LTSpice: importing models?

"Claus Jensen" schrieb im Newsbeitrag news:

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

formatting link

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

Reply to
Helmut Sennewald
Loading thread data ...

"Helmut Sennewald" schrieb im Newsbeitrag news:cqe79s$v9i$05$

Hello Claus, sorry that I overlooked the part about Christmas spirit.

Please tell me a part/example you are very interested. I promise to deliver it before Christmas Eve.

Merry Christmas and a Happy New Year, Helmut

Reply to
Helmut Sennewald

Claus The LT in LTspice stands for Linear Technology. The purpose of the program is to promote Linear Technology products. LTC competitors offer designs tools, as well, but none can compare to LTspice. The company hopes you'll evaluate LTC products first before looking elsewhere. You certainly can't use National's Webench to design in a TI part while LTspice gives you that freedom. You, as a user, can import any spice model you want to use into the program, but if any other semiconductor vendor attempts to model his products using the program, Linear Tech will sue them. This is discussed in the License Agreement/Disclaimer in the Help file. Linear Technology maintains ownership of the program. The LTspice group on Yahoo is the place to go for help not covered in the program Help file.

- Dave

Reply to

As some readers would already know, LTSpice is a great analog simulator but most of the included models are Linear Tech brand.

I have done some research, but still can't figure how to reliably import spice models from other providers.

Can some kind soul infused with the Christmas spirit please list in

1,2, 3 ... fashion how to do this, or direct me to an online source for same.

Maybe provide an example using a specific part, if possible.

Given the apparent popularity of this excellent program, I assume others would also benefit from this information in the future.

Many thanks,


Reply to
Claus Jensen

Thanks Helmut for the kind offer, but your previous excellent email has more than filled my socking :-)

Seriously, the spice models I need are fairly basic so I have hope of finding them on the mfr's sites.

I will also check out the group files you mention.

And thanks to LT for a great program.

Best regards,


Reply to
Claus Jensen

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.