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

"rmoreno.phone" asked how to enter a table of measured values for her/his CCVS.

Vlad might have had the table descriptions a little bit confused with respect to your question, because I think the data you have is voltage/current values, not voltage/time values.? You wanted a controlled or dependent source, not an independent source.

Using SPICE's built-in H element (current controlled voltage source or CCVS), LTspice *MIGHT* have the ability to accept a table of current/voltage values.? See the Help pages for E (VCVS) and G (VCCS) elements.? A table is listed as an option. ?"A look-up table is used to specify the transfer function." ?The same 'table' description is not listed for the F (CCCS) and H (CCVS) elements.? I am not sure if that was an omission on those Help pages, or if that option really doesn't exist for those two controlled sources.? The "LTwiki" () is where I usually go when I have questions about the Help pages.? Unfortunately, the LTwiki also doesn't show a table option for the CCVS.? That leads me to believe that you can't use a table with the standard CCVS element.

But LTspice's B-elements can do that and much more.

Here is from the Help page for B-elements:

? table(x,a,b,c,d,...) ??Interpolate a value for x based on a look up table given as a set of pairs of points.

Start with a Bv symbol, then right-click on "V=F(...)" and edit it.? I think (but could be wrong) it should look like this when you are done:

V=Table( I(V4), 0mA, 0V, 1mA, 1mV, 2mA, 1.9mV, 3mA, 2.5mV ...)

where I(V4) means the current measured through V4 (this is your controlling current), and the pairs that come next, are the (current, voltage) pairs that you measured.

I have rarely used the Table() functions in LTspice, so please excuse my inexperience with them.

Regards,

Andy