Hi
(I am student form Poland/Europe)
I'm looking for library for LTspice with power MOSFET (current ~ 20..100Ampers). I found very good transistors like:
IRL3705
IRL2203
... but International Recifier gives only PSpice (or Saber) models
https://www.infineon.com/cms/en/search.html#!term=IRL2203&view=all
Is simple way use them in LTspice?
thanks for help in advance
Maciej

 

Hi, welcome to the forum.
That looks like a standard model of a mosfet and I don´t think you should have any trouble using it in ltspice.
see http://www.linear.com/solutions/5360

 

hi matheu,
Try this,
Rename the LTS standard.mos as standardold.mos, then copy the attached file into the same folder as the standard.mos.
You will find the IRL3705 and IRL2203 in this file.
The Credit for this cmp file is due to @Bordodynov

To upload the file I have had to change the extension to .txt, change it back to .mos

E

 

Hi
(I am student form Poland/Europe)
I'm looking for library for LTspice with power MOSFET (current ~ 20..100Ampers). I found very good transistors like:
IRL3705
IRL2203
... but International Recifier gives only PSpice (or Saber) models
https://www.infineon.com/cms/en/search.html#!term=IRL2203&view=all
Is simple way use them in LTspice?
thanks for help in advance
Maciej

Hi

Generally speaking, LTspice is PSpice compatible, but sometimes you have to convert certain statements.
However, you should be able to use this model without conversion.

To use it:
1. Place the nmos symbol on the schematic.
2. View the symbols properties and change the "Prefix" to "X" without the double quotes.
3. Replace "NMOS" with "IRL2203N", without the double quotes, in the "Value" property.
4. Place the model file irl2203n.spi into the same folder as the schematic.
5. Add ".inc irl2203n.spi" statement, without the double quotes, to the schematic.

I performed these steps in the attached image.



You should be able to use the IRL3705N model in the same way.

 

I didnt belive that whos wants help me!
You are great (and VERY fast)
Thank you!

I did it according to eetech00 (and I gave irl2203n.spi to the folder with the schema), but I got only message:
"Can't find definition of model ... "

I think that I did only simple mistake, but I don't know where...

Ericgibbs:
I used library "standard.mos" from you - and some parameters from eetech00.

It works for me, but I have to work with chart.

Thank you, mates!
M.

 

...plot...

Hmm, how did you get a DC plot (or current versus DC voltage) in a transient simulation? Can you post the asc file so I can see how you did that?

 

Sure!

************************************ NMOS-test2.asc
Version 4
SHEET 1 880 680
WIRE -480 -544 -544 -544
WIRE -304 -544 -480 -544
WIRE -544 -464 -544 -544
WIRE -304 -400 -304 -544
WIRE -672 -384 -784 -384
WIRE -592 -384 -672 -384
WIRE -784 -368 -784 -384
WIRE -784 -272 -784 -288
WIRE -544 -272 -544 -368
WIRE -304 -272 -304 -320
FLAG -784 -272 0
FLAG -544 -272 0
FLAG -304 -272 0
FLAG -672 -384 gs
FLAG -480 -544 d
SYMBOL voltage -784 -384 R0
WINDOW 123 0 0 Left 2
WINDOW 39 -32 -16 Left 2
WINDOW 0 28 32 Left 2
WINDOW 3 35 60 Left 2
SYMATTR InstName V1
SYMATTR Value {Vgs}
SYMBOL voltage -304 -416 R0
WINDOW 123 0 0 Left 2
WINDOW 39 21 -2 Left 2
WINDOW 0 28 32 Left 2
WINDOW 3 30 80 Left 2
SYMATTR InstName V2
SYMATTR Value PWL(0 0 1 {Vds})
SYMBOL nmos -592 -464 R0
SYMATTR InstName M1
SYMATTR Value IRL2203N
TEXT -816 -232 Left 2 !.tran 1\n.options plotwinsize=0\n.step param vds 0 10 1\n.step param vgs list 2.7 3.0 3.3 3.5 3.7 4.5 10 15
****************************** end of file

 

Hmm, how did you get a DC plot (or current versus DC voltage) in a transient simulation? Can you post the asc file so I can see how you did that?

Hi

I explained it all in post #4. But I'll post a zip file.

Just unzip the file and run the .asc file. When it completes, reload the plot file so it refreshes the plot correctly.

 

I didnt belive that whos wants help me!
You are great (and VERY fast)
Thank you!

I did it according to eetech00 (and I gave irl2203n.spi to the folder with the schema), but I got only message:
"Can't find definition of model ... "

I think that I did only simple mistake, but I don't know where...

Ericgibbs:
I used library "standard.mos" from you - and some parameters from eetech00.

It works for me, but I have to work with chart.

Thank you, mates!
M.

Hi

Problems like that are usually related to how you manage your library files. Or caused by embedded file paths.
use the native NMOS symbol and place the irl2303.spi model file in the same folder as the schematic.
Don't forget to change the mosfet symbol's properties.

eT