Claus Jensen said:
As some readers would already know, LTSpice is a great analog
simulator but most of the included models are Linear Tech brand.
I have done some research, but still can't figure how to reliably
import spice models from other providers.
Can some kind soul infused with the Christmas spirit please list in
1,2, 3 ... fashion how to do this, or direct me to an online source
for same.
Maybe provide an example using a specific part, if possible.
Given the apparent popularity of this excellent program, I assume
others would also benefit from this information in the future.
Many thanks,
Claus
Hello Claus,
there is a great support group(forum) for LTSPICE users.
http://groups.yahoo.com/group/LTspice
It contains now more than 4300 postings and hundreds
of LTSPICE circuit(schematic) examples.
Basically there are two types of third party SPICE models,
..MODEL and .SUBCKT .
The .MODEL models are for the basic parts like transistors
diodes and mosfets. They decribe the intrinsic SPICE models.
The .SUBCKT models are subcircuit models which are used
when more than the intrinsic model is needed.
Examples are additional lead inductors and capacitors or
more complex subcircuits like opamp models.
The way how to include it depends on the model type.
The easiest way for a .MODEL part is placing the .MODEL
definition directly into the schematic or using a
..INCLUDE filename command line to add the definition
to your schematic.
Example for a npn transistor:
1. Add a npn-symbol to your schematic.
2. Replace the value NPN with BC547C
3a. Add the .MODEL BC547C line to your schematic
3b. If you have a file bipol.lib containing your
.MODEL BC547C (others may be too in this file),
then you have to add a command line
.INCLUDE bipol.lib
Example for a 5-pin opamp:
1. Add a opamp2-symbol to your schematic. [Opamps] opamp2
2. Replace the value opamp2 with TL072 in your schematic.
3a. Add the .SUBCKT ..... line to your schematic
3b. If you have a file ti.lib containing your
.SUBCKT TL072 (others may be too in this file)
then you have to add a command line
.INCLUDE ti.lib
Example for a 3-pin npn transistor, but with a .SUBCKT
1. Add a npn-symbol to your schematic.
2. Move the cursor over the placed npn.
Press <Ctrl>RightMouseButton. A dialog box will appear.
Change Prefix: QN to Prefix: X
X stands for subcircuit. OK
3. Replace the value NPN with BFG135
4a. Add the .SUBCKT BFG135 lines to your schematic
4b. If you have a file Phil.lib containing your
.SUBCKT BFG135 .... (others may be too in this file)
then you have to add a command line
.INCLUDE Phil.lib
These are the basics you should know for the green belt.
If you want learn more about symbols and subcircuits
with LTSPICE, then you should read my explanations in
the Files area of the mentioned Yahoo group. If you
have understood that, you get the black belt.
Files > Tut > Symbol Types For Subcircuits
Beyond that, LTSPICE offers hierarchical schematics.
This is indeed another great schematic feature.
A good description about it is in the LTSPICE help pages.
Best Regards,
Helmut
command line = SPICE directive
..MODEL BC547C NPN(IS=1e-12 ....)
..SUBCKT TL072 12 3 45 6 78
Many SPICE lines
..ENDS
