(Another reply that vanished into the Internet):
Hassan wrote:
"I have found either the .lib file or the symbol !!! "
That is good.
The first thing to understand is that they are almost completely
independent of one another. A symbol is just an icon, nothing more.
LTspice has some of the symbols already. In the Select Component (F2)
menu, choose the [Misc] area, then you can find DIAC, SCR, and TRIAC
symbols.
If you found .lib files, then you found their SPICE models.
Now all you need to do is: (A) include the .lib file in your
simulation, and (B) associate the symbol with the model inside the
library file.
To include the .lib file, first put the .lib file in the same folder
with your schematic that uses it. Then add this as a SPICE Directive
on your schematic:
.lib filename.lib
To associate the symbol with the model:
Right-click on the symbol body and make sure Prefix is set to X.
Open the .lib file in a text editor (such as Wordpad) to see what's
inside it. There should be a subcircuit definition for the part you
want to use. Scroll down until you find it. It might look something
like this:
.SUBCKT 2N6071B MT2 G MT1
Now you know the actual name of the model: 2N6071B. And you know the
order of the pins: MT2, G, MT1. There could be several .SUBCKTs in
the same file, each for a different part. Find the one you want.
Go back to your schematic. Edit the name next to the symbol, and
change it from "TRIAC" (or "SCR" or "DIAC"), to the name of the
subcircuit you want to use ("2N6071B" in this case).
The tricky part is to make sure the order of pins is correct.
For a Triac, LTspice assumes the order of pins is MT2, G, MT1. If the
order differs from that, then you should edit the .lib file and change
the pins in the above .SUBCKT line to make them in that order. This
may take a little effort to understand what the pins are, when they
don't have those specific names.
Regards,
Andy
Tony Casey