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
