I have >20 different types of MOSFET from fairchild that I would like to add to LTSpice's model tree. Fairchild encrypts their libraries. What is a straight forward method of adding their libraries to the model tree where I don't have to specify a sub-circuit every time I want to use them. I have hundreds of these FETs and I use them frequently.


I figure this may shed some light on the subject.

* LTspice Encrypted File
* This encrypted file has been supplied by a 3rd
* party vendor that does not wish to publicize
* the technology used to implement this library.
* Permission is granted to use this file for
* simulations but not to reverse engineer its
* contents.
* Fairchild Semiconductor SuperFETIII 650V Model Library
* Last Update: Jun. 02, 2016
* Model Version: 1.3
* Simulator: LTspice
* Model Contacts:
*    James Victory     [email protected]
*    Ken He            [email protected]
*    Scott Pearson     [email protected]
*    Hyeongwoo Jang    [email protected]
* Reversion History:
*   Vers.   Date        Brief Description
*   1.0     03/16/2016  1. Extract scalable base model from data of FCB070N65S3. The process parameters are from
*                          rev2 TCAD simulation (file "SJFET3_650V_TCAD_MODEL_PARAMETER_TABLE_rev2.xlsx")
*                       2. Generated models for :
*                           FCB070N65S3
*                           FCP067N65S3
*                           FCPF067N65S3
*   1.1     05/03/2016  Added model for FCH023N65S3_F155
*   1.2     05/25/2016  Added model for FCH067N65S3_F155
*   1.3     06/02/2016  Added model for FCH023N65S3L4
*                       Updated thermal parameters for FCH023N65S3_F155
* Usage:
* This library contains 3 and 5 pin(or terminal) models. The models include 
* self heating effects and were characterized under pulse conditions from 
* 10us to 1ms conditions. 
* The 5p models contain 2 additional pins tj (or junction temperature) and
* tcase (or device case thermal terminal). 
* tj should always be left floating or can be connected to a very
* large resistor (>1meg). This terminal is meant to provide the user with
* output information on the junction temperature under operation. For model
* verification purposes against the data sheet and isothermal device simulations
* for example, tcase should be connected to a voltage source with value {TEMP},
* the simulator ambient temperature. For system/module level simulations that
* include thermal effects, tcase should be connected to the device-module
* thermal interface node such as the heat sink interface point.
* For the device FCH023N65S3L4 which has a Kelvin Source (4-lead package), there are 4- and 6-pin models, the 3rd pin
* "s1" is the Kelvin Source, the 4th pin "s2" is the Power Source.
* Support devices:
*   FCB070N65S3_3p, FCB070N65S3_5p
*   FCP067N65S3_3p, FCP067N65S3_5p
*   FCPF067N65S3_3p, FCPF067N65S3_5p
*   FCH023N65S3_F155_3p, FCH023N65S3_F155_5p
*   FCH067N65S3_F155_3p, FCH067N65S3_F155_5p
*   FCH023N65S3L4_4p, FCH023N65S3L4_6p
** Begin:
 90 3B 2A 85 D1 AC 5A AE 43 66 6B A8 56 8C 9F F4
 03 E8 4D E9 30 FE 57 15 09 76 CA DC 5D 13 36 1F
 91 60 74 AB 47 45 20 03 46 D7 13 E8 66 1A 13 CF
 94 22 5C 5A 9C 1F 27 A1 4C 65 63 59 EF FC 09 07

I can't even get ltspice to recognize them. Fairchild provides no instruction on how to use them and on LT all I could find was encrypting your own. I tried using them like non encrypted Libraries. The crazy thing is a guy had a library of controller chips I downloaded from a forum and all I had to do was copy and paste it into the folder and I can drag and drop them in with no sweat. I'm designing a SMPS with an SG3525 and it works great in spice. Why is this a headache?

Heres the error I get

Property window

  • \$\begingroup\$ I don't think that's possible, if they're encrypted. The only way I see is placing them in the lib/sub path, together with the other subcircuits, and have them available by simply placing an .inc or .sub directive in the schematic. This, however, is not a practise that is encouraged, as exporting the schematic/project will not make it available for others that do not have that particular custom library. Just a quick question, though: are you sure those models use .MODEL, instead of .SUBCKT? \$\endgroup\$ Commented Sep 25, 2016 at 6:37
  • \$\begingroup\$ I have a lot of Fairchild models and none are encrypted; they do require me to login to get them, though. A specific part might be useful to see if an unencrypted version is available. I will note that Wurth provides an encrypted model library specifically for use in LTSpice. \$\endgroup\$ Commented Sep 25, 2016 at 10:16
  • \$\begingroup\$ I couldn't find anything on the older chip but I edited above to show what I'm dealing with \$\endgroup\$
    – iuppiter
    Commented Sep 25, 2016 at 12:04

1 Answer 1


This may or may not work, but when I have had to import an external model into the libraries so it always shows up (no include statement required), here is the method:

First, create a folder for your own parts within the LTSpice tree under lib\sym:

My parts folder

[Edit] Updated for the case ASY files are provided:

Place the provided ASY files in this folder; the editing procedure will not apply.

Editing proedure for the case where ASY files are not provided:

Open a new schematic and place the NMOS object. Do CTRL:right click to get the properties box:

Properties dialog

Now open the symbol (the top button), then do Edit->Edit attributes

Edit attributes dialog

Put the specific name of the file containing the model in the Spice model line.

Change the value to to the specific model you want to use as exactly the name is in the library (e.g. FCB070N65S3 from the listing above; this is also what will be displayed in the schematic editor).

Now save the file in your new folder as [modelname].asy (e.g.FCB070N65S3.asy)

End of editing procedure for the case where ASY files are not provided.

Make sure that the model file containing the model is in the lib/sub folder.

lib\sub location

This is it, showing one of my components.

Now you should see your own folder in the tree in the schematic editor:

My folder in LTSpice

You should navigate into the folder and you should be able to place the part. The file appears to have been encrypted for LTSpice, so hopefully it should work.

I do not know if the model has been implemented as a subckt (MOSFETs very usually are), so in the edit attributes, you may need to change the prefix from MN to X.

Note that the procedure is identical to the method for incorporating the Wurth encrypted library (and that definitely works).

  • \$\begingroup\$ The good thing I see here is that they already provided me with the ASY files, The library itself is .txt should I rename the extension, and where does it go? Thank you for the answer by the way I've been waiting all night for this. \$\endgroup\$
    – iuppiter
    Commented Sep 25, 2016 at 12:59
  • \$\begingroup\$ You do not need to rename the library file; just make sure you use that exact filename in the attributes; it is possible the ASY files already have that name in them. I am updating the answer as to where the file goes. \$\endgroup\$ Commented Sep 25, 2016 at 13:13
  • \$\begingroup\$ I just edited it to update you on the error I get and the difference in a normal NMOS and that thing \$\endgroup\$
    – iuppiter
    Commented Sep 25, 2016 at 13:50
  • \$\begingroup\$ @PeterSmith You should make a note that, even if this is the user's choice, it will (almost) break any chance of exporting your projects using those symbols, since it's most likely nobody else has your custom libraries/models/etc. As a matter a fact, the suggestion of simply placing an .inc or .lib, rather than messing with the default installation. should be the first thought (if not making folders for all projects and then copying sumbols/libs/etc in there, as needed). Comfort comes at a price that not all would be willing to pay for. \$\endgroup\$ Commented Sep 25, 2016 at 14:00
  • \$\begingroup\$ I don't really plan on sharing them, I'm in back in school, taking engineering now these are personal projects that I'd like to test in a simulated environment to get an Idea of how the components will behave. I'm trying to stay ahead of the class so to speak. We're on ac theory and I'm making an Inverter. \$\endgroup\$
    – iuppiter
    Commented Sep 25, 2016 at 14:07

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.