diff options
Diffstat (limited to 'Windows/spice/examples/xspice/table/README.table')
| -rw-r--r-- | Windows/spice/examples/xspice/table/README.table | 55 |
1 files changed, 0 insertions, 55 deletions
diff --git a/Windows/spice/examples/xspice/table/README.table b/Windows/spice/examples/xspice/table/README.table deleted file mode 100644 index ca286eec..00000000 --- a/Windows/spice/examples/xspice/table/README.table +++ /dev/null @@ -1,55 +0,0 @@ -This example/xspice/table directory offers input files, table files as -well as table generators for the ngspice table model. This model is a XSPICE -extension for ngspice. It enables simulation of devices that consist of in/out -data points, i.e. devices where analytical model equations are not available. - -The table model reads a value val from a file. With the 2D table model val -depends on 2 input parameters, i.e. val = f(x,y), with the 3D table on 3 input -parameters, i.e. val = f(x,y,z). Val may be defined as a voltage or as a -current, either single ended or differential. The inputs x, y (, z) may be -voltage inputs (infinite input resistance, single ended or differential) or -current sinks (zero input resistance, single ended or differential). Single -ended denotes: one node given, the other is 0 (ground), differential: both -nodes are to be given. - -For some implementation details, and the format of the 2D or 3D tables, -please have a look at the ngspice manual, chapters 12.2.27 and 12.2.28. - -How to generate these tables? -For simple functional relationships you may do this manually. For example in -the table directory there are the files test~.table containing simple linear -curves. - -You may analyse measured curves and fit their data into the table format. - -If you already have functional models, you may design a table generator. It -runs the models at certain input condition, calculates the output and stores -it with the correct format. Some examples are given here in the -table-generator files. The bsim4 tables have been thus generated already and -are distributed as files bsim4~.table. - -The example input files table-model-bip~.sp require some further user action -because their table is not provided with the distribution due to its large -size. So cd into the table directory and run the following command: -ngspice table-generator-q-2d.sp -The table will be generated, using the built in ngspice bipolar model and model -parameters for a CLC409 bipolar npn transistor. - -Some considerations for using table models -These table models are pure dc models. The input is an ideal open (for voltage) -or short circuit (for current). If your application requires a more complex -input behavior, it may be emulated by additional passive (or active?) devices -added to the table model. Also, if dynamic behavior ir expected, there a no -capacitors in the table model, so again add them externally. The example input -files give some hints: The bipolar table transistor should show a base input -behaviour like a common transistor, so we have added a diode with parameters -optimized to compare well with the analytical model. The MOS transistors at -least require some input capacitance, emulated by some extra capacitors. So -the table models offer a lot of freedome, but require careful considerations -of their environment to become really useful. - -The 2D and 3D table models use linear interpolation to obtain their output -data. This may limit the application to not have a too steep slope. Otherwise -convergence problems may arise. The derivatives (output vs. each input) -required by ngspice are calculated by an approach named eno (essentially non -oscillating) interpolation, that has proven itself to be very robust. |