//Translations of this page are also available in the following languages:// [[example_hsm.ru|Русский]].

====== Hierarchical SPICE model ======
Example of a hierarchical analog RF SPICE model in the:\\
**''${prefix}/share/doc/geda-gaf/examples/RF_Amp''**\\
directory, where ''${prefix}'' is the installation prefix for gEDA on your
system (usually **''/usr''** or **''/usr/local''**).

<code>This README created 3.31.2003

---------------------  Contents of directories  -----------------------

This directory holds the schematics and associated materials for a
SPICE model of Agilent's MSA-2643 bipolar amp.  The model was obtained
from Agilent's datasheet 5980-2396E.  The directory structure is as
follows:

RF_Amp (base directory)

MSA-2643.sch -- schematic of stuff inside device package (as shown in
p. 7 of datasheet.  Note that I have not included the transmission
lines in this schematic because no value of Z was included in the data
sheet.   (Yes, it's probably 50 ohms, but including them was a
sideshow compared to my main intent: build a hierarchical model of an
RF circuit.)
MSA-2643.cir -- netlisted circuit ready for SPICE simulation.

Q1.sch -- schematic model of Q1 MSA-26 transistor shown on p. 8 of datasheet.
Q1.cir -- netlisted circuit holding .SUBCKT model of Q1.

Q2.sch -- schematic model of Q2 MSA-26 transistor shown on p. 8 of datasheet.
Q2.cir -- netlisted circuit holding .SUBCKT model of Q2.

README -- this file.

Simulation.cmd -- a file holding SPICE analysis commands which is read
at simulation time by the SPICE simulator.

5980-2396E.pdf -- Agilent datasheet about the MSA-2643.


./model/

BJTM1_Q1.mod -- text-based SPICE model of BJT1 used in Q1 .SUBCKT
DiodeM1_Q1.mod -- text-based SPICE model of diode M1 used in Q1 .SUBCKT
DiodeM2_Q1.mod -- SPICE model of diode M2 used in Q1 .SUBCKT
DiodeM3_Q1.mod -- SPICE model of diode M3 used in Q1 .SUBCKT
(similar files for Q2 models. . . .)
These models were obtained from parameters give in p. 8 of the datasheet.

./sym/

BJT_Model.sym
spice-subcircuit-IO-1.sym
spice-subcircuit-LL-1.sym
Q_Model.sym -- symbol pointing to lower level models placed on upper
level schematic.

------------  Usage of hierarchical spice models ---------------------
This project exemplifies construction of a hierarchical SPICE
simulation using gEDA.  The project is built in the following way:

1.  Use a text editor to create .mod files containing SPICE models of
the transistors and diodes on p. 8 of the datasheet.

2.  Create Q1 and Q2 transistor model schematics using gschem.  Place
the .SUBCKT SPICE block on the schematic to alert the netlister that
the schematic is a lower level .SUBCKT for incorporation into other
schematics.  Place spice-IO pads on the schematic to instantiate the
IOs.  Make sure to number the spice-IO pads in the same order as you
wish them to appear in the .SUBCKT line in the .cir.

3.  Generate the .SUBCKT netlist by saying:

gnetlist -g spice-sdb -o Q1.cir Q1.sch
gnetlist -g spice-sdb -o Q2.cir Q2.sch

4.  Create a symbol for Q1.cir and Q2.cir which will be dropped onto
the higher lever schematic.  Name the symbol Q_Model.sym.  Set the
symbol "DEVICE" attribute = NPN_TRANSISTOR_subcircuit.  This causes
the netlister to use "write-default-component" to write out the SPICE
line for the component.  Make sure that the "REFDES" attribute is X?
and not Q? -- this enables the .SUBCKT file to be attached to the
device.

5.  Create the higher layer schematic MSA-2643.sch.  Place
two copies of Q_Model.sym onto the schematic, corresponding to Q1 and
Q2.  Make Q1 point to its model by setting the following attributes:

model-name: Q1_MSA26F
file: Q1.cir

Do the same for Q2.

6.  Create the rest of the higher layer schematic the usual way.  Make
sure to place a spice-include block on the schematic and point it to
"Simulation.cmd".  Place any analysis commands (e.g. .DC, .AC, .TRAN,
etc.) into the file "Simulation.cmd".

7.  Netlist the higher layer design:

gnetlist -g spice-sdb -o MSA-2643.cir MSA-2643.sch

8.  The circuit may be simulated by any desired SPICE simulation
and analysis package, e.g. LTSpice.

--------------------  Contact  ----------------------------
Documentation and other materials relevant to SPICE simulation under
gEDA lives at http://www.brorson.com/gEDA/SPICE

For inquiries or bug reports, please contact me:

Stuart Brorson
mailto:sdb@cloud9.net
</code>