--- In LTspice@..., "lawrence_joy" <lawrence_joy@...> wrote:
I am not understanding where/how to put 3rd party .SUBCKT files into
LTSpice. The explaination in the PDF manual seems to have the cart
before the horse. I "drew" a schematic using Opamp2.
Hello Lawrence,
The symbol "opamp2" can be used for most of the opamp models from
all manaufacturers. This symbol requires that the models have
the following pin-order in the .subckt line.
Symbol's netlist order: 1 2 3 4 5
Subcircuit's definiton: in+ in- v+ v- out
On page 94 of the manual, at the bottom, number 1 I can do.
Page 95, at the top, number 2 I could not do until I looked at
the ON Semiconductor file.
And number 3 I can not do because I don't understand the details.
Can you tell me which document you have?
I wonder about the page numbers.
Under "Library Path" on page 95, Example 1. After "\sub\" for the
library file can I have subfolders of ONSemi, TI, and NSC with
.SUBCKT files under each?
Library files can be stored in any folder on your hard disk.
There are two default folders were LTspice looks for these files if
you have only specified the file name. This default folders
for subcircuits are the folder where the schematic is saved or the
\lib\sub folder.
Do I need the last subfolder to have a .lib extension?
The name or file extension of the library file doesn't matter.
You can always leave the name as it is.
On page 96 of the manual under "Fast Route For Circuits And
Symbols" I tried the example.
By "Copy" I assume that means to pick the LT1013
device from the library and place it in a schematic. Editing
commands only has "Duplicate". The next step of
You have to open the symbol file LT1013.asy and then to save it
it under another name, e.g. MC324.asy.
"Change LTC.lib -> xyz.lib" can not be done because I get a
message "This Component can not be edited".
And that is exactly what Individual Symbol (Type-1) is.
You can edit the symbol properties if you are in the symbol editor.
This requires to open the symol file (extension .asy). See above.
Menu: Edit -> Attributes -> Edit Attributes
There are basically three different types of symbols possible.
The opamps from LT use a specific symbol for each type of opamp.
The library file is specified in the symbol attributes.
The "opamp2" symbol is a universal symbol with no library
specification in the symbol attributes. This library file name
has to be included in the schemaic with a command line.
.include lm324.abc
Please read the folowing documents.
1. FAQ "Third party models" in the help pages of LTspice
2. Yahoo group: Files > FAQ
3. Yahoo group: Files > Tut > Symbol Types For Subcircuits
There are many examples under "Files > Lib", e.g. with he LM324.
The LM324 example is using an universal symbol and a specific symbol.
Yahoo group: Files > Lib LM324
I recommend to keep the third party library files in the folder
of the schematic. This makes the backup of designs very easy.
This path is in the default search list and so you never have to
specify the whole path.
You always have the choice between an universal or a specific symbol.
Universal symbols have the advantage that one symbol fits all
models if the subcircuit definition has the same netlist order.
Best regards,
Helmut
