You can add many components to LTSPICE.
Step 1: get the respective SPICE model from the manufacturer.
Step 2: Look at the model file. There are basically 2 types of model:
a) a model based on the internal model for elementary components where the model parameters are added in form of a parameter list.
b) models based on subcircuits.
The two types of model are treated differently.
Example for a), BCX17:
Get the
model from NXP (under Downloads -> All models). Open the ZIP file and extract BCX17.PRM. This is a text file, you c an rename it to BCX17.TXT to open it with any text editor. Find the Library for bipolar transistors (e.g. C:\Program Files (x86)\LTC\LTspiceIV\lib\cmp\standard.bjt) Open it with a text editor (you may need admin rights) and append the model description from the BCX17.PRM file, the lines from
-----------------------
.MODEL QBCX17 PNP
+ IS=1.08E-13
...
+ FC=0.99
-----------------------
Save standard.bjt and you will now have QBCX17 as an additional model in LTSPICE.
Example for b), LMX321 operatinal amplifier.
Get the
model from MAXIM, save the file (LMX321.FAM on your hard drive). From within LTSPICE (!) go to file -> open -> and open the saved LMX321.FAM file (this is a text file, but you have to use the LTSPICE integrated editor for the following steps). Within the editor, fin the macro description, in this case it is this line:
.SUBCKT LMX321 1 2 3 4 5
Highlight the complete line with the mouse, the right click and select "Create Symbol" from the popup. Answer yes to the following popup (do you wish to create...) If you get an error message like "trouble creating...", restart LTSPICE with admin rights. LTSPICE will now create a block for this PSICE model that you can use like any other model. If you don't like the looks of the block, you can edit the symbol with the LTSPICE symbol editor.
Here is an
excellent book on LLTSPICE.
