NXP Transistor model PBSS5160PAP does not work

[FdW]

L.s.

Who can help me? From the NXP site I downloaded the files:
PBSS5160PAP :: NXP Semiconductors
and
PBSS4160PANP :: NXP Semiconductors
(click 'all models')

Then I created LTspice 'ASY' and 'SUB' files.
(See attached ZIP-file)

For testing the models I created 'PBSS Test.ASC'
(See attached ZIP-file)

When I run the simulation the error-log reads
/****
Circuit: * C:\Users\FdW\Electronics\Schemas LTspice\Abraxas Bal-Unbal\PBSS Test.asc

Fatal Error: Multiple instances of "Line"
****/

The question is: What is wrong with me or (unlikely ) what is wrong with models?

Regards,
Frans.

 

[FdW]

No one?

 

[ingenieus]

Quite a number of things wrong.

 

[FdW]

Quite a number of things wrong.

But one (me ) would expect that if a model is downloaded from a site like NXL's that the model at the least should work (don't you ). Any idea how to fix these, or should I just forget about it (them (these models)).

 

[ingenieus]

Here is the fixed version. Not much wrong with the models. To get the most out of them, you have to create a symbol with two transistors in it. That's not really needed and I just hacked the subcircuit files down to a single transistor.

The error about lines comes from SPICE trying to interpret the stuff inside the asy file as circuit elements. The asy file contains information on how to draw it. Open it with a text editor to see what I mean.

You don't include the symbol files in a SPICE directive, you add the symbol by pressing F2. Change the Top Directory to the working directory (C:\Users\FdW\Electronics\Schemas LTspice\Abraxas Bal-Unbal\ in your case).

Your circuit did not actually use the symbols that you created. I changed the symbols to include the subcircuit file, so that there is no need to add any SPICE directives for it. Also, the order of the pins were wrong in your symbol file. It has to match the order in the subcircuit file.

 

[spicer2012]

Hi,
you dont have to make changes on the original SPICE-Modelfile from the NXP-Homepage.

You just have to understand how the symbol and modelfile work together.

Every Symbol can work together with just one spcific SPICE-Modelfile. This SPICE-Modelfile can include one to infinitely many SPICE-Modelfiles.

The Symbol of a NPN-Transitor may fix to more than just one SPICE-Modelfile ;-)

Here is the Syntax of a Symbol-File for a NPN-Transistor:

Version 4
SymbolType CELL
LINE Normal 44 76 36 84
LINE Normal 64 96 44 76
LINE Normal 64 96 36 84
LINE Normal 40 80 16 64
LINE Normal 16 80 16 16
LINE Normal 16 32 64 0
LINE Normal 16 48 0 48
WINDOW 0 31 36 Left 2
WINDOW 3 31 60 Left 2
PIN 64 0 NONE 0
PINATTR PinName C
PINATTR SpiceOrder 3
PIN 0 48 NONE 0
PINATTR PinName B
PINATTR SpiceOrder 2
PIN 64 96 NONE 0
PINATTR PinName E
PINATTR SpiceOrder 1
WINDOW 38 84 60 Left 0
SYMATTR SpiceModel PBSS4160PANP_NPN
SYMATTR Prefix X
SYMATTR Description Bipolar NPN transistor PBSS4160PAN
SYMATTR ModelFile PBSS4160PANP_ORIGINAL_FROM_NXP.SUB

SYMATTR Prefix: The Prefix "X" must be used for subcircuits.
SYMATTR ModelFile: Here we need the path to the SPICE-Modelfile
SYMATTR SpiceModel: Here you choose the exakt name of the Subcircuit out of the choosen SPICE-Modelfile.

There are more than one strategies to expand your collection of downloaded SPICE-Modelfiles.

Here is a "small entrepreneur solution":
Put the *.asc, *.asy and *.sub(could also have a suffix like *.lib - it doesnt matter) in the same folder. Then your workingpath is automatical detected by LTSpice and you dont need to handle with path-names.

Create a npn.sub file which contains all your NPN Transistors as an Subckt. If you have a SPICE-Model without a Subcircuit, create one out of it... like:


before:

.MODEL Transistor_without_subcircuit NPN
+ IS = 8.732E-014
+ NF = 0.9718
+ ISE = 4.178E-015
+ NE = 1.387
+ BF = 433
.
.
.

after:

[COLOR=red].SUBCKT Transistor_without_subcircuit 1 2 3
*
Q1 1 2 3 Transistor_without_subcircuit[/COLOR]
*
.MODEL Transistor_without_subcircuit NPN
+ IS = 8.732E-014
+ NF = 0.9718
+ ISE = 4.178E-015
+ NE = 1.387
+ BF = 433
.
.
.
 
[COLOR=red].ENDS[/COLOR]

If you you need a NPN Transistor in your LTSpice-Circuit, you klick "component" and choose the NPN-Symbol you created. Place your Transitor. Now you have the ability to switch between all Transistore in your *.sub file. Right-Click to your Transistor in yout LTSpice Schematic, then left-doubbleclick to "SpiceModel" to activate the dropdownmenu. Now you can see all Transistors in your *.sub and are able to choose an other.





In case of the NXP-Model you have a NPN and PNP in the same *.SUB. For a "clean" NPN/PNP Library, you need to cut this Model in two pieces.

 

[spicer2012]

here is an example how to switch between different transistors ....

 

[FdW]

Here is the fixed version. Not much wrong with the models. To get the most out of them, you have to create a symbol with two transistors in it. That's not really needed and I just hacked the subcircuit files down to a single transistor.

The error about lines comes from SPICE trying to interpret the stuff inside the asy file as circuit elements. The asy file contains information on how to draw it. Open it with a text editor to see what I mean.

You don't include the symbol files in a SPICE directive, you add the symbol by pressing F2. Change the Top Directory to the working directory (C:\Users\FdW\Electronics\Schemas LTspice\Abraxas Bal-Unbal\ in your case).

Your circuit did not actually use the symbols that you created. I changed the symbols to include the subcircuit file, so that there is no need to add any SPICE directives for it. Also, the order of the pins were wrong in your symbol file. It has to match the order in the subcircuit file.

Thanks

 

[FdW]

here is an example how to switch between different transistors ....

Thank you