Diode Model

Old Content - visit altium.com/documentation

Modified by Phil Loughhead on Mar 4, 2014

Model Kind

General

Model Sub-Kind

Diode

SPICE Prefix

SPICE Netlist Template Format

@DESIGNATOR %1 %2 @MODEL &"AREA FACTOR" &"STARTING CONDITION" ?"INITIAL VOLTAGE"|IC=@"INITIAL VOLTAGE"| ?TEMPERATURE|TEMP=@TEMPERATURE|

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.

Area Factor	specifies the number of equivalent parallel devices of the specified model. This setting affects a number of parameters in the model.
Starting Condition	set to OFF to set diode voltage to zero during operating point analysis. Can be useful as an aid in convergence.
Initial Voltage	time-zero voltage across the diode (in Volts).
Temperature	temperature at which the device is to operate (in Degrees Celsius). (Default = 27).

Parameters (definable within model file)

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

IS	saturation current (in Amps). (Default = 1.0e-14).
RS	ohmic resistance (in Ohms). (Default = 0).
N	emission coefficient (Default = 1).
TT	transit-time (in seconds). (Default = 0).
CJO	zero-bias junction capacitance (in Farads). (Default = 0).
VJ	junction potential (in Volts). (Default = 1).
M	grading coefficient (Default = 0.5).
EG	activation energy (in eV). (Default = 1.11).
XTI	saturation-current temp exp. (Default = 3.0).
KF	flicker noise coefficient (Default = 0)
AF	flicker noise exponent (Default = 1).
FC	coefficient for forward-bias depletion capacitance formula (Default = 0.5).
BV	reverse breakdown voltage (in Volts). (Default = infinite).
IBV	current at breakdown voltage (in Amps). (Default = 1.0e-3).
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

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.
The Area Factor affects the following three model parameters:

saturation current (IS)
ohmic resistance (RS)
zero-bias junction capacitance (CJO)

If the Area Factor is omitted, a value of 1.0 is assumed.
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.
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 diode in the above image, with the following characteristics:

Pin1 (anode) is connected to net VIN
Pin2 (cathode) is connected to net Vhw
Designator is D1
The linked simulation model file is 1N4002.mdl

If no values are entered for the parameters in the Sim Model dialog, the entries in the SPICE netlist would be:

*Schematic Netlist: D1 VIN VHW 1N4002 . . *Models and Subcircuit: .MODEL 1N4002 D(IS=2.55E-9 RS=0.042 N=1.75 TT=5.76E-6 CJO=1.85E-11 VJ=0.75 + M=0.333 BV=100 IBV=1E-5 )

and the SPICE engine would use the indicated parameter information defined in the model file, along with default parameter values inherent to the model for those parameters not specified in the file.
If the following parameter values were specified on the Parameters tab of the Sim Model dialog:

Area Factor = 3
Initial Voltage = 2
Temperature = 22

then the entries in the SPICE netlist would be:

*Schematic Netlist: D1 VIN VHW 1N4002 3 IC=2 TEMP=22 . . *Models and Subcircuit: .MODEL 1N4002 D(IS=2.55E-9 RS=0.042 N=1.75 TT=5.76E-6 CJO=1.85E-11 VJ=0.75 + M=0.333 BV=100 IBV=1E-5 )

In this case, the SPICE engine would use this information, in conjunction with the indicated parameters defined in the model file (and any defaults for parameters not specified).

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:

IBVL	low-level reverse breakdown knee current (in Amps). (Default = 0).
IKF	high-injection knee current (in Amps). (Default = infinite).
ISR	recombination current parameter (in Amps). (Default = 0).
NBV	reverse breakdown ideality factor. (Default = 1).
NBVL	low-level reverse breakdown ideality factor. (Default = 1).
NR	emission coefficient for isr. (Default = 2).
TBV1	bv temperature coefficient - linear (in ˚C-1). (Default = 0).
TBV2	bv temperature coefficient - quadratic (in ˚C-2). (Default = 0).
TIKF	ikf temperature coefficient - linear (in ˚C-1). (Default = 0).
TRS1	rs temperature coefficient - linear (in ˚C-1). (Default = 0).
TRS2	rs temperature coefficient - quadratic (in ˚C-2). (Default = 0).

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 D(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 diode model in a simulation, refer to the example project Diode.PrjPCB.