I would need to simulate these two MOSFETs ino LTSPICE but I have the Spice Model

  1. IPW65R019C7
    Its PSpice model its insiede Nchannel CoolMos C7 https://www.infineon.com/cms/en/product/promopages/power-mosfet-simulation-models/#high-voltage-simulation-models

  2. SCT3022AL Its PSpice model its at this link https://www.rohm.com/search/application-notes?Category=3D%20Data|Frequency%20Model|IBIS%20Model|Ray%20File|SPICE%20Model|SPICE%20Simulation%20Evaluation%20Circuit|Thermal%20Model&Title=sct3022al

Can anyone explain me the steps necessary to insert them into LTspice?

Thank You.

  • 1
    \$\begingroup\$ I usually cheat and directly edit c:\program files\LTC\Ltspice\lib\sym\standard.mos and add one more line with the .model statement. You need to add mfg= and Vpk= manually. \$\endgroup\$
    – winny
    Commented Sep 22, 2018 at 8:54
  • \$\begingroup\$ Can you explain better all the steps? Sorry but I'm a beginner with LTspice. \$\endgroup\$
    – Fabio
    Commented Sep 22, 2018 at 9:01
  • \$\begingroup\$ Try to open the file and see if you can understand the syntax first. \$\endgroup\$
    – winny
    Commented Sep 22, 2018 at 9:05

3 Answers 3


An alternative solution that worked for me:

  1. Copy the downloaded foo.lib (extension of the file does not matter) to Documents\LTspiceXVII\lib\sub
  2. Start LTSpice and open foo.lib (select File Type to include All Files (*.*))
  3. Find the .SUBCKT line corresponding to the part you're interested in
  4. Right click on .SUBCKT keyword, and click Create Symbol menu item. This will create a .asy file with the symbol with pins that match the pins in the model file.
  5. Optional: edit the drawing of the auto-generated symbol (e.g. for a MOSFET, remove the yellow box and draw a MOSFET symbol); it is sometimes useful to hide the pin labels by right clicking the pin and selecting NONE(Not Visible).
  6. Save the symbol file. It is located in Documents\LTspiceXVII\lib\sym\AutoGenerated; you can leave it there.
  7. Open your schematic or create a new one, add component, navigate to [AutoGenerated] folder/category, the symbol you created above should be there.

P.S. The solution using .lib foo.sub and value=foo on a generic symbol (pmos in my case) makes sense, but it did not work for me: LTSpice throws an error that model foo was not found. This may be fixed by changing the prefix to X, to tell LTspice that you're loading a .SUBCKT, not a .MODEL (but I have not tried this.)

  • \$\begingroup\$ You don't keed to rename the circuit's extension: LTspice is oblivious to them. You can even open files without extensions. You can .lib foo.XXX (remember, extensions are not mandatory) with the generic PMOS symbol but you need to change the prefix to X, to tell LTspice you're loading a .SUBCKT, not a .MODEL. Your informations are skewed, probably from a lack of understanding the way LTspice works. I'm sorry, but -1 for misinformation. \$\endgroup\$ Commented Oct 14, 2021 at 9:17
  • \$\begingroup\$ Thanks for the tip about prefix. Perhaps that's missing from the other answer, seems like a critical piece. In my approach, I needed to rename to .cir in order to open the file in LTSpice (to be able to right-click .SUBCKT keyword). The open dialog accepts only a limited range of extensions. \$\endgroup\$
    – alexei
    Commented Oct 15, 2021 at 15:50
  • 1
    \$\begingroup\$ You can select All files (*.*) and you'll be able to open it. Or simply drag it over the workspace, whichever way is more convenient. Any file will be opened, even binary ones. In fact, if you take any file, binary or not, and insert a .subckt <whatever> [etc], it will be opened by LTspice, that line recognized, and the "create symbol" will be available on clicking over the .subckt part (I'm not saying successfully). Feel free to add this information to the answer (I'll remove the downvote). \$\endgroup\$ Commented Oct 15, 2021 at 16:14
  • \$\begingroup\$ Edited the answer. \$\endgroup\$
    – alexei
    Commented Oct 16, 2021 at 4:53
  • \$\begingroup\$ If you don't use the @ then the users won't be notified of any replies. Use @<TAB> to cycle between names. If no name comes up then there's no need to use @ -- such as it was in my case, because I was the only one commenting and because I did it below your answer (any comment below yours will automatically notify you, and any comment inside any main question, including answers, will automatically notify the OP). \$\endgroup\$ Commented Oct 17, 2021 at 6:54

When you download the files, you see that these is just basic .lib files which any spice simulator can handle. There is no conversion needed.

Here is a good youtube video by LT which shows you how to import and use a third party model. The part of the video you would be interested in starts at around 7:12


  • \$\begingroup\$ This should be the accepted solution. Works like a charm! \$\endgroup\$ Commented Aug 2, 2022 at 15:18

You can either create a symbol, or use a part (like an op amp) and link a circuit file to it. The thing to keep in mind with lt spice is the .asc files link .asy parts in the graphical editor together. The pins on these have to match the circuit library files or you might unintentionally swap a pin. After that a netlist is generated (which you can check to make sure the pins are in the right order) under view spice netlist.

It is possible in LTspice IV to create a new symbol from scratch for a third-party model but who has the time? Follow these easy steps to generate a new symbol for a third-party model defined in a subcircuit (.SUBCKT statement).

  1. Open the netlist file that contains the subcircuit definitions in LTspice (File > Open or drag file into LTspice)
  2. Right-click the line containing the name of the subcircuit, and select Create Symbol:
  3. Create Symbol: Edit the symbol if needed and save.

To use the new symbol (and associated third party model) in a schematic, select the symbol from the AutoGenerated directory in the component library (F2) and place it in your schematic:

Source: http://www.analog.com/en/technical-articles/ltspice-simple-steps-to-import-third-party-models.html

If your using a part like (opamp2 or nmosx ect) then do this:

  1. On the link you posted, scroll down to the PSpice model, unzip the folder, and open LM339_5.1 with notepad. Save the file in C:/program files/LTC/LTspiceIV/lib/sub as LM339.sub. Change "save as type" to "All files".

  2. If LTspice is already open, close and then reopen it.

  3. Open a new schematic window (Leftmost icon on toolbar). 4.Click on the component icon (the AND gate on the toolbar).
  4. Double-click on [Opamps].
  5. Scroll all the way to the end and select opamp2.
  6. Click OK.
  7. Left-click to place opamp2 symbol on schematic.
  8. Right-click on symbol to open Component Attribute Editor.
  9. Left-click on Value.
  10. In the edit window that says Value = opamp2, change opamp2 to LM339. In general, the value you enter here must be identical to the subcircuit name in the subcircuit file. In this case, that line reads .SUBCKT LM339 1 2 3 4 5
  11. Left-click on the .op icon (rightmost on the toolbar). This is the spice directive icon .
  12. Type .lib LM339.sub in the window. Left-click on OK.
  13. Place this spice directive on the schematic by dragging it to where you want to place it, and then left-clicking.
  14. You are now ready to place and connect other components before simulating.

Source: RonH https://forum.allaboutcircuits.com/threads/importing-models-into-ltspice.36456/

  • \$\begingroup\$ Thanks this works fine! A headsup though, LTspiceXVII (at least) copies the entire lib sub-folder into My Documents, and it's that copy you need to add the .sub to now.. \$\endgroup\$ Commented Dec 17, 2020 at 13:36

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.