).
DEFW	default width (in meters). - this value will be overridden by a value entered for Width in the Sim Model dialog.
NARROW	narrowing due to side etching (in meters). (Default = 0).
TNOM	parameter measurement temperature (in °C) - If no value is specified, the default value assigned to TNOM on the SPICE Options page of the Analyses Setup dialog will be used (Default = 27).

Notes

You can specify either a direct value for the resistance OR enter values for the resistors' length and width. In the case of the latter, a value for the resistance will be calculated, in conjunction with parameter information stored in the model.
The equation used to calculate the resistance from geometric data is:
R = RSH * ((L - NARROW) / (W - NARROW))
If a direct value for resistance is not specified, the model name and length must be supplied in order for the geometric-based resistance value to be calculated. If either the length or sheet resistance (RSH) is not specified, the default resistance value of 1K will be used and a warning will be generated.
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.
Entering a direct value for the resistance will override the geometric definition.
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 resistor in the above image, with the following characteristics:

Pin1 is connected to net Input
Pin2 is connected to net Inv
Designator is RIn
The linked simulation model file is RES.mdl.

If a value for the resistance was entered directly, say 10K, 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: RIn Input Inv RES 10K

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

Length = 10e-3
Width = 4e-3
Temperature = 24.

The entry in the netlist would be:

*Schematic Netlist: RIn INPUT INV RES L=10e-3 W=4e-3 TEMP=24

As long as a value for the sheet resistance (RSH) has been defined in the model file (RES.mdl), the value for the resistance will be calculated accurately from the geometric data given.

PSpice Support

The existing Spice3f5 model for the Resistor (Semiconductor) device has been enhanced to support the general PSpice model form:

R<name> <(+) node> <(-) node> [model name] <value> [TC = <TC1> [,<TC2>]]

A PSpice model of this type should be linked to a schematic component using a model file. Simply specify the model in a model file (*.mdl) then, in the Sim Model dialog, set the Model Kind to General and the Model Sub-Kind to Generic Editor. The Netlist Template Format should then be entered as follows:

@DESIGNATOR %1 %2 &MODEL &VALUE ?TC1/TC=@TC1?TC2|, @TC2| /

Although you could use the Spice3f5 Resistor (Semiconductor) model - as this model type allows use of a linked model file - specification of the netlist format for a PSpice Resistor model using the Generic Editor allows you to make use of the additional PSpice parameters ([TC = <TC1> [,<TC2>]]).

For the circuit to be parsed correctly, ensure that the Spice Prefix field is set to R.

In the Model Name field, enter the name specified for the model in the model file. Use the options in the Model Location region of the dialog to point to the required file. Click on the Model File tab to view the content of the model file.

The following additional model parameters are supported and can be entered into a linked model file (*.mdl) for the device:

R	resistance multiplier. (Default = 1).
TC1	linear temperature coefficient (in ˚C-1). (Default = 0).
TC2	quadratic temperature coefficient (in ˚C-2). (Default = 0).
TCE	exponential temperature coefficient (in %/˚C). (Default = 0).

Values for TC1 and TC2 can be entered on the Parameters tab of the Sim Model dialog. Where a parameter has an indicated default, that default will be used if no value is specifically entered - either on the Parameters tab or in the linked model file.

The format for the PSpice model file is:

.MODEL ModelName RES(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.

The following parameters - common to most devices in PSpice - are not supported:
T_ABS
T_MEASURED
T_REL_GLOBAL
T_REL_LOCAL.

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