|
LTspice Tutorial: Part 4
This LTspice Tutorial
explains how to import third party models into
LTspice®.
LTspice is not limited
to simulating Linear Technology parts. Third party
models can be imported into LTspice too. There are 2
types of model that can be imported into LTspice:
.MODEL parts - these
are simple components such as transistors and diodes
.SUBCKT parts - these
are more complex parts made up of simpler Spice
parts (diodes, transistors, resistors etc)
It is important to
note that LTspice looks at the first line of the
SPICE model to determine how the model should be
handled. If the part is defined with a .MODEL
statement, importing the model is handled one way;
if the part is defined with a .SUBCKT statement,
importing the model is handled in a slightly
different way. Thus we could import 2 identical
diodes, one defined with a .MODEL statement and one
defined with a .SUBCKT statement and they are
actually handled differently.
LTspice looks at the model definition, NOT the
component to determine how to import the part.
.MODEL parts:
To import a simple
third party SPICE model into LTspice using the
.MODEL directive , follow these steps:
-
Add a generic
component to the schematic that represents the
symbol of the SPICE model
-
Download the SPICE
model into the same directory as the circuit you
are simulating.
-
Make a note of the
filename of the SPICE model, including the file
extension.
-
Add a .include
SPICE directive to the schematic that will use
the model
-
Open the SPICE
model and note the name of the model - this is
the text immediately after the .MODEL directive
and before the part designator (in the case
below this is the text DI_SBG1030L). The SPICE
model can be viewed from within LTspice.
-
Press <CTRL> then
right click over the generic component and
change the 'Value' field to the SPICE model name
-
Ensure the
.include SPICE directive contains the exact
filename of the SPICE model
-
Ensure the name of
the generic component exactly matches the SPICE
model name
Here is an example of
how to import a Schottky diode into a circuit. FIG 1
shows a simple circuit to measure the forward
voltage drop across a diode. This can be downloaded
here: Diode
Test Circuit
FIG 1
Running the simulation
shows the diode has a forward voltage drop of
653.2mV
Remove diode D1 and
replace it with the standard Schottky diode from the
LTspice library.
Download the SPICE
model of the BAT 54 Schottky diode:
BAT 54 SPICE
model and save it in the same directory as the
circuit in FIG 1.
Add the following
SPICE directive to your schematic using the
symbol:
.include DI_BAT54.txt
To avoid spelling
mistakes, use Windows Explorer to highlight and copy
the filename including the filename extension
(.txt). Paste the text after the include statement.
Open the SPICE model
file (using, say, Notepad) and note the name of the model (in this case it
is DI_BAT54). Again, to avoid spelling mistakes, it
is easier to highlight the model name and copy it.
Press <CTRL> Right
click over the Schottky diode symbol and paste the
text DI_BAT54 into the Value field as shown in FIG
2. Do not put any comments in the Spice Model field.
FIG 2
The final circuit
should look like FIG 3
FIG 3
Run the simulation.
The forward voltage drop should now be 290mV.
If you encounter
errors, check the following:
Has the SPICE file
been loaded into the same directory as the
simulation file?
Is the part name the
same as that specified in the SPICE model?
Does the filename in
the .include statement exactly match the SPICE model
filename?
It is also worth
opening the SPICE model file from within LTspice and
checking its contents. Some text editors can add
formatting characters that confuse LTspice.
.SUBCKT parts
A similar procedure
can be used to import more complex models. Follow
the steps above, except when modifying the Component
Attribute Editor (see FIG 2), ensure the Prefix attribute is marked as
X (and not D as in FIG 2).
We are now going to
compare the performance of the LT6231, (215MHz low
noise op amp) with the LM324 (low cost op amp).
Download the circuit
in FIG 4:
Op
Amp Test Circuit
FIG 4
Running this circuit
shows the output falls from 1V at dc to 0.707V at
about 2.77MHz.
Now remove the LT6231
and replace it with a standard 5 terminal op amp.
This is the 'opamp2' model in the Op Amps folder in
LTspice.
Download the LM324
model: LM324
model and save it in the same directory as the
circuit in FIG 4.
Make a note of the
SPICE model filename (in this case it is LM324.txt).
Add a .include SPICE directive in your schematic as
follows:
.include LM324.txt
Open the SPICE model
and make a note of the SPICE model name (immediately
after the .SUBCKT command). In this case it is
LM324.
Press <CTRL> Right
click over the op amp symbol in the schematic and
insert the model name into the Value field as shown
in FIG 5
FIG 5
Ensure that the Prefix
attribute is filled in with X.
NOTE: The SPICE model
of some simple components (e.g. Zener diodes) are
defined as a SUBCKT. In this case, the Prefix
attribute has to be 'X' and not 'D' to correspond
with the .SUBCKT SPICE definition (and not a .MODEL
definition).
Creating a Quick
Part Outline for 3rd Party SPICE models
Once the SPICE model
has been imported, an outline can be created for the
part. Open the SPICE model in LTspice, move the
mouse over the .SUBCKT line, right click and select
'Create Symbol'. A square symbol will appear showing
the nodes of the SPICE model.
FIG 5a
Then select a new
component (using the AND gate symbol) and in the
dialogue box, the new component is stored under the
[AutoGenerated] directory.
Running the simulation
shows the output falls to 0.707V at about 10kHz,
showing the inferior frequency response of the LM324
over the LT6231.
The final circuit is
shown in FIG 6
FIG 6
SPICE models for many
components that are needed with LTC devices can be
downloaded here:
SPICE Models
for LTspice
Want to know more?
Please see
LTspice
Tutorial: Part 5
LTspice is a registered trademark of Linear
Technology Corporation |
