1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
16
17
18
19
20
21
22
23
24
25
26
27
28
29
30
31
32
33
34
35
36
37
38
39
40
41
42
43
44
45
46
47
48
49
50
51
52
53
54
55
|
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.
|
