• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

Can LTSpice use pspice models

PickyBiker

New Member
I'm new to LTSpice and have trouble understanding how to import 3rd party simulation models. I saw some online comments that say you can use Pspice models, but no clear instructions on how to use them in LTSpice.

If I could get help with this example, I would probably understand how to import others.
Using Windows 10
LTSpice XVII
Part of interest Infineon IPP080N06
Downloaded the PSpice simulation file for this part
The folder is 01_OptiMOS and it contains several files, the .lib file is OptiMOS_60V.lib

So now what needs to happen?
 

MikeMl

Well-Known Member
Most Helpful Member
Post your .lib file, and I will show you how to incorporated it into a running sim...
 

MikeMl

Well-Known Member
Most Helpful Member
This is not going to be easy. Optimos uses a non-standard five pin symbol for its devices (instead of three, like everybody else), where in addition to the standard three "drain, gate, source" pins, they add two "non-physical" pins to send in Tj (junction temperature) and Tcase (case temp). You will have to create a new symbol for LTSpice with five pins.

I have no idea how they "communicate" with those extra pins???
 

PickyBiker

New Member
Not sure I understand the problem.
This chip uses 3 pins in a standard T0220 package.
Manufacturer Part#:
IPP080N06
Product Category: FETs - Single
Manufacturer: INFINEON
Description: MOSFET N-CH 60V 80A TO-220
 

eTech

Active Member
Not sure I understand the problem.
This chip uses 3 pins in a standard T0220 package.
Manufacturer Part#:
IPP080N06
Product Category: FETs - Single
Manufacturer: INFINEON
Description: MOSFET N-CH 60V 80A TO-220

Attached is symbol per AN2014-02 and a test circuit for LTspice.
The Tj terminal is an output used to monitor Junction temperature.
The Tcase terminal is an input and models ambient temperature (1V=1C).
See Infineon application note "Application Note AN 2014-02".

eT
 

Attachments

PickyBiker

New Member
Okay eTech, I see that you have the part and symbol working in LTSpice. But I do not see how you got from A to B (where A is where I am and B is where you are).

Here is what I did to try to create an LTSpice schematic using the same part:
created a new folder called My Test
created the My Test schematic and named the mosfet IPB080N06N
inserted the op command: .inc OptiMOS_60V.lib.txt
copied the files OptiMOS_60V.lib.txt and nmos_Infineon.asy into that folder​

When I run it, the error message says "m1: Can't find the definition of model "ipb080n06n"".

What else do I need to do to make this work and where did nmos_Infineon.asy come from?


Here is the My Test folder folder:
https://www.dropbox.com/s/amm892lsvfxgcgb/My Test.zip?dl=0
 
Last edited:

eTech

Active Member
Okay eTech, I see that you have the part and symbol working in LTSpice. But I do not see how you got from A to B (where A is where I am and B is where you are).

Here is what I did to try to create an LTSpice schematic using the same part:
created a new folder called My Test

Good.

created the My Test schematic and named the mosfet IPB080N06N
Don't use the native mosfet symbol.
Copy the symbol and .txt file I gave you into the folder. Then use the component selector to browse to the folder and select the symbol.
Rht-clk the symbol and set the property "value" to IPB080N06N

inserted the op command: .inc OptiMOS_60V.lib.txt
If placed on the schematic...Good
I usually place the directive on the schematic then rht-clk and browse to the file.
This way I'm sure LTspice will find it.

copied the files OptiMOS_60V.lib.txt and nmos_Infineon.asy into that folder
Bad. correct action, wrong timing :)

When I run it, the error message says "m1: Can't find the definition of model "ipb080n06n"".


What else do I need to do to make this work and where did nmos_Infineon.asy come from?


Here is the My Test folder folder:
https://www.dropbox.com/s/amm892lsvfxgcgb/My Test.zip?dl=0
Follow the above comments. Then it should work.

eT
 

PickyBiker

New Member
eTech......... BINGO, it works! Thankk you.

One last question, I know where the .lib.txt file came from but where did the nmos_Infineon.asy come from?

In any case, thanks so much for the help. It is appreciated.
 

eTech

Active Member
eTech......... BINGO, it works! Thankk you.

One last question, I know where the .lib.txt file came from but where did the nmos_Infineon.asy come from?

In any case, thanks so much for the help. It is appreciated.
I made a custom LTspice symbol based on the Infineon App note AN 2014-02.
 

eTech

Active Member
Okay, thank you. I'll read up on that App note.
Just to clarify how I made the symbol:

1. Place the native nmos symbol on the schematic.
2. ctrl-rht-clk the nmos symbol then click the "open symbol" button.
3. Select "File->Save As" from the menu bar, browse to the new folder, TYPE A NEW SYMBOL FILE NAME, then click "Save".
4. The symbol is now saved with the new symbol file name in the new folder and is currently being edited.
5. Finish modifying the symbol as desired.

Note - Be aware that it is important not to use a symbol name that is already a file name used for a native symbol.
The native symbol will override the new symbol.

Hope that helps...

eT
 

auzer

New Member
On a similar subject, I'd like to use the model of an Infineon BSP752T in LTspice XVII.

Information on the part is below. Is it possible to use this model in LTspice, and if so, I'd appreciate some detailed steps with the process. TIA


The delivery packages contains the following : --
/doc/ : application note detailing how to simulate the model --
/lib/ : the directory containing the encrypted model library file --
/results/ : some simulation screenshots of the testbench delivered --
/symbol/ : symbol files for OrCAD and dummy generation file --
/bsp752t_project-PSpiceFiles/ : OrCAD project files including schematic --
/BSP752t_PROJECT.DSN : OrCAD project configuration file --
/bsp752t_project.opj : OrCAD project load file
 

eTech

Active Member
On a similar subject, I'd like to use the model of an Infineon BSP752T in LTspice XVII.

Information on the part is below. Is it possible to use this model in LTspice, and if so, I'd appreciate some detailed steps with the process. TIA


The delivery packages contains the following : --
/doc/ : application note detailing how to simulate the model --
/lib/ : the directory containing the encrypted model library file --
/results/ : some simulation screenshots of the testbench delivered --
/symbol/ : symbol files for OrCAD and dummy generation file --
/bsp752t_project-PSpiceFiles/ : OrCAD project files including schematic --
/BSP752t_PROJECT.DSN : OrCAD project configuration file --
/bsp752t_project.opj : OrCAD project load file
Hi

Unfortunately, the model file is encrypted for Orcad. So it cant be used in LTspice.
Perhaps you can ask Infineon for an unencrypted pspice file.

eT
 

auzer

New Member
Hi

Unfortunately, the model file is encrypted for Orcad. So it cant be used in LTspice.
Perhaps you can ask Infineon for an unencrypted pspice file.

eT
Thanks. Looks like Infineon have their own flavour of spice with Infineon Designer based on TIs TINA, but it can't use their own models.
 

Latest threads

EE World Online Articles

Loading

 
Top