Importing power mosfet model into LTspice

Thread Starter

Sam A

Joined Oct 10, 2016
3
Hey all,

I am somewhat of a newbie when it comes to using LTspice. I have a Pspice model of a power mosfet that I downloaded from the Infineon website and I want to import it into my LTspice model. I have opened the .lib text file of the model, saved it as a .sub file in the library location on my C drive, but what do I do after I click the component button? I have attached the model for reference.

Thanks!
 

Attachments

wayneh

Joined Sep 9, 2010
17,498
It could be as easy as using the "include" Spice directive into your simulation.

I've adopted the "recommended" procedure of putting the component models in the same directory as my project. One big advantage of this is that you can zip the folder and everything you need will be there in one file. Great for portability and sharing.

You can instead make custom components behave just like they're part of LTspice, but it takes jumping through a few hoops. You potentially will have to redo the hoops after every update to LTspice.

Do you have a symbol model of your MOSFET? If you need a custom symbol, you need to place it in your user's library. For instance adding an op-amp symbol to your library on a Mac, place it at
users:yourUserName:library:application support:LTspice:lib:sym: opamps: your file.asy
 
Last edited:

eetech00

Joined Jun 8, 2013
3,942
Hey all,

I am somewhat of a newbie when it comes to using LTspice. I have a Pspice model of a power mosfet that I downloaded from the Infineon website and I want to import it into my LTspice model. I have opened the .lib text file of the model, saved it as a .sub file in the library location on my C drive, but what do I do after I click the component button? I have attached the model for reference.

Thanks!
Hi

Based on the content of the CompPower_20V.sub file, these are the names of the devices:

BSL215C_n_L1
BSL215C_p_L1
BSL215C_n_L0
BSL215C_p_L0

BSZ15DC02KD_n_L1
BSZ15DC02KD_p_L1
BSZ15DC02KD_n_L0
BSZ15DC02KD_p_L0

BSL235C_n_L1
BSL235C_p_L1
BSL235C_n_L0
BSL235C_p_L0

So....for the following example I'll use the nmos device "BSL215C_n_L0" and the .sub file location is the "c:\mylib\nmos" folder:

1. Place an nmos symbol on the schematic.
2. CTL+RHT CLK the symbol, then:
2a. change the "Prefix" field to "X" (without quotes)
2b. change the "Value" field to "BSL215C_n_L0" (without quotes)
2c. click OK​
3. Click anywhere on schematic, then type the letter "t", to open a text dialog box.
3a. click "Spice directive" radio button
3b. click in the text box area, then type ".include c:\mylib\nmos\CompPower_20V.sub" (without quotes)
3c. click OK​

Perform this same operation for any of the devices while choosing either the nmos or pmos symbol.
Note-
If you place the .sub file in the default LTSpice "lib\sub" folder, then you can skip step 3b.
If you place the .sub file in the same folder as your schematic, then the folder path specified in step 3b is not needed.
 
Hi Sam,
There is a simple way. Open .lib file in LTspice, click the .SUBCKT, then right click it, chose "create a symbol". Then you will get an auto generated symbol (.asy file). When you open a new schematic file, you can find it in "Autogenerated" folder after you click "component" symbol. See the attach picture.
 

Attachments

Top