• 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.

Pspice to LTspice igbt model

Thread starter #1
Hello everyone!

I got a problem and i would be very pleased if anyone could help me.

I downloaded this model of an IGBT (IXGT32N170A) on IXYS website, the .zip file comes with a .olb and .lib files.

However, i wanted to input this model in my ltspice simulation.

Does anyone have any tip?
 

Attachments

#2
*******************************************
6th Sept 2016: LTspice XVII has an NIGBT and an PIGBT model. Download this version of LTspice from linear.com

Select the new component icon (the AND gate symbol in the toolbar), then go to the MISC directory. They are in there

*******************************************


Follow my LTSpice tutorial:
http://www.simonbramble.co.uk/lt_spice/ltspice_lt_spice.htm

You need tutorial number 3: importing 3rd party models

Use the .lib file and import this into LTS. You can rename the .lib file to a .txt file if it makes it easier. it is just text

The 2 files you mention are PSPICE compatible, so you should be able to use them with LTSpice
 
Last edited:
#3
Hello,

I'm getting the same problem to connect that IXYS IGBT.
Its lib file looks like this (so without pins input):

.MODEL IXGT32N170A NIGBT
+ TAU=63.552E-9
+ KP=14.397
+ AREA=16.000E-6
+ AGD=6.4000E-6
+ WB=117.00E-6
+ VT=5.3804
+ MUN=1.0000E6
+ MUP=150
+ BVF=9.9990
+ KF=.5005
+ CGS=38.737E-9
+ COXD=88.530E-9
+ VTD=-5

I've tried almost everything and still get the same error message "Unknown subcircuit called in: xu1 n001 n004 ixgt32n170a".
Does anyone know how to solve that problem.

Thanks in advance
bob
 

alec_t

Well-Known Member
Most Helpful Member
#4
What directive do you have on the schematic? Which folder is the .lib file in?
 
#5
I wrote the directive .include IXGT32N170A.lib on my schematic.
And my lib is saved under .LTspiceIV/lib/sub as it should be.
I draw an IGBT model (IXGT32N170A.asy) and save it in .LTspiceIV/lib/sym
I think to have done everything right yet, just suprise that it doesn't work.

Any other clue

thanks
 
Last edited:
#10
ok, I replace prefix: X with --> MN
and got a new message error: m1: can't find definition of model "ixgt32n170a" :(
 
Last edited:
#11
How can I include the .subckt command on this model?

.MODEL IXGT32N170A NIGBT
+ TAU=63.552E-9
+ KP=14.397
+ AREA=16.000E-6
+ AGD=6.4000E-6
+ WB=117.00E-6
+ VT=5.3804
+ MUN=1.0000E6
+ MUP=150
+ BVF=9.9990
+ KF=.5005
+ CGS=38.737E-9
+ COXD=88.530E-9
+ VTD=-5
 
#13
OK here goes... If you use a suffix 'M' LTSpice expects a whole load of mosfet related parameters to follow. Likewise with a transistor, it expects transistor characteristics to follow. If you use the suffix X, it expects a subcircuit made up of simpler .model statements. You dont have any of this. In fact it looks at first glance that you have a bunch of parameter specific to an IGBT. If LTSpice does not recognise these, no amount of trickery will overcome this. Looking at other posts, I have seen people making their own models using a MOSFET on the front end and a transistor on the back end. This is the only compromise I can offer. If i hear of any other way of doing this, I will let you know
 
#14
I've cracked it. Please find attached the circuit IGBT.asc. Save this to a directory of your choice. IN THE SAME DIRECTORY, save the attached file IGBT.txt. You should be able to run the circuit.

I got the file from the Fairchild website, so it seems that if you want to simulate IGBTs, look at the Fairchild parts

For future reference:

Open IGBT.txt (the model file) in LTSpice. Navigate to the line starting .subckt. Right Click over this line and select Create Symbol. This will create a block according to the subckt model.

Create a new simulation file. Click on the AND gate symbol to select a new symbol. In the root component directory, go to [AutoGenerated]. In there will be the symbol you have just created. Add the line .include IGBT.txt (or whatever your file is called). Make sure the filename EXACTLY matches the file called up in the .include statement.

Just as a check, do CTRL Right Click over the IGBT symbol and make sure that the name in the Value field is IDENTICAL to the name directly after the .subckt directive in your Spice model (in my case it is FGA180N33ATD).

This should then work.

Importing third party spice models is detailed in my LTSpice tutorial:
http://www.simonbramble.co.uk/lt_spice/ltspice_lt_spice.htm
 

Attachments

#15
What about if I want to simulate the IXYS model IXGT32N170A?
How to get the .subckt inputs on it?

.MODEL IXGT32N170A NIGBT
+ TAU=63.552E-9
+ KP=14.397
+ AREA=16.000E-6
+ AGD=6.4000E-6
+ WB=117.00E-6
+ VT=5.3804
+ MUN=1.0000E6
+ MUP=150
+ BVF=9.9990
+ KF=.5005
+ CGS=38.737E-9
+ COXD=88.530E-9
+ VTD=-5
 
Last edited:
#16
You can't (at least not that I know). The .MODEL statement tells LTSpice to model a specific 'simple' component, such as a transistor, resistor, diode etc. At the end of every .model statement line is a D (for diode), NMOS for an N channel FET etc. Your model has a NIGBT at the end which is a component not recognised by LTSpice. The only way around this is to use a dedicated .subckt statement and Fairchild appears to do this.

A .subckt statement tells LTSpice to look for a subcircuit made up of several simpler .model statements. Thus you can build one component made up of lots of smaller simpler (.model) components (like an op amp). Looking at the Fairchild model, it looks like they have build the subcircuit around an NMOS front end with an npn back end.

You might want to post something on the Yahoo LTSpice user group to see what they come up with. Failing that, get the datasheet of the Fairchild part next to teh datasheet of your part and modify the Fairchild model accordingly
 
#19
I got another model from IXYS which include .subckt input (see attach).
I'm getting another error message: <can't find definition of model "32N170A">
 
Last edited:
#20
follow my pages on importing 3rd party spice models. You want tutorial number 4:

http://www.simonbramble.co.uk/lt_spice/ltspice_lt_spice.htm

Have you made the filename in the include statement exactly the same as the filename of your model?
Have you saved the model in the same directory as the simulation file?
is the component in your circuit called IXGT32N170A ?
Have you labeled your component prefix as X?
Please include your circuit and I will have a look at it

Still not heard back from IXYS yet

Simon
 

Latest threads

EE World Online Articles

Loading

 
Top