LTRA - Lossy Transmission Line Model

Old Content - visit altium.com/documentation

Modified by Phil Loughhead on Mar 4, 2014

Model Kind

Transmission Line

Model Sub-Kind

Lossy

SPICE Prefix

SPICE Netlist Template Format

@DESIGNATOR %1 %2 %3 %4 @MODEL

Parameters (definable at component-level)

It is not possible to pass parameter information directly from the schematic component. The parameters must be defined in the associated model file.

Parameters (definable within model file)

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

R	resistance per unit length (in Ohms/unit). (Default = 0).
L	inductance per unit length (in Henrys/unit). (Default = 0).
G	conductance per unit length (in mhos/unit). (Default = 0).
C	capacitance per unit length (in Farads/unit). (Default = 0).
LEN	length of transmission line.
REL	breakpoint control (in arbitrary units). (Default = 1).
ABS	breakpoint control (in arbitrary units). (Default = 1).
NOSTEPLIMIT	a flag that, when set, will remove the restriction of limiting time-steps to less than the line delay. (Default = not set).
NOCONTROL	a flag that, when set, prevents limiting of the time-step, based on convolution error criteria. (Default = not set).
LININTERP	a flag that, when set, will use linear interpolation instead of the default quadratic interpolation, for calculation of delayed signals. (Default = not set).
MIXEDINTERP	a flag that, when set, uses a metric for determining whether quadratic interpolation is applicable and, if it isn't, uses linear interpolation. (Default = not set).
COMPACTREL	a specific quantity used to control the compaction of past history values used for convolution. By default, this quantity uses the value specified for the relative simulation error tolerance (RELTOL), which is defined on the Spice Options page of the Analyses Setup dialog.
COMPACTABS	a specific quantity used to control the compaction of past history values used for convolution. By default, this quantity uses the value specified for the absolute current error tolerance (ABSTOL), which is defined on the Spice Options page of the Analyses Setup dialog.
TRUNCNR	a flag that, when set, turns on the use of the Newton-Raphson iteration method to determine an appropriate time-step in the time-step control routines. (Default = not set, whereby a trial and error method is used - cutting the previous time-step in half each time).
TRUNCDONTCUT	a flag that, when set, removes the default cutting of the time-step to limit errors in the actual calculation of impulse-response related quantities. (Default = not set).

Notes

The operation of the lossy transmission line model (LTRA) is based on the convolution of the transmission line's impulse responses with its inputs.
The length of the transmission line (LEN) must be specified.
Setting any of the NOCONTROL, NOSTEPLIMIT and TRUNCDONTCUT flags increases simulation speed but may affect the accuracy of the results.
Using larger values for COMPACTREL and COMPACTABS will result in reduced accuracy but greater simulation speed. If defined, these parameters will only be applied if the TRYTOCOMPACT option is enabled on the Spice Options page of the Analyses Setup dialog.
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 in the model file. The default should be applicable to most simulations. Generally you do not need to change this value.
A lossy transmission line with zero loss may be more accurate than the lossless transmission line due to implementation details.
The simulation-ready lossy transmission line component (LTRA) can be found in the Simulation Transmission Line integrated library (\Library\Simulation\Simulation Transmission Line.IntLib).
You can easily create and reference your own model file. To do this copy the file ltra.MDL. Edit this new model file and change the string immediately after the .MODEL statement to be the same as the new file name, then edit the parameters as required. For example, from the existing model file ltra.MDL:

.MODEL LTRA LTRA(R=0.000 L=9.130n C=3.650p LEN=1.000)

You could create a new file, ltra10.MDL:

.MODEL LTRA10 LTRA(R=0.2 L=32n C=13p LEN=10.000)

Examples

Consider the lossy transmission line in the above image, with the following characteristics:

Pin1 (positive node of Port 1) is connected to net IN
Pin2 (negative node of Port 1) is connected to net GND
Pin3 (positive node of Port 2) is connected to net OUT
Pin4 (negative node of Port 2) is connected to net GND
Designator is LTRA1
The linked simulation model file is LTRA.mdl.

The entry in the SPICE netlist would be:

*Schematic Netlist: OLTRA1 IN 0 OUT 0 LTRA . . *Models and Subcircuit: .MODEL LTRA LTRA(R=0.000 L=9.130N C=3.650P LEN=1.000)

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.