LTSpice Error Log Unknown Parameter Using Vishay FET Model

Thread Starter

Gipper

Joined May 20, 2021
2
I am hoping an LTSPICE expert can help me with a model.

I downloaded a SPICE model from Vishay's website to test a PFET in a power supply design, specifically Vishay SQJ431EP. The model is attached as "SQJ431EP_HS.TXT".

If I run this in my design, LTSPICE takes much longer than normal and struggles to finish the sim. If it does finish, I am presented with an LTSPICE error log. The log is attached as "ERROR.txt".

I've tried using this model in a fresh simpler design, but I'm still presented with errors.

Any ideas what is causing issues with this model? I'd really like to use this part!
 

Attachments

Papabravo

Joined Feb 24, 2006
16,160
It appear as though you have a model in which the syntax and semantics to define a resistor allows for 3 values after the node name. LTspice does not support this syntax and has no way to know what the two extra numbers are for. It supports one <value> and additional parameters follow a <name>=<value> syntax. Those are the two fatal errors.

R1 D 3 1.864e-01 5.970e-3 1.422e-05
RTCV 100 S 1e6 2.291e-06 -1.331e-05

The non-fatal errors:
In the definition of the diode, the parameter TRS is not defined in LTspice but it is ignored
.MODEL DBD D (
+FC = 0.1 TT = 2.000e-08 TREF = 25 BV = 201
+RS = 4.725e-02 N = 1.187e+00 IS = 7.376e-12
+EG = 1.144e+00 XTI = 2.352e+00 TRS = 2.475e-03
+CJO = 7.806e-11 VJ = 5.826e-01 M = 5.757e-01 )

In the definition of the MOS transistors the parameter CAPOP is not defined in LTspice, but it is ignored.
.MODEL PMOS PMOS ( LEVEL = 3 TOX = 7e-8
+ RS = 0 KP = 7.910e-06 NSUB = 7.45e+16
+ KAPPA = 3.095e-03 NFS = 8.000e+09
+ LD = 0 IS = 0 TPG = -1 CAPOP = 12 )
***************************************************************
.MODEL NMOS NMOS ( LEVEL = 3 TOX = 7e-8
+NSUB = 2.858e+15 IS = 0 TPG = -1 CAPOP = 12 )

You might wan to ask the manufacturer which spice version supports this model

From the LTspice Help pages

R. Resistor
Symbol Names: RES, RES2
Syntax: Rxxx n1 n2 <value> [tc=tc1, tc2, ...] [temp=<value>]
The resistor supplies a simple linear resistance between nodes n1 and n2. A temperature dependence can be defined for each resistor instance with the parameter tc. The resistance, R, at will be
R = R0 * (1. + dt * tc1 + dt**2 * tc2 + dt**3 * tc3 + ...)

where R0 is the resistance at the nominal temperature and dt is the difference between the resistor's temperature and the nominal temperature.

The allowed parameters for a diode and for an NMOS and PMOS transistor are listed in the LTspice Help pages as well.
 

eetech00

Joined Jun 8, 2013
2,364
I am hoping an LTSPICE expert can help me with a model.

I downloaded a SPICE model from Vishay's website to test a PFET in a power supply design, specifically Vishay SQJ431EP. The model is attached as "SQJ431EP_HS.TXT".

If I run this in my design, LTSPICE takes much longer than normal and struggles to finish the sim. If it does finish, I am presented with an LTSPICE error log. The log is attached as "ERROR.txt".

I've tried using this model in a fresh simpler design, but I'm still presented with errors.

Any ideas what is causing issues with this model? I'd really like to use this part!
Errors are generated because you are using the wrong model file.

No errors are generated if you use the PSpice compatible file.

For LTspice, use the PSpice compatible file "SQJ431EP_PS.TXT".
 

Thread Starter

Gipper

Joined May 20, 2021
2
Thank you both for the responses.

I tried the "SQJ431EP_PS.TXT" model, and it now works! I've also learned something now about the syntax. :)
 

Papabravo

Joined Feb 24, 2006
16,160
The total number of Spice variations out there is thankfully small. Over a period of almost 50 years it is actually surprising, that without a standards body to enforce compliance, there is for the most part wide agreement on how to construct and distribute models. I give ON Semiconductor, great credit for having 4 common models for many of the discrete transistors. They are:
  1. Pspice
  2. Spice2
  3. Spice3
  4. Saber
The Pspice models seem to work well with LTspice and that is the one I normally choose.
 
Top