Importing RF Device Models

From Emagtech Wiki
Jump to: navigation, search

Multiport Network device, i.e. one-ports, two-ports, three-ports and four-ports, are all modeled based on their frequency-domain S-parameters. Most active and passive RF devices can be modeled as multipart networks. For example, RF diodes can be modeled as one-ports, while RF transistors (BJTs, JFETs, MOSFETs, and MESFETs) can be modeled as two-ports. Many semiconductor manufacturers publish S-parameter data sets for their RF devices. The manufacturer data sheets usually contain S-parameters in Mag/Phase format tabulated as a function of frequency expressed in GHz. On the other hand, you can model many passive devices such as filters, directional couplers, hybrids, etc. as multiport structures using full-wave electromagnetic simulators like EM.Cube. The port characteristics of such devices are typically written into data files as a function of frequency. A particular case of interest is transmission line components with complex geometries or material composition, for which RF.Spice does not provide any database models. as an example, consider the case of a "Finline" transmission line. In a finlike-based circuit, you may need one of more of the following general transmission line components:

  • Open End
  • Bend (right-angled or mitered)
  • Step Junction
  • Tee Junction (symmetric or asymmetric, possibly with a notch)
  • Cross Junction (symmetric or asymmetric)


RF. Spice currently does not provide any models for finline components. However, you can use EM.Cube to analyze various finline structures over a frequency range of interest and generate S-parameter data sets for them.


RF.Spice allows you to import S-parameter-based models of RF devices from text files. Before describing how to import S-parameter data files, let us first discuss the format of the data files in more detail. S-parameter data files must have a ".TXT" file extension. These files must start with a ".model", a ".symbol" statement, and a format statement starting with the character "#". The model text file can have any number of comment lines at the beginning of the file or elsewhere. Comment lines are preceded by "*" or "!". All the text after these characters on the rest of the line will be ignored.


Format:


.model <model_name>

.symbol <symbol_name>

#<frequency_units>   s   <complex_data_format>   r   <reference_impedance_value>

freq     s11 s21 s31 ...     s12 s22 s32 ...     s13 s23 s33 ...


Example:


! This is an example of an RF BJT model based on measured S-parameters.

.model MyNewRFBJT

.symbol bjt_npn

#ghz   s   ma   r   50

! GHz   MAG   ANG   MAG   ANG   MAG   ANG   MAG   ANG

0.500   0.6943   -122.1   4.977   105.7   0.0901   33.0   0.6170   -37.8

1.000   0.6470   -169.7   2.820   76.8   0.0975   23.3   0.4862   -45.5

1.500   0.6586   162.9   1.959   57.6   0.0978   25.6   0.4468   -54.5

2.000   0.6854   142.0   1.481   41.5   0.1055   32.2   0.4315   -65.1

2.500   0.7070   128.1   1.246   30.1   0.1175   37.7   0.4261   -75.5

3.000   0.7449   110.9   0.985   15.5   0.1475   41.9   0.4218   -93.3


The model statement specifies the name of your RF device model, in this case, MyNewRFBJT. The symbol statement determines the device type and schematic symbol. The symbol_name can only be one of the choice given in the table below. The frequency units can be hz, khz, mhz or ghz. "s" implies the s-parameters. If the complex_data_format is left blank, the S-parameters are interpreted to have Mag/Phase format, with the magnitude on a linear scale and phase expressed in degrees. The other options for complex_data_format are "ma" for magnitude expressed in dB, or "ri" for Real/Imag format. The last part specifies the reference impedance value, which must come after letter "r". In the above example, the reference impedance is 50 Ohms.


Device Type Symbol Name Model Type Schematic Symbol
RF Capacitor capacitor one-port G6a.png
RF Inductor inductor one-port G7a.png
RF Diode diode one-port G9.png
RF BJT bjt_npn_2port
bjt_pnp_2port
two-port G11A.png
RF JFET jfet_n
jfet_p
two-port G12.png
RF MOSFET mosfet_n
mosfet_p
two-port G13a.png
RF MESFET mesfet_n
mesfet_p
two-port G14.png
One-Port one-port one-port G60.png
Two-Port two-port two-port G61.png
Three-Port three-port three-port G62.png
Four-Port four-port four-port G63.png
Open End open_end one-port G64.png
Bend bend_junction two-port G65.png
Step Junction step_junction two-port G66.png
Tee Junction tee_junction three-port G67.png
Cross Junction cross_junction four-port G68.png


Using Device Editor for Importing S-Parameter Data

The Device Editor of RF. Spice has an additional RF Menu that lets you import S-parameter text files in a variety of ways. There are three menu items for this purpose:

  • Import S-Parameter Model from Text File...
  • Create New Generic Multiport from S-Parameter Text File...
  • Create New RF Device from S-Parameter Text File...
  • Create New Generic T-Line Discontinuity from S-Parameter Text File...


The first item in the above list simply lets you import an S-parameter ".TXT" file and saves it as a simulation model in RF.Spice's parts database. You can use this model later to build a new device or share it among several devices. The next three items in the above list create new devices complete with simulation models and schematic symbols. The newly create devices are permanently stored in your RF.Spice parts database and can be used as new parts in your RF circuits. For example, an imported RF BJT device has the same BJT symbol with the same pin map as the other BJT devices of B2.Spice A/D. The main difference is that instead of a technology process models or a Netlist subcircuit model, the RF BJT is modeled by its imported, measured S-parameters. In a similar manner, you can import Multiport Network devices or T-Line Discontinuity models from S-parameter text files that are generated at the end of full-wave simulations of such structures using an electromagnetic modeling tool like EM.Cube

 

Network Analysis of RF Circuits   Larr.png   Back to RF.Spice Wiki Main Page   Rarr.png   List of RF.Spice Keyboard Shortcuts