LTSpice: importing models?

"Claus Jensen" schrieb im Newsbeitrag news: snipped-for-privacy@4ax.com...

Hello Claus, there is a great support group(forum) for LTSPICE users.

It contains now more than 4300 postings and hundreds of LTSPICE circuit(schematic) examples.

Basically there are two types of third party SPICE models, ..MODEL and .SUBCKT .

The .MODEL models are for the basic parts like transistors diodes and mosfets. They decribe the intrinsic SPICE models.

The .SUBCKT models are subcircuit models which are used when more than the intrinsic model is needed. Examples are additional lead inductors and capacitors or more complex subcircuits like opamp models.

The way how to include it depends on the model type. The easiest way for a .MODEL part is placing the .MODEL definition directly into the schematic or using a ..INCLUDE filename command line to add the definition to your schematic.

Example for a npn transistor:

1. Add a npn-symbol to your schematic.
2. Replace the value NPN with BC547C

3a. Add the .MODEL BC547C line to your schematic 3b. If you have a file bipol.lib containing your .MODEL BC547C (others may be too in this file), then you have to add a command line .INCLUDE bipol.lib

Example for a 5-pin opamp:

1. Add a opamp2-symbol to your schematic. [Opamps] opamp2
2. Replace the value opamp2 with TL072 in your schematic.

3a. Add the .SUBCKT ..... line to your schematic 3b. If you have a file ti.lib containing your .SUBCKT TL072 (others may be too in this file) then you have to add a command line .INCLUDE ti.lib

Example for a 3-pin npn transistor, but with a .SUBCKT

1. Add a npn-symbol to your schematic.
2. Move the cursor over the placed npn. Press RightMouseButton. A dialog box will appear. Change Prefix: QN to Prefix: X X stands for subcircuit. OK
3. Replace the value NPN with BFG135

4a. Add the .SUBCKT BFG135 lines to your schematic 4b. If you have a file Phil.lib containing your .SUBCKT BFG135 .... (others may be too in this file) then you have to add a command line .INCLUDE Phil.lib

These are the basics you should know for the green belt.

If you want learn more about symbols and subcircuits with LTSPICE, then you should read my explanations in the Files area of the mentioned Yahoo group. If you have understood that, you get the black belt.

Files > Tut > Symbol Types For Subcircuits

Beyond that, LTSPICE offers hierarchical schematics. This is indeed another great schematic feature. A good description about it is in the LTSPICE help pages.

Best Regards, Helmut

command line = SPICE directive

..MODEL BC547C NPN(IS=1e-12 ....)

..SUBCKT TL072 12 3 45 6 78 Many SPICE lines ..ENDS